This document helps you to understand how to create, manage, and execute subprograms and macros in SINUMERIK-controlled machines. It includes commands for file handling, motion commands, protection zones, and synchronization actions essential for complex machining tasks.
Category
Business
SINUMERIK 840D 840Di 810D Advanced Programming Guide - ITSCNC
Programming Guide 11/2002 Edition
Advanced
SINUMERIK 840D/840Di/810D
Flexible NC 1
Programming
Subprograms, Macros 2
File and Program 3
Management
SINUMERIK 840D/840Di/810D Protection Zones 4
Advanced Special Motion 5
Commands
Frames 6
Programming Guide
Transformations 7
Tool Offsets 8
Path Traversing 9
Behavior
Motion-Synchronous 10
Action
Oscillation
Valid for 11
Control Software Version
SINUMERIK 840D 6 Punching and Nibbling
SINUMERIK 840DE (export version) 6 12
SINUMERIK 840D powerline 6
SINUMERIK 840DE powerline 6
SINUMERIK 840Di 2 Additional Functions
SINUMERIK 840DiE (export version) 2 13
SINUMERIK 810D 3
SINUMERIK 810DE (export version) 3
SINUMERIK 810D powerline 6 User Stock Removal
SINUMERIK 810DE powerline 6 14Programs
Tables 15
11.02 Edition
Appendix A
SINUMERIK® Documentation
Printing history
Brief details of this edition and previous editions are listed below.
The status of each edition is shown by the code in the "Remarks" column.
Status code in the "Remarks" column:
A .... New documentation.
B .... Unrevised reprint with new Order No.
C .... Revised edition with new status.
If factual changes have been made on the page since the last edition, this is indicated by a
new edition coding in the header of that page.
Edition Order No. Comment
02.95 6FC5298-2AB00-0BP0 A
04.95 6FC5298-2AB00-0BP1 C
12.95 6FC5298-3AB10-0BP0 C
03.96 6FC5298-3AB10-0BP1 C
08.97 6FC5298-4AB10-0BP0 C
12.97 6FC5298-4AB10-0BP1 C
12.98 6FC5298-5AB10-0BP0 C
08.99 6FC5298-5AB10-0BP1 C
04.00 6FC5298-5AB10-0BP2 C
10.00 6FC5298-6AB10-0BP0 C
09.01 6FC5298-6AB10-0BP1 C
11.02 6FC5298-6AB10-0BP2 C
This manual is included in the documentation on CD-ROM (DOCONCD)
Edition Order No. Comment
11.02 6FC5298-6CA00-0BG2 C
Trademarks
SIMATIC, SIMATIC HMI, SIMATIC NET, SIROTEC, SINUMERIK and SIMODRIVE are registered
trademarks of Siemens AG. The other designations in this publication may also be trademarks, the use of
which by third parties may constitute copyright violation.
Further information is available on the Internet under: Other functions not described in this documentation might be executable in the
http://www.ad.siemens.de/sinumerik control. This does not, however, represent an obligation to supply such functions
with a new control or when servicing.
This publication was produced with WinWord V8.0 We have checked that the contents of this documentation correspond to the
and Designer V7.0. hardware and software described. Nonetheless, differences might exist and we
The reproduction, transmission or use of this document or its contents is not cannot therefore guarantee that they are completely identical. The information
permitted without express written authority. Offenders will be liable for damages. contained in this document is, however, reviewed regularly and any necessary
All rights, including rights created by patent grant or registration of a utility model changes will be included in the next edition. We welcome suggestions for
or design, are reserved. improvement.
© Siemens AG, 1995–2001. All rights reserved Subject to change without prior notice.
Order No. 6FC5298-6AB10-0BP2 Siemens Aktiengesellschaft
Printed in Germany
0 11.02 Contents 0
Contents
Preface 0-14
Flexible NC Programming 1-25
1.1 Variable and arithmetic parameters ................................................................................ 1-26
1.2 Variable definition............................................................................................................ 1-29
1.3 Array definition ................................................................................................................ 1-34
1.4 Indirect programming ...................................................................................................... 1-40
1.5 Assignments.................................................................................................................... 1-45
1.6 Arithmetic operations and functions ................................................................................ 1-46
1.7 Comparison and logic operators ..................................................................................... 1-48
1.8 Priority of operators ......................................................................................................... 1-53
1.9 Possible type conversions............................................................................................... 1-54
1.10 String operations ............................................................................................................. 1-55
1.10.1 Type conversion....................................................................................................... 1-56
1.10.2 Concatenation of strings .......................................................................................... 1-58
1.10.3 Conversion to lower/upper case .............................................................................. 1-59
1.10.4 Length of the string .................................................................................................. 1-60
1.10.5 Search for character/string in a string...................................................................... 1-60
1.10.6 Selection of a substring............................................................................................ 1-62
1.10.7 Selection of a single character................................................................................. 1-63
1.11 CASE instruction ............................................................................................................. 1-65
1.12 Control structures............................................................................................................ 1-67
1.13 Program coordination...................................................................................................... 1-72
1.14 Interrupt routine ............................................................................................................... 1-77
1.15 Axis transfer, spindle transfer.......................................................................................... 1-85
1.16 NEWCONF: Setting machine data active (SW 4.3 and higher)...................................... 1-90
1.17 WRITE: Write file (SW 4.3 and higher) ........................................................................... 1-91
1.18 DELETE: Delete file (SW 4.3 and higher) ....................................................................... 1-93
1.19 READ: Read lines in file (SW 5.2 and higher)................................................................. 1-94
1.20 ISFILE: File available in user memory NCK (SW 5.2 and higher)................................... 1-97
1.21 CHECKSUM: Creation of a checksum over an array (SW 5.2 and higher) .................... 1-98
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-5
0 Contents 11.02 0
Subprograms, Macros 2-101
2.1 Using subprograms .......................................................................................................2-102
2.2 Subprogram with SAVE mechanism .............................................................................2-104
2.3 Subprograms with parameter transfer...........................................................................2-105
2.4 Calling subprograms: L or EXTERN..............................................................................2-109
2.5 Parameterizable subprogram return (SW 6.4 and higher) ............................................2-113
2.6 Subprogram with program repetition: P.........................................................................2-117
2.7 Modal subprogram: MCALL...........................................................................................2-118
2.8 Calling the subprogram indirectly: CALL .......................................................................2-119
2.9 Repeating program sections with indirect programming (SW 6.4 and higher)..............2-120
2.10 Calling up a program in ISO language indirectly: ISOCALL ..........................................2-121
2.11 Calling subprogram with path specification and parameters PCALL ............................2-122
2.12 Extending a search path for subprogram calls with CALLPATH (SW 6.4 and higher) 2-123
2.13 Suppress current block display: DISPLOF ....................................................................2-125
2.14 Single block suppression: SBLOF, SBLON (SW 4.3 and higher) .................................2-126
2.15 Executing external subprogram: EXTCALL (SW 4.2 and higher) .................................2-132
2.16 Subprogram call with M/T function ...............................................................................2-136
2.17 Cycles: Setting parameters for user cycles ..................................................................2-138
2.18 Macros. DEFINE...AS...................................................................................................2-142
File and Program Management 3-145
3.1 Overview........................................................................................................................3-146
3.2 Program memory...........................................................................................................3-147
3.3 User memory.................................................................................................................3-153
3.4 Defining user data .........................................................................................................3-156
3.5 Defining protection levels for user data (GUD)..............................................................3-160
3.6 Automatic activation of GUDs and MACs (SW 4.4 and higher) ....................................3-162
3.7 Data-specific protection level change for machine and setting data .............................3-164
3.7.1 Change...................................................................................................................3-164
3.7.2 Undoing a change ..................................................................................................3-165
3.8 Changing attributes of NC language elements (SW 6.4 and higher) ............................3-165
3.9 Structuring instruction SEFORM in the Step editor (SW 6.4 and higher)......................3-173
© Siemens AG, 2002. All rights reserved
0-6 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 Contents 0
Protection Zones 4-175
4.1 Defining the protection zones CPROTDEF, NPROTDEF............................................ 4-176
4.2 Activating/deactivating protection zones: CPROT, NPROT......................................... 4-180
Special Motion Commands 5-185
5.1 Approaching coded positions, CAC, CIC, CDC, CACP, CACN .................................... 5-186
5.2 Spline interpolation........................................................................................................ 5-187
5.3 Compressor COMPON/COMPCURV/COMPCAD (SW 6.2) ........................................ 5-196
5.4 Polynomial interpolation – POLY, POLYPATH (SW 5 and higher) ............................... 5-204
5.5 Settable path reference, SPATH, UPATH (SW 4.3 and higher) ................................... 5-211
5.6 Measurements with touch trigger probe, MEAS, MEAW .............................................. 5-215
5.7 Extended measuring function MEASA, MEAWA, MEAC (SW 4 and higher, option).... 5-218
5.8 Special functions for OEM users................................................................................... 5-228
5.9 Programmable motion end criterion (SW 5.1 and higher) ............................................ 5-229
5.10 Programmable servo parameter block (SW 5.1 and higher) ........................................ 5-232
Frames 6-235
6.1 Coordinate transformation via frame variables ............................................................ 6-236
6.2 Frame variables/assigning values to frames................................................................ 6-241
6.3 Coarse/fine offset ......................................................................................................... 6-248
6.4 DRF offset .................................................................................................................... 6-249
6.5 External zero offset ...................................................................................................... 6-250
6.6 Programming PRESET offset, PRESETON ................................................................ 6-251
6.7 Deactivating frames ..................................................................................................... 6-252
6.8 Frame calculation from three measuring points in the area: MEAFRAME .................. 6-253
6.9 NCU-global frames (SW 5 and higher) ........................................................................ 6-256
6.9.1 Channel-specific frames ........................................................................................ 6-257
6.9.2 Frames active in the channel ................................................................................. 6-259
Transformations 7-265
7.1 Three, four and five axis transformation: TRAORI....................................................... 7-266
7.1.1 Programming tool orientation................................................................................ 7-269
7.1.2 Orientation axes reference – ORIWCS, ORIMCS ................................................. 7-274
7.1.3 Singular positions and how to handle them ........................................................... 7-275
7.1.4 Orientation axes (SW 5.2 and higher) ................................................................... 7-276
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-7
0 Contents 11.02 0
7.1.5 Cartesian PTP travel (from SW 5.2) ......................................................................7-279
7.1.6 Online tool length compensation (SW 6.4 and higher) ..........................................7-284
7.2 Milling turned parts: TRANSMIT...................................................................................7-287
7.3 Cylinder surface transformation: TRACYL ...................................................................7-290
7.4 Inclined axis: TRAANG.................................................................................................7-296
7.4.1 Inclined axis programming: G05, G07 (SW 5.3 and higher) ..................................7-300
7.5 Constraints when selecting a transformation ...............................................................7-302
7.6 Deselect transformation: TRAFOOF ............................................................................7-304
7.7 Chained transformations ..............................................................................................7-305
7.8 Switchable geometry axes, GEOAX.............................................................................7-308
Tool Offsets 8-313
8.1 Offset memory..............................................................................................................8-314
8.2 Language commands for tool management.................................................................8-316
8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF.................................8-319
8.4 Maintain tool radius compensation at constant level, CUTCONON
(SW 4 and higher) ........................................................................................................8-325
8.5 Activate 3D tool offsets.................................................................................................8-328
8.6 Tool orientation.............................................................................................................8-336
8.7 Free assignment of D numbers, cutting edge number CE (SW 5 and higher).............8-341
8.7.1 Check D numbers (CHKDNO) ...............................................................................8-342
8.7.2 Renaming D numbers (GETDNO, SETDNO) ........................................................8-343
8.7.3 T numbers for the specified D number (GETACTTD) ...........................................8-344
8.7.4 Set final D numbers to invalid ................................................................................8-345
8.8 Toolholder kinematics ..................................................................................................8-346
Path Traversing Behavior 9-351
9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL ........................................9-352
9.2 Coupled motion TRAILON, TRAILOF ..........................................................................9-358
9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV,
CTABSSV, CTABSEV ..................................................................................................9-362
9.4 Axial leading value coupling, LEADON, LEADOF ........................................................9-375
9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO.........................................................9-381
9.6 Program run with preprocessing memory, STARTFIFO, STOPFIFO, STOPRE .........9-386
9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH..........................9-388
© Siemens AG, 2002. All rights reserved
0-8 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 Contents 0
Motion-Synchronous Action 10-393
10.1 Structure, basic information ....................................................................................... 10-395
10.1.1 Programming and command elements................................................................ 10-397
10.1.2 Validity range: Identification number ID ............................................................... 10-398
10.1.3 Vocabulary word .................................................................................................. 10-399
10.1.4 Actions ................................................................................................................. 10-402
10.1.5 Overview of synchronized actions........................................................................ 10-404
10.2 Basic modules for conditions and actions .................................................................. 10-406
10.3 Special real-time variables for synchronized actions ................................................. 10-409
10.3.1 Flags/counters $AC_MARKER[n] ........................................................................ 10-409
10.3.2 Timer variable $AC_TIMER[n], SW 4 and higher ................................................ 10-409
10.3.3 Synchronized action parameters $AC_PARAM[n]............................................... 10-410
10.3.4 Access to R parameters $Rxx ............................................................................. 10-411
10.3.5 Machine and setting data read/write (SW 4 and higher)...................................... 10-412
10.3.6 FIFO variable $AC_FIFO1[n] … $AC_FIFO10[n] (SW 4 and higher).................. 10-413
10.4 Actions within synchronized actions ........................................................................... 10-415
10.4.1 Auxiliary functions output ..................................................................................... 10-415
10.4.2 Set read-in disable RDISABLE ............................................................................ 10-416
10.4.3 Cancel preprocessing stop STOPREOF ............................................................. 10-417
10.4.4 Deletion of distance-to-go .................................................................................... 10-418
10.4.5 Delete distance-to-go with preparation, DELDTG, DELDTG ("Axis 1 to x") ........ 10-418
10.4.6 Polynomial definition, FCTDEF, block-synchronized ........................................... 10-420
10.4.7 Laser power control ............................................................................................. 10-422
10.4.8 Evaluation function SYNFCT ............................................................................... 10-423
10.4.9 Adaptive control (additive).................................................................................... 10-424
10.4.10 Adaptive control (multiplicative) ........................................................................... 10-425
10.4.11 Clearance control with limited compensation....................................................... 10-426
10.4.12 Online tool offset FTOC ....................................................................................... 10-428
10.4.13 Positioning movements........................................................................................ 10-430
10.4.14 Position axis POS ................................................................................................ 10-432
10.4.15 Start/stop axis MOV............................................................................................. 10-432
10.4.16 Axial feed FA........................................................................................................ 10-433
10.4.17 SW limit switch..................................................................................................... 10-434
10.4.18 Axis coordination.................................................................................................. 10-434
10.4.19 Set actual value.................................................................................................... 10-436
10.4.20 Spindle motions ................................................................................................... 10-437
10.4.21 Coupled-axis motion TRAILON, TRAILOF .......................................................... 10-438
10.4.22 Leading value coupling LEADON, LEADOF ........................................................ 10-439
10.4.23 Measurement ....................................................................................................... 10-441
10.4.24 Set/clear wait marks: SETM, CLEARM (SW 5.2 and higher) .............................. 10-441
10.4.25 Error responses ................................................................................................... 10-442
10.4.26 Travel to fixed stop FXS and FOCON/FOCOF.................................................... 10-442
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-9
0 Contents 11.02 0
10.5 Technology cycles ......................................................................................................10-445
10.5.1 Lock, unlock, reset: LOCK, UNLOCK, RESET ....................................................10-447
10.6 Cancel synchronized action: CANCEL .......................................................................10-449
10.7 Supplementary conditions ..........................................................................................10-450
Oscillation 11-455
11.1 Asynchronous oscillation ............................................................................................11-456
11.2 Oscillation controlled via synchronous actions ...........................................................11-463
Punching and Nibbling 12-475
12.1 Activation, deactivation ...............................................................................................12-476
12.1.1 Language commands...........................................................................................12-476
12.1.2 Use of M commands ............................................................................................12-479
12.2 Automatic path segmentation.....................................................................................12-480
12.2.1 Path segmentation for path axes .........................................................................12-481
12.2.2 Path segmentation for single axes .......................................................................12-482
12.2.3 Programming examples .......................................................................................12-484
Additional Functions 13-487
13.1 Axis functions AXNAME, SPI, ISAXIS, AXSTRING (SW 6 and higher).....................13-489
13.2 Function call ISVAR ( ) (SW 6.3 and higher)..............................................................13-491
13.3 Learn compensation characteristics: QECLRNON, QECLRNOF ..............................13-493
13.4 Synchronized spindle..................................................................................................13-495
13.5 EG: Electronic gear (SW 5 and higher) ......................................................................13-505
13.5.1 Define electronic gear: EGDEF............................................................................13-505
13.5.2 Activate electronic gear ........................................................................................13-506
13.5.3 Deactivate electronic gear....................................................................................13-510
13.5.4 Delete definition of an electronic gear..................................................................13-511
13.5.5 Revolutional feedrate (G95)/electronic gear (SW 5.2) .........................................13-511
13.5.6 Response of EG at Power ON, RESET, mode change, block search.................13-512
13.5.7 The electronic gear's system variables ................................................................13-512
13.6 Extended stopping and retract (SW 5 and higher) .....................................................13-513
13.6.1 Drive-independent reactions ................................................................................13-514
13.6.2 NC-controlled reactions........................................................................................13-515
13.6.3 Possible trigger sources.......................................................................................13-518
13.6.4 Logic gating functions: Source/reaction operation ...............................................13-518
13.6.5 Activation..............................................................................................................13-519
13.6.6 Generator operation/DC link backup....................................................................13-519
13.6.7 Drive-independent stop ........................................................................................13-520
© Siemens AG, 2002. All rights reserved
0-10 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 Contents 0
13.6.8 Drive-independent retract .................................................................................... 13-521
13.6.9 Example: Using the drive-independent reaction .................................................. 13-521
13.7 Link communication (SW 5.2 and higher) .................................................................. 13-522
13.8 Axis container (SW 5.2 and higher) ........................................................................... 13-526
13.9 Program execution time/Workpiece counter (SW 5.2 and higher) ............................ 13-528
13.9.1 Program runtime .................................................................................................. 13-528
13.9.2 Workpiece counter............................................................................................... 13-530
13.10 Interactive window call from parts program, command MMC
(SW 4.4 and higher) ................................................................................................... 13-532
13.11 Influencing the motion control .................................................................................... 13-534
13.11.1 Percentage jerk correction: JERKLIM.................................................................. 13-534
13.11.2 Percentage velocity correction: VELOLIM ........................................................... 13-535
13.12 Master/slave grouping ................................................................................................ 13-536
User Stock Removal Programs 14-541
14.1 Supporting functions for stock removal ...................................................................... 14-542
14.2 Contour preparation: CONTPRON............................................................................. 14-543
14.3 Contour decoding: CONTDCON (SW 5.2 and higher)............................................... 14-550
14.4 Intersection of two contour elements: INTERSEC ..................................................... 14-554
14.5 Traversing a contour element from the table: EXECTAB .......................................... 14-556
14.6 Calculate circle data: CALCDAT ................................................................................ 14-557
Tables 15-559
15.1 List of instructions....................................................................................................... 15-561
15.2 List of system variables .............................................................................................. 15-591
15.2.1 R parameters ....................................................................................................... 15-591
15.2.2 Channel-specific synchronized action variables .................................................. 15-591
15.2.3 Frames 1.............................................................................................................. 15-592
15.2.4 Toolholder data .................................................................................................... 15-593
15.2.5 Channel-specific protection zones ....................................................................... 15-601
15.2.6 Tool parameters................................................................................................... 15-603
15.2.7 Cutting edge data OEM user ............................................................................... 15-609
15.2.8 Monitoring data for tool management .................................................................. 15-617
15.2.9 Monitoring data for OEM users ............................................................................ 15-618
15.2.10 Tool-related data.................................................................................................. 15-619
15.2.11 Tool-related grinding data .................................................................................... 15-621
15.2.12 Magazine location data ........................................................................................ 15-622
15.2.13 Magazine location data for OEM users................................................................ 15-623
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-11
0 Contents 11.02 0
15.2.14 Magazine description data for tool management .................................................15-624
15.2.15 Tool management magazine description data for OEM users.............................15-625
15.2.16 Magazine module parameter ...............................................................................15-626
15.2.17 Adapter data.........................................................................................................15-626
15.2.18 Measuring system compensation values .............................................................15-626
15.2.19 Quadrant error compensation ..............................................................................15-627
15.2.20 Interpolatory compensation..................................................................................15-629
15.2.21 NCK-specific protection zones .............................................................................15-630
15.2.22 Cycle parameterization.........................................................................................15-631
15.2.23 System data .........................................................................................................15-636
15.2.24 Frames 2 ..............................................................................................................15-636
15.2.25 Tool data ..............................................................................................................15-638
15.2.26 Magazines ............................................................................................................15-643
15.2.27 Programmed geometry axis values......................................................................15-646
15.2.28 G groups ..............................................................................................................15-647
15.2.29 Programmed values .............................................................................................15-647
15.2.30 Channel states .....................................................................................................15-651
15.2.31 Synchronized actions ...........................................................................................15-656
15.2.32 I/Os.......................................................................................................................15-657
15.2.33 Reading and writing PLC variables ......................................................................15-657
15.2.34 NCU link ...............................................................................................................15-658
15.2.35 Direct PLC I/O ......................................................................................................15-658
15.2.36 Tool management ................................................................................................15-659
15.2.37 Timers ..................................................................................................................15-662
15.2.38 Path movement ....................................................................................................15-663
15.2.39 Speeds/accelerations...........................................................................................15-665
15.2.40 Spindles................................................................................................................15-667
15.2.41 Polynomial values for synchronized actions.........................................................15-670
15.2.42 Channel states .....................................................................................................15-672
15.2.43 Measurement .......................................................................................................15-673
15.2.44 Positions...............................................................................................................15-677
15.2.45 Indexing axes .......................................................................................................15-679
15.2.46 Encoder values.....................................................................................................15-679
15.2.47 Axial measurement ..............................................................................................15-680
15.2.48 Offsets..................................................................................................................15-681
15.2.49 Axial paths............................................................................................................15-684
15.2.50 Oscillation.............................................................................................................15-685
15.2.51 Axial velocities......................................................................................................15-685
15.2.52 Drive data .............................................................................................................15-687
15.2.53 Axis statuses ........................................................................................................15-688
15.2.54 Master/slave links.................................................................................................15-689
15.2.55 Travel to fixed stop...............................................................................................15-690
15.2.56 Electronic gear .....................................................................................................15-691
15.2.57 Leading value coupling.........................................................................................15-692
© Siemens AG, 2002. All rights reserved
0-12 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 Contents 0
15.2.58 Synchronized spindle ........................................................................................... 15-693
15.2.59 Safety Integrated.................................................................................................. 15-696
Appendix A-701
A Index .................................................................................................................................A-702
B Commands, Identifiers......................................................................................................A-719
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-13
0 Preface 11.02Structure of documentation 0
Preface
Overview of documentation
The SINUMERIK documentation is organized in three
parts:
• General Documentation
• User Documentation
• Manufacturer/Service Documentation
Target group
This documentation is intended for the programmer.
It provides detailed information for programming the
SINUMERIK 840D/840Di/840Di/810D.
Standard scope
The Programming Guide describes the functionality
included in the standard scope. Extensions or changes
made by the machine tool manufacturer are
documented by the machine tool manufacturer.
You can obtain more detailed information on
publications about SINUMERIK 840D/840Di/810D or
publications that apply to all the SINUMERIK controls
(e.g. universal interface, measurement cycles, etc.),
from your Siemens branch.
Other functions not described in this documentation
might be executable in the control. This does not,
however, represent an obligation to supply such
functions with a new control or when servicing.
© Siemens AG, 2002. All rights reserved
0-14 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 PrefaceStructure of documentation 0
Validity
This Programming Guide is valid for the following
controls:
SINUMERIK 840D SW6
SINUMERIK 840DE (export version) SW6
SINUMERIK 840Di SW2
SINUMERIK 840DiE (export version) SW2
SINUMERIK 810D SW3
SINUMERIK 810DE (export version) SW3
with operator panel fronts OP 010, OP 010C, OP 010S,
OP 12 or OP 15 (PCU 20 or PCU 50)
SINUMERIK 840D powerline
From 09.2001, the
• SINUMERIK 840D powerline and the
• SINUMERIK 840DE powerline
will be available with improved performance. A list of the
available powerline modules can be found in the
Hardware Reference Manual
/PHD/ in Section 1.1
SINUMERIK 810D powerline
From 12.2001, the
• SINUMERIK 810D powerline and the
• SINUMERIK 810DE powerline
will be available with improved performance. A list of the
available powerline modules can be found in the
Hardware Reference Manual
/PHC/ in Section 1.1
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-15
0 Preface 11.02Structure of documentation 0
Hotline Should you have any questions, please consult the following Hotline:
A&D Technical Support Tel.: ++49-(0)180-5050-222
Fax: ++49-(0)180-5050-223
E-mail: [email protected]
If you have any questions about the documentation (suggestions,
corrections) please send a fax to the following fax address, or e-mail
us:
Fax: ++49-(0)0131-98-2176
E-mail: [email protected]
Fax form: see the feedback page at the back of this document.
Internet address http://www.ad.siemens.de/sinumerik
Export version
The following functions are not available in the export
version:
Function 810DE 840DE
Machining package for 5 axes − −
Transformation package handling (5 axes) − −
Multiple axes interpolation (> 4 axes) − −
Helix interpolation 2D+6 − −
Synchronized actions stage 2 − O1)
Measurement stage 2 − O1)
Adaptive control O1) O1)
Continuous dressing O1) O1)
Use of the compile cycles (OEM) − −
Multidimensional sag compensation O1) O1)
− Function not available
1) Limited functionality
© Siemens AG, 2002. All rights reserved
0-16 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 PrefaceStructure of documentation 0
Structure of the descriptions
All cycles and programming options have been
described – where appropriate and possible – according
to the same internal structure. The organization into
different information levels allows you to find the
information you need quickly.
1. At a glance
Drilling cycles and drilling patterns 03.96
2 2.1 Drilling cycles 2
If you want to look up a seldom used command or the
meaning of a parameter, you can see at a glance how
2.1.2 Drilling, centering – CYCLE81
to program the function together with an explanation of Programming
CYCLE81 (RTP, RFP, SDIS, DP)
the commands and parameters.
RTP real Retraction plane (absolute)
RFP real Reference plane (absolute)
SDIS real Safety clearance (enter without sign)
DP real Final drilling depth (absolute)
DPR real Final drilling depth relative to reference plane (enter without sign)
This information is always presented at the start of the
page. Function Z
The tool drills at the programmed spindle speed and
feedrate to the programmed final drilling depth.
Note:
X
To keep this documentation as compact as possible,
it is not always possible to list all the types of
representation available in the programming
Operating sequence
language for the individual commands and Position reached before the beginning of thecycle:
The drilling position is the position in the two axes of
parameters. The commands are therefore always the selected plane.
The cycle implements the following motion
programmed in the context most frequently used in sequence:• Approach of the reference plane brought forward
by the safety clearance with G0
the workshop. • Travel to the final drilling depth at the feedrate
programmed in the calling program (G1)
• Retraction to retraction plane with G0
Siemens AG 1997 All rights reserved.
2-36 SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-17
0 Preface 11.02Structure of documentation 0
2. Detailed explanations
03.96 Drilling cycles and drilling patterns
2 2.1 Drilling cycles 2
The theory part contains detailed information on the
following:
Explanation of parameters
Z
G1
RFP and RTP
G0
Generally, the reference plane (RFP) and the
What is the purpose of the command? retraction plane (RTP) have different values. In the
cycle it is assumed that the retraction plane lies in
front of the reference plane. The distance between RTP
the retraction plane and the final drilling depth is RFP+SDIS
therefore greater than the distance between the RFPX
reference plane and the final drilling depth.
What is the effect of the command?
SDIS
The safety clearance (SDIS) refers to the reference
DP=RFP-DPR
plane. which is brought forward by the safety
clearance. The direction in which the safety
clearance is active is automatically determined by
What is the sequence of command? the cycle.
DP and DPR
The drilling depth can be defined either absolute
(DP) or relative (DPR) to the reference plane.
If it is entered as an absolute value, the value is
What effect do the parameters have? traversed directly in the cycle.
Additional notes
If a value is entered both for the DP and the DPR,
What else has to be taken into account? the final drilling depth is derived from the DPR. If theDPR deviates from the absolute depth programmed
via the DP, the message "Depth: Corresponds to
value for relative depth" is output in the dialog line.
The theory parts are suitable primarily as a guide for
NC beginners. Work through the manual carefully at
least once to gain an overview of the performance
scope and capabilities of your SINUMERIK control.
Siemens AG 1997 All rights reserved.
SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition. 2-37
3. From theory to practice
Drilling cycles and drilling patterns 083..976
2 2.1 Drilling cycles 2
The programming example shows you how to apply
the commands in the program.
If the values for the reference plane and the
retraction plane are identical, a relative depth must
not be programmed. The error message
You will find an application example for practically all 61101 "Reference plane incorrectly defined" isoutput and the cycle is not executed. This error
message is also output if the retraction plane lies
behind the reference plane, i.e. the distance to the
the commands after the theory part. final drilling depth is smaller.
Programming example
Drilling_centering Y Y A - B
You can use this program to make 3 holes using the
A
drilling cycle CYCLE81, whereby this cycle is called
with different parameter settings. The drilling axis is 120
always the Z axis.
30
0
B X Z
40 90 35 100 108
N10 G0 G90 F200 S300 M3 Specification of the technology values
N20 D3 T3 Z110 Traverse to retraction plane
N30 X40 Y120 Traverse to first drilling position
N40 CYCLE81 (110, 100, 2, 35) Cycle call with absolute final drilling
depth, safety clearance and incomplete
parameter list
N50 Y30 Traverse to next drilling position
N60 CYCLE81 (110, 102, , 35) Cycle call without safety clearance
N70 G0 G90 F180 S300 M03 Specification of the technology values
N80 X90 Traverse to next position
N90 CYCLE81 (110, 100, 2, , 65) Cycle call with relative final drilling depth
and safety clearance
N100 M30 End of program
Siemens AG 1997 All rights reserved.
2-38 SINUMERIK 840D/810D/FM-NC Programming Guide, Cycles (PGZ) - 08.97 Edition.
© Siemens AG, 2002. All rights reserved
0-18 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 PrefaceStructure of documentation 0
Explanation of the symbols
Sequence of operations
Explanation
Function
Parameters
Programming example
Programming
Additional notes
Cross-references to other documentation and sections
Important information and safety notices
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-19
0 Preface 11.02Structure of documentation 0
For your information
Your SINUMERIK 840D/840Di/810D is state of the art
and is manufactured in accordance with recognized
safety regulations, standards and specifications.
Additional devices
SIEMENS offers special add-on equipment, products
and system configurations for the focused expansion of
SIEMENS controls in your field of application.
Personnel
Only specially trained, authorized and experienced
personnel should be allowed to work on the control.
This applies at all times, even for short periods.
It is necessary to clearly define the respective
responsibilities of the personnel for setting up,
operation and maintenance; it is necessary to
supervise the compliance thereof.
Actions
It must be ascertained that the Instruction Manuals have
been read and understood by the persons working on
the control before installation and start-up of the control.
In addition, operation must be conducted under
constant supervision regarding the overall technical
state (faults and damages visible from outside, as well
as changes in operation behavior) of the control.
© Siemens AG, 2002. All rights reserved
0-20 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 PrefaceStructure of documentation 0
Service
Only qualified personnel specifically trained for this
purpose should be allowed to perform repairs, and only
in accordance with the contents of the maintenance
guides. Hereby, all established safety regulations have
to be complied with.
Note
The following are considered not compliant with the
usage to the intended purposes and are therefore
excluded from all liability of the manufacturer:
Every usage not complying with or going beyond the
abovementioned points.
If the control is not operated in a technically faultless
state, if proper safety precautions are not taken, or if
the instructions in the Instruction Manual are not
complied with.
If faults which could influence safety of operation are
not remedied before installation and start-up of the
control.
Each change, jumpering or shut-down of devices on
the control which serve for proper functioning, universal
usage and active and passive safety.
Unforeseen dangers may result in:
• personal injury and death,
• damage to the control, machine and other property
of the company and operator.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-21
0 Preface 11.02Structure of documentation 0
The following notes used in the documentation have a
special significance:
Notes
This symbol always appears in the documentation if
secondary information is given and there is an important
fact to be considered.
In this documentation, you will find the symbol shown
with reference to an ordering data option. The function
described can only be run if the control includes the
designated option.
Warnings
The following warnings, of graduated significance, are
used in the publication.
Danger
Indicates an imminently hazardous situation which, if
not avoided, will result in death or serious injury or in
substantial property damage.
Notice
Indicates a potentially hazardous situation which, if not
avoided, could result in death or serious injury or in
substantial property damage.
Caution
Used with the safety alert symbol indicates a potentially
hazardous situation which, if not avoided, may result in
minor or moderate injury or in property damage.
Caution
Used without safety alert symbol indicates a potentially
hazardous situation which, if not avoided, may result in
property damage.
© Siemens AG, 2002. All rights reserved
0-22 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
0 11.02 PrefaceStructure of documentation 0
Notice
Used without the safety alert symbol indicates a
potential situation which, if not avoided, may result in an
undesirable result or state.
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 0-23
0 Preface 11.02Structure of documentation 0
© Siemens AG, 2002. All rights reserved
0-24 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming 1
Flexible NC Programming
1.1 Variable and arithmetic parameters ................................................................................ 1-26
1.2 Variable definition............................................................................................................ 1-29
1.3 Array definition ................................................................................................................ 1-34
1.4 Indirect programming ...................................................................................................... 1-40
1.5 Assignments.................................................................................................................... 1-45
1.6 Arithmetic operations and functions ................................................................................ 1-46
1.7 Comparison and logic operators ..................................................................................... 1-48
1.8 Priority of operators ......................................................................................................... 1-53
1.9 Possible type conversions............................................................................................... 1-54
1.10 String operations ............................................................................................................. 1-55
1.10.1 Type conversion....................................................................................................... 1-56
1.10.2 Concatenation of strings .......................................................................................... 1-58
1.10.3 Conversion to lower/upper case .............................................................................. 1-59
1.10.4 Length of the string .................................................................................................. 1-60
1.10.5 Search for character/string in a string...................................................................... 1-60
1.10.6 Selection of a substring............................................................................................ 1-62
1.10.7 Selection of a single character................................................................................. 1-63
1.11 CASE instruction ............................................................................................................ 1-65
1.12 Control structures........................................................................................................... 1-67
1.13 Program coordination..................................................................................................... 1-72
1.14 Interrupt routine .............................................................................................................. 1-77
1.15 Axis transfer, spindle transfer......................................................................................... 1-85
1.16 NEWCONF: Setting machine data active (SW 4.3 and higher) ..................................... 1-90
1.17 WRITE: Write file (SW 4.3 and higher) .......................................................................... 1-91
1.18 DELETE: Delete file (SW 4.3 and higher) ...................................................................... 1-93
1.19 READ: Read lines in file (SW 5.2 and higher)................................................................ 1-94
1.20 ISFILE: File available in user memory NCK (SW 5.2 and higher).................................. 1-97
1.21 CHECKSUM: Creation of a checksum over an array (SW 5.2 and higher) ................... 1-98
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 1-25
1 Flexible NC Programming 11.021.1 Variable and arithmetic parameters 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
1.1 Variable and arithmetic parameters
Function
Using variables in place of constant values makes a
program more flexible. You can respond to signals
such as measured values or, by storing setpoints in
the variables, you can use the same program for
different geometries.
With variable calculation and jump instructions a
skilled programmer is able to create a very flexible
program archive and save a lot of programming
work.
Variable classes
The controller uses 3 classes of variable:
User-defined variable Name and type of variable defined by the
user, e.g. arithmetic parameter.
Arithmetic parameter Special, predefined arithmetic variable
whose address is R plus a number. The
predefined arithmetic variables are of the
REAL type.
System variable Variable provided by the controller that can
be processed in the program (write, read).
System variables provide access to zero
offsets, tool offsets, actual values, measured
values on the axes, control states, etc. (See
Appendix for the meaning of the system
variables)
Siemens AG, 2002. All rights reserved
1-26 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.1 Variable and arithmetic parameters 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Variable types
Type Meaning Value range
INT Integers with sign ±(231 - 1)
REAL Real numbers (fractions with decimal point, LONG ±(10-300 … 10+300)
REAL according to IEEE)
BOOL Boolean values: TRUE (1) and FALSE (0) 1, 0
CHAR 1 ASCII character specified by the code 0 … 255
STRING Character string, number of characters in […], Sequence of values
Max. 200 characters with 0 ... 255
AXIS Axis names (axis addresses) only All axis identifiers and
spindles in the channel
FRAME Geometric data for translation, rotation, scaling,
mirroring, see Chapter 4.
Arithmetic variable
Address R provides 100 arithmetic variables of type
REAL by default.
The exact number of arithmetic variables (up to
1000) is defined in machine data.
Example: R10=5
System variable
The controller provides system variables that can be
contained and processed in all running programs.
System variable provide machine and controller
states. Some of the system variables cannot be
assigned values.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 1-27
1 Flexible NC Programming 11.021.1 Variable and arithmetic parameters 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Special identifiers of system variables always begin
with a "$" sign followed by the specific names.
Summary of system variable types
1st letter Meaning
$M Machine data
$S Setting data
$T Tool management data
$P Programmed values
$A Current values
$V Service data
2nd letter Meaning
N NCK global
C Channel-specific
A Axis-specific
Example: $AA_IM
Means: Current axis-specific value in the machine
coordinate system.
Siemens AG, 2002. All rights reserved
1-28 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.2 Variable definition 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
1.2 Variable definition
User-defined variables
The programmer can define and assign values to
variables in addition to using predefined variables.
Local variables (LUD) are only valid in the program
where they are defined.
Global variables (GUD) are valid in all programs.
SW 4.4 and higher:
Machine data are used to redefine the local user
variables (LUD) defined in the main program as
program-global user variables (PUD).
Machine manufacturer
See machine manufacturer's specifications.
If they are defined in the main program, they will also
be valid at all levels of the subprograms called. They
are created with parts program start and deleted with
parts program end or reset.
Example:
$MN_LUD_EXTENDED_SCOPE=1
PROC MAIN ;Main program
DEF INT VAR1 ;PUD definition
...
SUB2 ;Subprogram call
...
M30
PROC SUB2 ;Subprogram SUB2
DEF INT VAR2 ;LUD DEFINITION
...
IF (VAR1==1) ;Read PUD
VAR1=VAR1+1 ;Read & write PUD
VAR2=1 ;Write LUD
ENDIF
SUB3 ;Subprogram call
...
M17
PROC SUB3 ;Subprogram SUB3
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 1-29
1 Flexible NC Programming 11.021.2 Variable definition 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
...
IF (VAR1==1) ;Read PUD
VAR1=VAR1+1 ;Read & write PUD
VAR2=1 ;Error: LUD from SUB2
;not known
ENDIF
...
M17
If machine data $MN_LUD_EXTENDED_SCOPE is set,
it is not possible to define a variable with the same
name in the main and subprograms.
Variable names
A variable name consists of up to 31 characters. The
first two characters must be a letter or an underscore.
The "$" sign can not be used for user-defined
variables because it is used for system variables.
Programming
DEF INT name
or DEF INT name=value
DEF REAL name
or DEF REAL name1,name2=3,name4
or DEF REAL name[array_index1,array_index2]
DEF BOOL name
DEF CHAR name
or DEF CHAR name[array_index]=("A","B",…)
DEF STRING[string_length] name
DEF AXIS name
or DEF AXIS name[array_index]
DEF FRAME name
Siemens AG, 2002. All rights reserved
1-30 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.2 Variable definition 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
If a variable is not assigned a value on definition, the
system sets zero as the default.
Variables must be defined at the beginning of the
program before they are used. The definition must
be made in a separate block; only one variable type
can be defined per block.
Explanation
INT Variable type integer, i.e. whole number
REAL Variable type real, i.e. factional number with decimal point
BOOL Variable type Boolean, i.e. 1 or 0 (TRUE or FALSE)
CHAR Variable type char, i.e. ASCII-coded character (0 to 255)
STRING Variable type string, i.e. sequence of char
AXIS Variable type axis, i.e. axis addresses and spindles
FRAME Variable type frame, i.e. geometric data
name Variable name
Programming examples
Variable type INT
DEF INT NUMBER This creates a variable of type integer with
the name NUMBER.
The system initializes the variable with zero.
DEF INT NUMBER= 7 This creates a variable of type integer with
the name NUMBER.
The system initializes the variable with zero.
Variable type REAL
DEF REAL DEPTH This creates a variable of type real with the
name DEPTH.
System initializes with zero (0.0).
DEF REAL DEPTH=6.25 This creates a variable of type real with the
name DEPTH. The variable is initialized
with 6.25.
DEF REAL DEPTH=3.1,LENGTH=2,NUMBER More than one variable can be defined in a
line.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 1-31
1 Flexible NC Programming 11.021.2 Variable definition 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Variable type BOOL
DEF BOOL IF_TOO_MUCH This creates a variable of type BOOL with
the name IF_TOO_MUCH.
System initializes with zero (FALSE).
DEF BOOL IF_TOO_MUCH=1 or This creates a variable of type BOOL with
DEF BOOL IF_TOO_MUCH=TRUE or the name IF_TOO_MUCH.
DEF BOOL WENN_ZUVIEL=FALSE
Variable type CHAR
DEF CHAR GUSTAV_1=65 A code value for the corresponding ASCII
character or the ASCII character itself
DEF CHAR GUSTAV_1="A" can be assigned to a variable of type CHAR
(code value 65 corresponds to letter "A").
Variable type STRING
DEF STRING[6] MUSTER_1="BEGIN" Variables of type string can contain a string
(sequence of characters). The maximum
number of characters is enclosed in square
brackets after the variable type.
Variable type AXIS
DEF AXIS AXIS_NAME=(X1) Variable of type AXIS are called
AXIS_NAME and contain the axis identifier
of a channel – here X1. (Axis names with an
extended address are in parentheses.)
Variable type FRAME
DEF FRAME BEVEL_1 Variables of type FRAME have names like
BEVEL_1.
Siemens AG, 2002. All rights reserved
1-32 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.2 Variable definition 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
A variable of type AXIS can contain an axis identifier
and a spindle identifier of a channel.
Note:
Axis names with an extended address must be in
parentheses.
Example of programming with program-
local variables
DEF INT COUNT
LOOP: G0 X… ;Loop
COUNT=COUNT+1
IF COUNT greater than
< less than
>= greater than or equal to
=100 GOTOF DEST
or
R11=R10>=100
IF R11 GOTOF DEST
The result of the R10>=100 comparison is first
buffered in R11.
Siemens AG, 2002. All rights reserved
1-48 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.7 Comparison and logic operators 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Precision correction on comparison errors
T RUNC (R1*1000)
T he TRUNC command truncates the operand multiplied by a precision factor
Function
Settable precision for comparison commands
Program data of type REAL are displayed internally
with 64 bits in IEEE format. This display format can
cause decimal numbers to be displayed imprecisely
and lead to unexpected results when compared with
the ideally calculated values.
Relative equality
To prevent the imprecision caused by the display
format from interfering with program flow, the
comparison commands do not check for absolute
equality but for relative equality.
SW 6.3 and lower
Relative equality considered 10-12 for
• Equality (==)
• Inequality ()
• Greater than or equal to (>=)
• Less than or equal to ()
• Less than () and ( R3 GOTOF ERROR Jump executed (SW 6.3 and lower)
N42 M30 End of program
N43 ERROR: SETAL(66000)
R1=61.01 R2=61.02 R3=0.01 Assignment of initial values
R11=TRUNC(R1*1000) R12=TRUNC(R2*1000) Precision correction
R13=TRUNC(R3*1000)
IF ABS(R12-R11) > R13 GOTOF ERROR Jump not executed
M30 End of program
ERROR: SETAL(66000)
Calculate and evaluate quotient of both operands
R1=61.01 R2=61.02 R3=0.01 Assignment of initial values
IF ABS((R2-R1)/R3)-1) > 10EX-5 GOTOF Jump not executed
ERROR
M30 End of program
ERROR: SETAL(66000)
Siemens AG, 2002. All rights reserved
1-50 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.7 Comparison and logic operators 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Logic operators
Logic operators are used to link truth values.
AND, OR, NOT, and XOR can only be applied to
variables of type BOOL. However, they can also be
applied to data types CHAR, INT, and REAL by
implicit type conversion.
Spaces must be left between BOOLEAN operands
and operators.
For the logic (Boolean) operations, the following
applies to data types BOOL, CHAR, INT, and REAL:
0 means FALSE
not equal to 0 means TRUE
Meaning of logic operators
AND AND
OR OR
NOT Negation
XOR Exclusive OR
In arithmetic expressions, the execution order of all
the operators can be specified by parentheses, in
order to override the normal priority rules.
Programming example
IF (R10=17.5) GOTOF ZIEL
IF NOT R10 GOTOB START
NOT is only applied to one operand.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 1-51
1 Flexible NC Programming 11.021.7 Comparison and logic operators 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Bit logic operators
Logic operations can also be applied to single bits of
types CHAR and INT. Type conversion is automatic.
Meaning of bit logic operators
B_AND Bit AND
B_OR Bit OR
B_NOT Bit negation
B_XOR Bit exclusive OR
The operator B_NOT refers to one operand only, it
comes after the operator.
Programming example
IF $MC_RESET_MODE_MASK B_AND 'B10000' GOTOF ACT_PLANE
Siemens AG, 2002. All rights reserved
1-52 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.8 Priority of operators 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
1.8 Priority of operators
Priority of the operators
Each operator is assigned a priority. When an
expression is evaluated, the operators with the
highest priority are always applied first. Where
operators have the same priority, the evaluation is
from left to right.
In arithmetic expressions, the execution order of all
the operators can be specified by parentheses, in
order to override the normal priority rules.
Order of operators
(from the highest to lowest priority)
1. NOT, B_NOT Negation, bit negation
2. *, /, DIV, MOD Multiplication, division
3. +, – Addition, subtraction
4. B _AND B it AND
5. B _XOR Bit exclusive OR
6. B _OR B it OR
7. A ND A ND
8. XOR Exclusive OR
9. OR OR
10. , =, = 0.5 are rounded up, others
rounded down (cf. ROUND function)
1) Value 0 corresponds to TRUE, value == 0
corresponds to FALSE
2) If the value is in the permissible range
3) If only 1 character
4) String length 0 = >FALSE, otherwise TRUE
If conversion produces a value greater than the
target range, an error message is output.
Additional notes
If mixed types occur in an expression, type
conversion is automatic.
Siemens AG, 2002. All rights reserved
1-54 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
1 11.02 Flexible NC Programming1.10 String operations 1
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
1.10 String operations
Overview
Further string manipulations are provided in addition to the
conventional operations "Assignment" and "Comparison"
described in this section:
Explanation
Type conversion to STRING:
1)
STRING_ERG = character.
Example:
EXTCALL (”/_N_WKS_DIR/_N_SHAFT_WPD/_N_SHAFT_SPF”) or
EXTCALL (”SHAFT”)
Function
EXTCALL can be used to reload a program from the
HMI in "Processing from external source" mode. All
programs that can be accessed via the directory
structure of HMI can be reloaded and run.
External program path
SD 42700: EXT_PROG_PATH permits flexible
setting of the call path. SD 42700 contains a path
definition that builds the absolute path name of the
program to be called in conjunction with the
programmed subprogram identifier.
Call of an external subprogram
An external subprogram is called up with parts
program command EXTCALL.
The
• subprogram names programmed with EXTCALL
and
• setting data SD 42700: EXT_PROG_PATH
Siemens AG, 2002. All rights reserved
2-132 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
2 11.02 Subprograms, Macros2.15 Executing external subprogram: EXTCALL (SW 4.2 and higher) 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
result in the program path for the external
subprogram call by character concatenation of
• the content of SD 42700: EXT_PROG_PATH
(e.g. /_N_WKS_DIR/_N_WKST1_WPD)
• the character "/" as the separator
(if a path was specified with SD 42700:
EXT_PROG_PATH)
• the subprogram path or subprogram identifier
specified with EXTCALL.
SD 42700: EXT_PROG_PATH has a blank as its
default. If the external subprogram is called without
an absolute path name, the same search path is
executed on the HMI Advanced as for calling a
subprogram from NCK memory.
1. current directory/ subprogram identifier
2. current directory/subprogram identifier_SPF
3. current directory/subprogram identifier_MPF
4. /_N_SPF_DIR/subprogram identifier_SPF
5. /_N_CUS_DIR/subprogram identifier_SPF
6. /_N_CMA_DIR/subprogram identifier_SPF
7. /_N_CST_DIR/subprogram identifier_SPF
"current directory": stands for the directory in which
the main program was selected.
"subprogram identifier": stands for the subprogram
name programmed with EXTCALL.
Adjustable load memory (FIFO buffer)
A load memory is required in the NCK in order to
process a program in "Execution from external"
mode (main program or subprogram). The default
setting for the size of the load memory is 30 Kbytes.
MD 18360: MM_EXT_PROG_BUFFER_SIZE sets
the size of the reload buffer. MD 18362:
MM_EXT_PROG_BUFFER_NUM sets the number
of reload buffers. One reload buffer must be set for
each program (main program or subprogram) to run
concurrently in "Processing from external source"
mode.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 2-133
2 Subprograms, Macros 11.022.15 Executing external subprogram: EXTCALL (SW 4.2 and higher) 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming examples
1. The program to be reloaded is located on the
local hard disk of HMI Advanced:
Setting data SD 42700: EXT_PROG_PATH contains the
following path: "/_N_WKS_DIR/_N_WST1".
The main program _N_MAIN_MPF
is in the user memory and selected.
N10 PROC MAIN
N20 ...
N30 EXTCALL "ROUGHING" ; Call of external subprogram
; ROUGHING
N40 ...
N50 M30
Subprogram "ROUGHING" (located in the HMI Advanced
directory structure under workpieces ->WST1):
N10 PROC ROUGHING
N20 G1 F1000
N30 X=... Y=... Z=...
N40 ...
N90 M17
2. The program to be reloaded is located on the
network drive or ATA card of HMI
EXTCALL Windows path
Call for network drive (HMI Embedded or Advanced)
EXTCALL \\R4711\workpieces\contour1.spf
Call for ATA card (HMI Embedded), e.g.
EXTCALL C:\workpieces\contour2.spf
F or HMI Embedded, an absolute path must always
be specified.
F or more information about operation, see
/ BEM/ HMI Embedded
/BAD/ HMI Advanced
Siemens AG, 2002. All rights reserved
2-134 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
2 11.02 Subprograms, Macros2.15 Executing external subprogram: EXTCALL (SW 4.2 and higher) 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
External subprograms are not permitted to include
jump commands such as GOTOF, GOTOB, CASE,
FOR, LOOP, WHILE or REPEAT.
Subprogram calls – even nested EXTCALL calls are
possible.
SW 6.3 and higher
IF-ELSE-ENDIF constructions are possible.
POWER ON, RESET
Reset and power ON cause external subprogram
calls to be interrupted and the associated load
memory to be erased.
F or more information about "Processing from
external source", see:
/ FB/ K1, BAG, Channel, Program control
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 2-135
2 Subprograms, Macros 11.022.16 Subprogram call with M/T function 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
2.16 Subprogram call with M/T function
Function
The T/M function can be replaced with a subprogram
call by making the appropriate setting in the machine
data, for example, for calling the tool change routine.
At block search subprogram calls with M/T functions
behave like standard subprogram calls.
F or more information about "Subprogram call with
M/T functions", see:
/FB/ K1, BAG, Channel, Program control
Example 1: Tool change with M6
M function M6 is replaced by tool change routine TC_UP_M6
N10 PROC ROUGHING3
N20 G1 F1000
N30 X=... Y=... Z=...
N40 T1234 M6 ; ; Call TC_UP_M6
M30
Associated subprogram TC_UP_M6:
N110 PROC TC_UP_M6
...
N130 G53 D0 G0 X=... Y=... Z=... ; ; Approach tool change point
N140 M6 ; ; Execute tool change
...
N190 M17
Example 2: Tool change with T function programming
T function is replaced by tool change routine TC_UP_T
N10 PROC ROUGHING4
N20 G1 F1000
N30 X=... Y=... Z=...
N40 T1234 ; ; Call TC_UP_T
M30
Siemens AG, 2002. All rights reserved
2-136 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
2 11.02 Subprograms, Macros2.16 Subprogram call with M/T function 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Associated subprogram TC_UP_T:
N310 PROC TC_UP_T
...
N330 IF $C_T_PROG == 1
N340 G53 D0 G0 X=... Y=... Z=... ; Approach tool change point
N350 T=$C_T ; Execute tool change
N360 ENDIF
...
N390 M17
Extension of T function substitution
As from SW 6.4, T function substitution is
extended to permit setting in machine data whether
with programming of both:
D numbers or DL numbers and T numbers
• in one block, D or DL will be passed as
parameters to the T substitution cycle as
predefined (default) or
• run before the T substitution cycle call.
MD 10719: T_NO_FCT_CYCLE_MODE sets
parameterization of the T function substitution as
follows
Value 0: the D or DL number is passed to the cycle,
as previously, (default).
Value 1: the D or DL number is calculated directly
in the block.
This function is only active if the tool change was
configured with an M function (MD 22550:
TOOL_CHANGE_MODE = 1), otherwise the D or DL
values are always passed.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 2-137
2 Subprograms, Macros 11.022.17 Cycles: Setting parameters for user cycles 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
2.17 Cycles: Setting parameters for user cycles
Files and paths
Explanation
cov.com Overview of cycles
uc.com Cycle call description
Function
Customized cycles can be parameterized with these
files.
Sequence
The cov.com file is included with the standard cycles
at delivery and is to be expanded accordingly. The
uc.com file is to be created by the user.
Both files are to be loaded in the passive file system
in the "User cycles" directory (or must be given the
appropriate path specification in the program:
;$PATH=/_N_CUS_DIR
Adaptation of cov.com – Overview of cycles
The cov.com file supplied with the standard cycles
has the following structure:
%_N_COV_COM File name
;$PATH=/_N_CST_DIR) Path specification
;Vxxx 11.12.95 Sca cycle overview Comment line
C1(CYCLE81) drilling, centering Call for 1st cycle
C2(CYCLE82) Boring, counterboring Call for 2nd cycle
...
C24(CYCLE98) Chaining of threads Call for last cycle
M17 End of file
Siemens AG, 2002. All rights reserved
2-138 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
2 11.02 Subprograms, Macros2.17 Cycles: Setting parameters for user cycles 2
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
For each newly added cycle a line must be added
with the following syntax:
C () comment text
Number: Any integer, must not have been used in
the file before;
Cycle name: The program name of the cycle to be
included
Comment text: Optionally a comment text for the
cycle
Example:
C25 (MY_CYCLE_1) usercycle_1
C26 (SPECIAL CYCLE)
Example of uc.com file
User cycle description
The explanation is based on the continuation of the
example:
For the following two cycles a cycle parameterization
is to be newly created:
PROC MY_CYCLE_1 (REAL PAR1, INT PAR2, CHAR PAR3, STRING[10] PAR4)
;The cycle has the following transfer parameters:
;
;PAR1: Real value in range -1000.001 $P_UIFR [$P_UIFRNUM]
(settable frame) effective
$P_ACTFRAME = $P_BFRAME : $P_IFRAME : $P_PFRAME
Entered via program, e.g. Entered via program, e.g.
$P_BFRAME=CTRANS(X,10) $P_PFRAME=CTRANS(X,10)
or TRANS X10
Entered via program, e.g.
$P_IFRAME=CTRANS(X,10)
P redefined settable frames $P_UBFR
T he base frame is programmed with $P_UBFR, but
it is not simultaneously active in the parts program.
The base frame programmed with $P_UBFR is
included in the calculation if
• Reset was activated and bits 0 and 14 are set in
MD RESET_MODE_MASK and
• instructions G500, G54...G599 were executed.
Predefined settable frames $P_UIFR[n]
The predefined frame variable $P_UIFR[n] can be
used to read or write the settable zero offsets G54 to
G599 from the parts program.
T hese variables produce a one-dimensional array of
type FRAME called $P_UIFR[n].
Assignment to G commands
F ive predefined settable frames are set as standard
$P_UIFR[0]...$P_UIFR[4] or 5 G commands with
the same meaning – G500 and G54 to G57 – at
whose addresses values can be stored.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-239
6 Frames 11.026.1 Coordinate transformation via frame variables 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
$ P_IFRAME=$P_UIFR[0] corresponds to G500
$P_IFRAME=$P_UIFR[1] corresponds to G54
$ P_IFRAME=$P_UIFR[2] corresponds to G55
$ P_IFRAME=$P_UIFR[3] corresponds to G56
$P_IFRAME=$P_UIFR[4] corresponds to G57
You can change the number of frames with machine
data:
$ P_IFRAME=$P_UIFR[5] corresponds to G505
… … …
$P_IFRAME=$P_UIFR[99] corresponds to G599
T his allows you to generate up to 100 coordinate
systems which can be called up globally in different
programs, for example, as zero point for various
fixtures.
F rame variables must be programmed in a separate
NC block in the NC program.
Exception: programming of a settable frame with
G54, G55, ...
Siemens AG, 2002. All rights reserved
6-240 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.2 Frame variables/assigning values to frames 6
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
6 .2 Frame variables/assigning values to frames
V alues can be assigned directly, frames can be
chained or frames can be assigned to other frames
in the NC program.
Direct value assignment
Programming
$P_PFRAME=CTRANS (X, axis value, Y, axis value, Z, axis value, …)
$ P_PFRAME=CROT (X, angle, Y, angle, Z, angle, …)
$ P_PFRAME=CSCALE (X, scale, Y, scale, Z, scale, …)
$P_PFRAME=CMIRROR (X, Y, Z)
P rogramming $P_BFRAME is carried out analog to
$P_PFRAME.
Explanation of the commands
C TRANS Translation of specified axes
CROT Rotation around specified axes
C SCALE Scale change on specified axes
C MIRROR Direction reversal on specified axis
Function
You can use these functions to assign frames or
frame variables directly in the NC program.
Sequence
You can program several arithmetic rules in
succession.
Example:
$P_PFRAME=CTRANS(…):CROT(…):CSCALE…
P lease note that the commands must be connected CROTNS
CTR
A
by the colon chain operator: (…):(…).
This causes the commands firstly to be linked and
secondly to be executed additively in the
programmed sequence.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-241
CSCALE
6 Frames 11.026.2 Frame variables/assigning values to frames 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
T he values programmed with the above commands
are assigned to the frames and stored.
T he values are not activated until they are assigned
to the frame of an active frame variable $P_BFRAME
or $P_PFRAME.
Programming example Z 2
T ranslation, rotation and mirroring are activated by
value assignment to the current programmable Y
frame.
3
Y
Y
Z X X
1
Y
1 CTRA NS
2 CROT
3 CM IRROR
X
N 10 $P_PFRAME=CTRANS(X,10,Y,20,Z,5):CROT(Z,45):CMIRROR(Y)
Siemens AG, 2002. All rights reserved
6-242 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.2 Frame variables/assigning values to frames 6
8 40D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
R eading and changing frame components
Programming (examples)
R10=$P_UIFR[$P_UIFRNUM, X, RT] Assign the angle of rotation RT around the X
axis from currently valid settable zero offset
$P_UIFRNUM to the variable R10.
R12=$P_UIFR[25, Z, TR] Assign the offset value TR in Z from the data
record of set frame no. 25 to the variable
R12.
R15=$P_PFRAME[Y, TR] Assign the offset value TR in Y of the current
programmable frame to the variable R15.
$P_PFRAME[X, TR]=25 Modify the offset value TR in X of the current
programmable frame. X25 applies
immediately.
E xplanation of the commands
$P_UIFRNUM T his command automatically establishes the reference to the currently
valid settable zero offset.
P_UIFR[n, …, …] Specify the frame number n to access the settable frame no. n.
S pecify the component to be read or modified:
TR TR translation, FI translation fine, RT rotation, SC scale change,
FI MI mirroring.
RT T he corresponding axis is also specified (see examples).
S C
M I
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-243
6 Frames 11.026.2 Frame variables/assigning values to frames 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Function
T his feature allows you to access individual data of
a frame, e.g. a specific offset value or angle of
rotation.
You can modify these values or assign them to
another variable.
Sequence
Calling frame
B y specifying the system variable $P_UIFRNUM you
can access the current zero offset set with $P_UIFR
or G54, G55, ... ($P_UIFRNUM contains the number
of the currently set frame).
A ll other stored settable $P_UIFR frames are called
up by specifying the appropriate number
$P_UIFR[n].
For predefined frame variables and user-defined
frames, specify the name, e.g. $P_IFRAME.
C alling data
The axis name and the frame component of the
value you want to access or modify are written in
square brackets, e.g. [X, RT] or [Z, MI].
Siemens AG, 2002. All rights reserved
6-244 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6 .2 Frame variables/assigning values to frames 6
8 40D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Linking complete frames
A complete frame can be assigned to another frame.
Programming (examples)
D EF FRAME SETTING1 Assign the values of the user frame
SETTING1=CTRANS(X,10) SETTING1 to the current programmable
$ P_PFRAME=SETTING1 frame.
D EF FRAME SETTING4
T he current programmable frame is
S ETTING4=$P_PFRAME
stored temporarily and can be recalled.
$P_PFRAME=SETTING4
Additional notes
Value range for RT rotation
Rotation around 1st geometry axis: –180° to +180°
Rotation around 2nd geometry axis: –89.999° to +90°
Rotation around 3rd geometry axis: –180° to +180°
Frame chaining
Programming (examples)
$P_IFRAME=$P_UIFR[15]:$P_UIFR[16] $P_UIFR[15] contains, for example,
data for zero offsets. The data of
$P_UIFR[16], e.g. data for rotations,
are subsequently processed additively.
$P_UIFR[3]=$P_UIFR[4]:$P_UIFR[5] The settable frame 3 is created by
chaining the settable frames 4 and 5.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-245
6 Frames 11.026.2 Frame variables/assigning values to frames 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Function
F rame chaining is suitable for the description of Z
Yseveral workpieces, arranged on a pallet, which are
to be machined in the same process.
G54
X
Sequence
T he frames are chained in the programmed
sequence. The frame components (translations,
rotations, etc.) are executed additively in succession.
T he frame components can only contain
intermediate values for the description of pallet
tasks. These are chained to generate various
workpiece zeroes.
P lease note that the frames must be linked to one
another by the colon chain operator : .
Siemens AG, 2002. All rights reserved
6-246 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.2 Frame variables/assigning values to frames 6
840D 8 40D 810D 840Di
NCU 571 NCU 572
NCU 573
Definition of new frames
Programming
DEF FRAME PALLET1
PALETT1=CTRANS(…):CROT(…)…
Function
In addition to the predefined settable frames described
above, you also have the option of creating new frames.
T his is achieved by creating variables of type FRAME to
which you can assign a name of your choice.
Sequence
You can use the functions CTRANS, CROT, CSCALE
and CMIRROR to assign values to your frames in the
NC program.
You will find more information on this subject on the
previous pages.
Frame rotation definition
Function
Frame rotations can be used to define application-
specific orientations in the area:
• ROT: Individual rotations for all geometry axes
• ROTS, AROTS, CROTS: Rotation by specifying
a solid angle (max. 2); see description in /FB1/
K2: coordinate systems.
• TOFRAME: Rotation by frame "TOFRAME", with
Z axis pointing in the tool direction.
• TOROT: Rotation by frame "TOROT", which
only overwrites the rotation component of
frames that have already been programmed.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-247
6 Frames 11.026.3 Coarse/fine offset 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
6.3 Coarse/fine offset
Function
Fine offset
A fine offset of the base frames and of all other
settable frames can be programmed with command
CFINE(X, ..,Y, ...). Mirroring Scaling
Rotation
Coarse offset Fine offset
The coarse offset is defined with CTRANS(...).
Coarse offset
Coarse and fine offset add up to the total offset.
Frame structure with fine offset
Programming
$P_UBFR=CTRANS(x, 10) : CFINE(x, 0.1) : CROT(x, 45) ;chaining offset, fine
offset and rotation
$P_UIFR[1]=CFINE(x, 0.5, y, 1.0, z, 0.1) ;the total frame is overwritten with
CFINE, incl. coarse offset.
A ccess to the individual components of the fine offset is
achieved through component specification FI.
Programming
DEF REAL FINEX ;Definition of variable FINEX
FINEX=$P_UIFR[$P_UIFRNUM, x, FI] ;Readout the fine offset via variable FINEX
F INEX=$P_UIFR[3, X, FI] ;Readout the fine offset of X axis in the 3rd frame via
variable FINEX
F ine offset can only take place if MD 18600:
MM_FRAME_FINE_TRANS=1.
A fine offset changed via operator input is only active
after the corresponding frame is activated, i.e.
activation is conducted via G500, G54...G599. An
activated fine offset of a frame is active for as long
as the frame is active.
Siemens AG, 2002. All rights reserved
6-248 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.4 DRF offset 6
8 40D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
T he programmable frame has no fine offset. If the
programmable frame is assigned a frame with fine
offset, then the total offset is established by adding
the coarse and the fine offset. When reading the
programmable frame the fine offset is always zero.
Machine manufacturer
S W 5 and higher
T he fine offset can be configured by means of
MD 18600 MM_FRAME_FINE_TRANS in the
following variants:
0: Fine offset cannot be entered or programmed.
G58 and G59 are not possible.
1: Fine offset for settable frames, base frames,
programmable frames, G58 and G59 can be
entered/programmed
6 .4 DRF offset
Offset using handwheel, DRF
I n addition to all the translations described in this Z BOS
section, you can also define zero offsets with the
Z
handwheel (DRF offset). BCS
Y
Y BCSBOS
The DRF offset acts on the basic coordinate system.
See the diagram for the relationships.
Base frame
You will find more information in the Operator’s
X
Guide. BOS
DRF, external ZO
XBCS
Clear DRF offset, DRFOF
DRFOF clears the handwheel offset for all axes
assigned to the channel. DRFOF is programmed in
a separate NC block.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-249
6 Frames 11.026.5 External zero offset 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
6 .5 External zero offset
External zero offset
Y Y Y Y Y
T his is another way of moving the zero point MCS MCS BCS BOS SZS
between the basic and workpiece coordinate
system.
X
SZSG54...G599
O nly linear translations can be programmed with the
X
external zero offset. BOSBasic frame
External zero offset
P rogramming offset values, $AA_ETRANS DRF offset
The offset values are programmed by assigning the XBCS
Kinematic transformation
axis-specific system variables.
X
Preset offset MCS
Assigning offset value
$ AA_ETRANS[axis]=RI
RI is the arithmetic variable of type REAL which
contains the new value.
T he external offset is generally set by the PLC and
not specified in the parts program.
T he value entered in the parts program only
becomes active when the corresponding signal is
enabled at the VDI interface (NCU-PLC interface).
Siemens AG, 2002. All rights reserved
6-250 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.6 Programming PRESET offset, PRESETON 6
8 40D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
6 .6 Programming PRESET offset, PRESETON
Programming
PRESETON(AXIS,VALUE,…)
Explanation of the commands
PRESETON Set actual value
Axis Machine axis parameter
Value New actual value to apply to the specified axis
Function YMCS YMCS
I n special applications, it can be necessary to assign
a new programmed actual value to one or more
axes at the current position (stationary).
Kinematic transformation
Note: Preset mode with synchronized actions should XMCS
only be implemented the vocabulary word "WHEN" Preset offset
or "EVEREY".
Sequence
T he actual values are assigned to the machine
coordinate system – the values refer to the machine
axes.
E xample:
N 10 G0 A760
N20 PRESETON(A1,60)
Axis A travels to position 760. At position 760, machine
axis A1 is assigned the new actual value 60.
From this point, positioning is performed in the new
actual value system.
T he reference point becomes invalid with the function
PRESETON. You should therefore only use this
function for axes which do not require a reference point.
If the original system is to be restored, the reference
point must be approached with G74 – see Section 3.1.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-251
6 Frames 11.026.7 Deactivating frames 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
6 .7 Deactivating frames
Explanation of the commands
D RFOF Deactivate (clear) the handwheel offsets (DRF)
G53 N on-modal deactivation of programmable and all settable frames
G153 Non-modal deactivation of programmable frames, base frames and all
settable frames
SUPA Non-modal deactivation of all programmable frames, base frames, all
settable frames and handwheel offsets (DRF)
Additional notes
The programmable frames are cleared by assigning
a "zero frame" (without axis specification) to the
programmable frame.
Example:
$P_PFRAME=TRANS( )
$P_PFRAME=ROT( )
$P_PFRAME=SCALE( )
$P_PFRAME=MIRROR( )
Siemens AG, 2002. All rights reserved
6-252 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.8 Frame calculation from 3 measuring points in the area: MEAFRAME 6
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
6 .8 Frame calculation from three measuring points in the area: MEAFRAME
M EAFRAME is an extension of the 840D language
used for supporting measuring cycles.
This function is valid in SW 4.3 and higher.
Function
When a workpiece is positioned for machining, its
position relative to the Cartesian machine coordinate
system is generally both shifted and rotated referring
to its ideal position.
For exact machining or measuring either a costly
physical adjustment of the part is required or the
motions defined in the parts program must be
changed.
A frame can be determined by probing three points in
the area for which the ideal positions are known.
Probing is performed with a tactile or optical sensor
touching special holes or spheres that are precisely
fixed to the backing plate.
T he function MEAFRAME calculates the frame from
three ideal and the corresponding measured points.
In order to map the measured coordinates onto the
ideal coordinates using a rotation and a translation, the
triangle formed by the measured points must be
congruent to the ideal triangle. This is achieved by
means of a compensation algorithm that minimizes the
sum of squared deviations needed to reshape the
measured triangle into the ideal triangle.
Since the effective distortion can be used to judge the
quality of the measurement, MEAFRAME returns it as
an additional variable.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-253
6 Frames 11.026.8 Frame calculation from 3 measuring points in the area: MEAFRAME 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming
MEAFRAME(IDEAL_POINT,MEAS_POINT,FIT_QUALITY)
Explanation of the commands
MEAFRAME Frame calculation of three measured points in space
IDEAL_POINT 2 -dim. array of real data containing the three coordinates of the ideal
points
MEAS_POINT 2-dim. array of real data containing the three coordinates of the measured
points
F IT_QUALITY Variable of type real returning the following information:
- 1: The ideal points are located approximately on a straight line: The
frame could not be calculated. The frame variable returned
contains a neutral frame.
-2: The measured points are located approximately on a straight line:
The frame could not be calculated. The frame variable returned
contains a neutral frame.
-4: The calculation of the rotation matrix failed for a different reason
P ositive value:
Sum of the distortions (distances between the points) needed to
reshape the measured triangle into one that is congruent to the
ideal triangle.
Application example
; Parts program 1
;
D EF FRAME CORR_FRAME
;
; Setting measured points
DEF REAL IDEAL_POINT[3,3] = SET(10.0,0.0,0.0, 0.0,10.0,0.0, 0.0,0.0,10.0)
D EF REAL MEAS_POINT[3,3] = SET(10.1,0.2,-0.2, -0.2,10.2,0.1, -0.2,0.2, 9.8); for test
DEF REAL FIT_QUALITY = 0
;
D EF REAL ROT_FRAME_LIMIT = 5; allows max. 5o rotation of the part position
DEF REAL FIT_QUALITY_LIMIT = 3; allows max. 3 mm distortion between the ideal;
and the measured triangle
DEF REAL SHOW_MCS_POS1[3]
DEF REAL SHOW_MCS_POS2[3]
DEF REAL SHOW_MCS_POS3[3]
; =======================================================
;
Siemens AG, 2002. All rights reserved
6-254 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.8 Frame calculation from 3 measuring points in the area: MEAFRAME 6
8 40D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
N100 G01 G90 F5000
N110 X0 Y0 Z0
;
N200 CORR_FRAME=MEAFRAME(IDEAL_POINT,MEAS_POINT,FIT_QUALITY)
;
N230 IF FIT_QUALITY < 0
SETAL(65000)
G OTOF NO_FRAME
E NDIF
,
N240 IF FIT_QUALITY > FIT_QUALITY_LIMIT
SETAL(65010)
G OTOF NO_FRAME
ENDIF
;
N250 IF CORR_FRAME[X,RT] > ROT_FRAME_LIMIT; limiting the 1st RPY angle
SETAL(65020)
G OTOF NO_FRAME
ENDIF
;
N260 IF CORR_FRAME[Y,RT] > ROT_FRAME_LIMIT; limiting the 2nd RPY angle
S ETAL(65021)
G OTOF NO_FRAME
ENDIF
;
N270 IF CORR_FRAME[Z,RT] > ROT_FRAME_LIMIT; limiting the 3rd RPY angle
S ETAL(65022)
GOTOF NO_FRAME
ENDIF
;
N300 $P_IFRAME=CORR_FRAME; activate the probe frame via a settable frame
;
; check the frame by positioning the geometry axes at the ideal points
;
N400 X=IDEAL_POINT[0,0] Y=IDEAL_POINT[0,1] Z=IDEAL_POINT[0,2]
N410 SHOW_MCS_POS1[0]=$AA_IM[X]
N420 SHOW_MCS_POS1[1]=$AA_IM[Y]
N430 SHOW_MCS_POS1[2]=$AA_IM[Z]
;
N500 X=IDEAL_POINT[1,0] Y=IDEAL_POINT[1,1] Z=IDEAL_POINT[1,2]
N510 SHOW_MCS_POS2[0]=$AA_IM[X]
N520 SHOW_MCS_POS2[1]=$AA_IM[Y]
N530 SHOW_MCS_POS2[2]=$AA_IM[Z]
;
N600 X=IDEAL_POINT[2,0] Y=IDEAL_POINT[2,1] Z=IDEAL_POINT[2,2]
N610 SHOW_MCS_POS3[0]=$AA_IM[X]
N620 SHOW_MCS_POS3[1]=$AA_IM[Y]
N 630 SHOW_MCS_POS3[2]=$AA_IM[Z]
;
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-255
6 Frames 11.026.9 NCU-global frames (SW 5 and higher) 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
N 700 G500; Deactivate settable frame, as preset with zero frame (no value set)
;
N O_FRAME:
M0
M30
6.9 NCU-global frames (SW 5 and higher)
Function
NCU-global frames are only available once for all
channels of each NCU. NCU-global frames can be
written and read from all channels. The NCU-global
frames are activated in the respective channel.
C hannel axes and machine axes with offsets can be
scaled and mirrored by means of global frames.
W ith global frames there is no geometrical
relationship between the axes. Therefore, it is not
possible to perform rotations or program geometry
axis identifiers.
• It is not possible to use global frames for rotations.
Programming a rotation is refused and alarm:
"18310 channel %1 block %2 frame: rotation not
allowed" is displayed.
• Chaining of global frames and channel-specific
frames is possible. The resulting frame contains all
frame elements including rotations for all axes. If a
frame with rotation elements is assigned to a global
frame, it is rejected and alarm "Frame: rotation not
allowed" is displayed.
NCU-global base frames: $P_NCBFR[n]
You can configure up to 8 NCU-global basic frames.
Siemens AG, 2002. All rights reserved
6-256 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.9 NCU-global frames (SW 5 and higher) 6
8 40D 8 40D 810D 840Di
NCU 571 NCU 572
NCU 573
Machine manufacturer
The number of global base frames is configured via
machine data. (See /FB/ K2, Axes, Coordinate
Systems, Frames)
Channel-specific base frames can be present at the
same time.
G lobal frames can be written and read from all
channels of an NCU. When writing global frames, the
user must pay attention to channel coordination, for
example, by using Wait marks (WAITMC).
NCU-global settable frames: $P_UIFR[n]
All settable frames G500, G54...G599 can be
configured either NCU-global or channel-specific.
Machine manufacturer
A ll settable frames can be reconfigured as global frames
via MD 18601 MM_NUM_GLOBAL_USER_FRAMES.
See /FB/ K2, Axes, Coordinate Systems, Frames.
C hannel axis identifiers and machine axis identifiers
can be used as axis identifiers for the frame program
commands. Programming of geometry identifiers is
rejected with an alarm.
6.9.1 Channel-specific frames
Function
T he number of base frames can be configured in the
channel via MD 28081 MM_NUM_BASE_FRAMES.
The standard configuration provides at least one base
frame per channel. A maximum of eight base frames
are supported per channel. In addition to the eight
base frames, there can also be eight NCU-global base
frames in the channel.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-257
6 Frames 11.026.9 NCU-global frames (SW 5 and higher) 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
S ettable frames/base frames can be written and read
from the control and the PLC
• via the parts program and
• via the OPI.
Fine offset is also possible for global frames.
Suppression of global frames also takes place, as is
the case with channel-specific frames, via G53, G153,
SUPA and G500.
$P_CHBFR[n]
The base frames can be read and written via system
variable $P_CHBFR[n]. When writing a base frame,
the chained total base frame is not activated; it is
only activated when the G500, G54..G599 instruction
is executed. The variable mainly serves as memory
for writing processes to the MMC and PLC base
frame. These frame variables are saved by data
backup.
First basic frame in the channel
Writing to a predefined variable $P_UBFR will not
activate the basic frame with array index 0
simultaneously, but it will be activated only after a
G500, G54..G599 command is executed. The
variable can also be written and read in the program.
$P_UBFR
$P_UBFR is identical to $P_CHBFR[0].
As standard, there is always a base frame in the
channel making the system variable compatible with
older versions. If there is no channel-specific base
frame, an alarm is issued at read/write: "Frame:
instruction not permissible".
Siemens AG, 2002. All rights reserved
6-258 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.9 NCU-global frames (SW 5 and higher) 6
8 40D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
6.9.2 Frames active in the channel
Function
SW 6.1 and higher
Current system frames for
$P_PARTFRAME TCARR and PAROT
$P_SETFRAME preset actual value memory and
scratching,
$P_EXTFRAME zero offset external,
You can read and write the current system frame in
the parts program via these system variables.
$P_NCBFRAME[n]
Current NCU-global basic frames
You can read and write the current global basic
frame field elements via system variable
$P_NCBFRAME[n]. The resulting total base frame
is calculated by means of the write process in the
channel.
The modified frame is only active in the channel in
which the frame was programmed. If the frame is
to be changed for all channels of an NCU, both [n]
and $P_NCBFRAME[n] have to be programmed.
The other channels must then still activate the
frame with, for example, G54. When writing a base
frame, the total base frame is calculated again.
$P_CHBFRAME[n]
Current channel basic frames
You can read and write the current channel basic
frame field elements via system variable
$P_CHBFRAME[n]. The resulting total base frame
is calculated by means of the write process in the
channel. When writing a base frame, the total base
frame is calculated again.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-259
6 Frames 11.026.9 NCU-global frames (SW 5 and higher) 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
$P_BFRAME
Current first basic frame in the channel
You can read and write the current basic frame with
array index 0, which applies for the channel, in the
parts program via the predefined frame variable
$P_BFRAME. The written basic frame is
immediately included in the calculation.
$P_BFRAME is identical to $P_CHBFRAME[0]. The
default is for the system variable to always have a
valid value. If there is no channel-specific base
frame, an alarm is issued at read/write: "Frame:
instruction not permissible".
$P_ACTBFRAME
Total basic frame
Variable $P_ACTBFRAME determines the chained
total basic frame. The variable can only be read.
$P_ACTBFRAME corresponds to
$P_NCBFRAME[0] : ... : $P_NCBFRAME[n] :
$P_CHBFRAME[0] : ... : $P_CHBFRAME[n].
Y BCS Y Y BOS
$P_ACTBFRAME
BOS
X BOS
$P_CHBFRAME[n], n programmable via $MC_MM_NUM_BASE_FRAMES
$P_CHBFRAME[0] = $P_BFRAME
$P_NCBFRAME[n], n programmable via $MN_MM_NUM_GLOBAL_BASE_FRAMES
X
$P_NCBFRAME[0]
X BCS
BOS = Basic origin system
BCS BCS = Basic coordinate system
$P-ACTBFRAME = $P_NCBFRAME[0] : $P_NCBFRAME[n] : $P_CHBFRAME[0] : $P_CHBFRAME[n]
$P_CHBFRMASK and $P_NCBFRMASK
Total basic frame
Via system variables $P_CHBFRMASK and
$P_NCBFRMASK, the user can select the basic frames
to be included in the calculation of the "total" basic frame.
The variables can only be programmed in the program
and read via OPI. The value of the variable is interpreted
as bit mask and determines which base frame field
element of $P_ACTBFAME is included in the calculation.
Siemens AG, 2002. All rights reserved
6-260 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.9 NCU-global frames (SW 5 and higher) 6
840D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
You can specify with $P_CHBFRMASK which channel-
specific base frames, and with $P_NCBFRMASK which
NCU-global base frames, are to be included in the
calculation.
By programming the variables the total base frame and
the total frame are calculated again. After a Reset is
performed, the basic setting value is
$P_CHBFRMASK = $MC_CHBFRAME_RESET_MASK and
$P_NCBFRMASK = $MN_NCBFRAME_RESET_MASK.
e.g.
$P_NCBFRMASK = 'H81' ; $P_NCBFRAME[0] : $P_NCBFRAME[7]
$P_CHBFRMASK = 'H11' ; $P_CHBFRAME[0] : $P_CHBFRAME[4]
$P_IFRAME
Current settable frame
You can read and write the current settable frame,
which applies in the channel, in the parts program
via the predefined frame variable $P_IFRAME. The
written settable frame is immediately included in the
calculation.
With NCU-global settable frames, the modified frame is
only active in the channel in which the frame was
programmed. If the frame is to be changed for all
channels of an NCU, both $P_UIFR[n] and $P_IFRAME
have to be programmed. The other channels must then
still activate the respective frame with, for example,
G54.
SW 6.1 and higher
Current system frames for
$P_TOOLFRAME TOROT and TOFRAME
SW 6.3 and higher
$P_WPFRAME Workpiece reference points
You can read and write the current system frame in
the parts program via these system variables.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-261
6 Frames 11.026.9 NCU-global frames (SW 5 and higher) 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
$P_PFRAME
Current programmable frame
$P_PFRAME is the programmable frame which results
from programming TRANS/ATRANS, G58/G59,
ROT/AROT, SCALE/ASCALE, MIRROR/AMIRROR or
from assigning CTRANS, CROT, CMIRROR, CSCALE
to the programmable frame.
Current, programmable frame variable that
establishes the reference between the settable zero
system (SZS) and the workpiece coordinate system
(WCS).
SW 6.3 and higher
Current system frame for $P_CYCFRAME Cycles
You can read and write the current system frame in
the parts program via this system variable.
$P_ACTFRAME
Current total frame
The current resulting total frame $P_ACTFRAME
now results from chaining all basic frames, the
current settable frame and the programmable frame.
The current frame is always updated if a frame
element is modified.
SW 6.3 and higher, $P_ACTFRAME corresponds to
$P_SETFRAME : $P_EXTFRAME : $P_PARTFRAME : $P_ACTBFRAME :
$P_IFRAME : $P_TOOLFRAME : $P_WPFRAME : $P_PFRAME : $P_CYCFRAME
SW 6.4 and higher, $P_ACTFRAME corresponds to
$P_PARTFRAME : $P_SETFRAME : $P_EXTFRAME: $P_ACTBFRAME :
$P_IFRAME : $P_TOOLFRAME : $P_WPFRAME : $P_PFRAME : $P_CYCFRAME
Siemens AG, 2002. All rights reserved
6-262 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
6 11.02 Frames 6.9 NCU-global frames (SW 5 and higher) 6
8 40D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Data management frames Input via program, e.g. Input via program, e.g.
$P_CHBFR=CTRANS(Z,10) $P_NCBFR=CTRANS(X,10) $P_UIFR[n]=CTRANS(X,10)
Channel-specific Input Input
system frames $P_CYCTFR via MMC via MMC
$P_WPFR
$P_TOOLFR
$P_PARTFR
$P_CHBFR[n] $P_NCBFR[n]
$P_EXTFR
Channel-specific NCU-global
$P_SETFR $P_UIFR[n]
NCU basic frames : frames
Activated via Activated via
G500, G54...G599 G500, G54...G599
Active total frame
$P_ACTFRAME = $P_PARTFRAM : $P_SETFRAME : : $P_EXTFRAME : $P_ACTRAME :
Input via program, e.g.
$P_NCBFRAME[1]=CTRANS(X,10)
$P_IFRAME : $P_TOOLFR :AME : : $P_WPF R A : ME : $P_PFRAME : $P_CYCFRAME
Input via program, e.g. Input via program, e.g.
$P_PFRAME=CTRANS(X,10) $P_IFRAME=CTRANS(X,10)
bzw. TRANS X10
Frame chaining
The current frame consists of the total basic frame,
the settable frame, the system frame and the
programmable frame according to the current total
frame mentioned above.
Frame chain
WCS
Frame for cycles,
programmable frame
SZS
System frame for TOROT
(TOFRAME), workpieces
G54 ... G599 settable frame,
channel-specific or NCU-global
BZS
Chained filed of basic frames,
channel-specific of NCU-global
Chained system frames for actual value setting,
scratching, external zero offset, PAROT
Handwheel (DRF) offset, override motion,
[external zero offset]
BCS
Kinematic transformation
MCS
Reference point offset
MCS = Machine Coordniate System BCS = Basic Coordinate System WCS = Workpiece Coordinate System
BZS = Basic Zero System SZS = Settable Zero System
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 6-263
6 Frames 11.026.9 NCU-global frames (SW 5 and higher) 6
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Siemens AG, 2002. All rights reserved
6-264 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7
Transformations
7.1 Three, four and five axis transformation: TRAORI........................................................ 7-266
7.1.1 Programming tool orientation ................................................................................. 7-269
7.1.2 Orientation axes reference – ORIWCS, ORIMCS .................................................. 7-274
7.1.3 Singular positions and how to handle them ............................................................ 7-275
7.1.4 Orientation axes (SW 5.2 and higher)..................................................................... 7-276
7.1.5 Cartesian PTP travel (from SW 5.2) ....................................................................... 7-279
7.1.6 Online tool length compensation (SW 6.4 and higher) ........................................... 7-284
7.2 Milling turned parts: TRANSMIT ................................................................................... 7-287
7.3 Cylinder surface transformation: TRACYL.................................................................... 7-290
7.4 Inclined axis: TRAANG ................................................................................................. 7-296
7.4.1 Inclined axis programming: G05, G07 (SW 5.3 and higher) ................................... 7-300
7.5 Constraints when selecting a transformation ................................................................ 7-302
7.6 Deselect transformation: TRAFOOF............................................................................. 7-304
7.7 Chained transformations ............................................................................................... 7-305
7.8 Switchable geometry axes, GEOAX.............................................................................. 7-308
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-265
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1 Three, four and five axis transformation: TRAORI
To obtain optimum cutting conditions when
Tool axis
machining surfaces with a three-dimensional curve,
it must be possible to vary the setting angle of the
tool.
The machine design to achieve this is stored in the
axis data.
Cardanic tool head
Three linear axes (X, Y, Z) and two orientation axes
define the setting angle and the operating point of
the tool here. One of the two orientation axes is
created as an inclined axis, in our example A' - in
many cases, placed at 45°.
ϕ
The axis sequence of the orientation axes and the
orientation direction of the tool are set up via the ,
A
machine data subject to the machine kinematics. In
Z Y
the examples shown here, you can see the C
arrangements in the CA machine kinematics
X
example!
Cardanic tool head, version 1
Siemens AG, 2002. All rights reserved
7-266 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
There are the following possible relationships:
A' is below angle ϕ to the X axis
B' is below angle ϕ to the Y axis
C' is below angle ϕ to the Z axis
Angle ϕ can be configured in the range 0° to +89° , A
via machine data. C
Depending on the orientation direction selected for
the tool, the active working plane (G17, G18, G19) ϕ
must be set in the NC program in such a way that
tool length compensation works in the direction of
tool orientation.
Cardanic tool head, version 2
Transformation with a swiveling linear axis
This is an arrangement with a moving workpiece and
a moving tool. Z
The kinematics consists of three linear axes
(X, Y, Z) and two orthogonally arranged rotary axes. A
The first rotary axis is moved, for example, over a
compound slide of two linear axes, the tool standing B Y
parallel to the third linear axis.
The second rotary axis turns the workpiece.
The third linear axis (swivel axis) lies in the X
compound slide plane.
The axis sequence of the rotary axes and the
orientation direction of the tool are set up via the
machine data subject to the machine kinematics.
There are the following possible relationships:
Axes: Axis sequences:
1st rotary axis A A B B C C
2nd rotary axis B C A C A B
Swiveled linear axis Z Y Z X Y X
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-267
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
3-axis and 4-axis transformations
3-axis and 4-axis transformations are special forms
of 5-axis transformations.
The user can configure two or three translatory axes
and one rotary axis. The transformations assume
that the rotary axis is orthogonal on the orientation
plane.
Tool orientation is only possible in the plane that is
perpendicular to the rotary axis. Transformation
supports machine types with a mobile tool and a
mobile workpiece.
Configuration and programming for 3-axis and
4-axis transformations are the same as for
5-axis transformations.
Programming
TRAORI(n)
TRAFOOF
Explanation of the commands
TRAORI Activates the first specified orientation transformation
TRAORI(n) Activates the orientation transformation specified by n
n The number of the transformation (n = 1 or 2), TRAORI(1) corresponds
to TRAORI
TRAFOOF Disable transformation
Additional notes
When the transformation is enabled, the positional
data (X, Y, Z) always relates to the tip of the tool.
Changing the position of the rotary axes involved in
the transformation causes so many compensating
movements of the remaining machine axes that the
position of the tool tip is unchanged.
Siemens AG, 2002. All rights reserved
7-268 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1.1 Programming tool orientation
5-axis programs are usually generated by CAD/CAM
systems and not entered at the control. So the
following explanations are directed mainly at the
programmers of postprocessors.
There are three options available when
programming tool orientation:
1. Programming the motion of the rotary axes. The
change of orientation always occurs in the basic
or machine coordinate system. The orientation
axes are traversed as synchronized axes.
2. Programming in Euler angles or RPY angles via
A2, B2, C2
or
Programming the direction vector via A3, B3, C3.
The direction vector points from the tool tip
towards the toolholder.
3. Programming via the lead angle LEAD and
the tilt angle TILT (face milling).
In all cases, orientation programming is only
permissible if an orientation transformation is active.
Without 5-axis transformation
With 5-axis transformation
Advantage: These programs can be transferred to
any machine kinematics.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-269
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Programming
G1 X Y Z A B C Programming the motion of the rotary axes.
G1 X Y Z A2= B2= C2= Programming in Euler angles
G1 X Y Z A3= B3= C3= Programming the direction vector
G1 X Y Z A4= B4= C4= Programming the surface normal vector at block start
G1 X Y Z A5= B5= C5= Programming the surface normal vector at end of block
LEAD Lead angle for programming tool orientation
TILT Tilt angle for programming tool orientation
Machine data can be used to switch between Euler
and RPY angles.
Programming in Euler angles
Z Z
The values programmed during orientation Z Y Z X
programming with A2, B2, C2 are interpreted as Y
Euler angles (in degrees).
X YY
With A2 = 90°
The orientation vector results from turning a rotating around
vector in the Z direction firstly with A2 around the the Z axis X
Basic setting X
Z axis, then with B2 around the new X axis and lastly Z
with C2 around the new Z axis. Y Z X
B2
In this case the value of C2 (rotation around the new Y With B2 = 45°
Z axis) is meaningless and does not have to be rotating aroundrotating X axis
programmed.
X Y
Siemens AG, 2002. All rights reserved
7-270 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Programming in RPY angles
Z Z
The values programmed during orientation Z Z Y
programming with A2, B2, C2 are interpreted as X
RPY angles (in degrees).
X Y B2
The orientation vector results from turning a vector in C2
Y
the Z direction firstly with C2 around the Z axis, then
X Basic setting
with B2 around the new Y axis and lastly with A2 X YZ Z Y
around the new X axis. With C2 = 90°
rotating around
X the Z axis
In contrast to Euler angle programming, A2 with B2 = +45°
all three values here have an effect on the With A2 = 30°
rotating around
rotating around rotating Y axis
orientation vector the rotating
X axis X Y
Programming the direction vector
Z
The components of the direction vector are
programmed with A3, B3, C3. The vector points
towards the toolholder; the length of the vector is
meaningless.
Vector components that have not been programmed Direction vector
are set equal to zero. C3 =...
X
Y
B3 =...
A3 =...
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-271
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Face milling
Face milling is used to machine curved surfaces of
any kind.
For this type of 3D milling, you require line-by-line
definition of 3D paths on the workpiece surface.
The tool shape and dimensions are taken into
account in the calculations that are normally
performed in CAM.
The fully calculated NC blocks are then read into the
control via postprocessors.
Surface description
The path curvature is described by surface normal
vectors with the following components:
A4, B4, C4 start vector at block start
A5, B5, C5 end vector at block end
If a block only contains the start vector, the surface
normal vector will remain constant throughout the
block.
A4
If a block only contains the end vector, interpolation B4
C4 A5
will run from the end value of the previous block via B5
large circle interpolation to the programmed end C5
value.
If both start and end vectors are programmed,
interpolation runs between the two directions, also
via large circle interpolation. This allows continuously
smooth paths to be be created.
In the initial setting, surface normal vectors –
whatever the active G17 to G19 level – point in the Z
direction.
The length of a vector is meaningless.
Vector components that have not been programmed
are set to zero.
Siemens AG, 2002. All rights reserved
7-272 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
With active ORIWCS (see following pages), the
surface normal vectors relate to the active frame and
also turn when the frame is turned.
The surface normal vector must be perpendicular to
the path tangent, within a limit value set via machine
data, otherwise an alarm will be output.
Programming the tool orientation with LEAD and TILT
TILT
The resultant tool orientation is determined from:
− the path tangent,
− the surface normal vector LEAD
− the lead angle LEAD
− the tilt angle TILT at end of block.
Explanation of the commands
LEAD Angle relative to the surface normal vector in the plane put up by the
path tangent and the surface normal vector
TILT Angle in the plane, perpendicular to the path tangent relative to the
surface normal vector
Behavior at inside corners (for 3D-tool
compensation)
If the block at an inside corner is shortened, the
resultant tool orientation is also achieved at end of
block.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-273
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1.2 Orientation axes reference – ORIWCS, ORIMCS
Programming
N.. ORIMCS
or
N.. ORIWCS
Explanation of the commands
ORIMCS Rotation in the machine coordinate system
ORIWCS Rotation in the workpiece coordinate system
Function
With orientation programming in the workpiece
coordinate system via Euler or RPY angles or the
orientation vector, ORIMCS/ORIWCS can be used
to adjust the course of the rotary motion.
Sequence
With ORIMCS, the movement executed by the tool
is dependent on the machine kinematics. With an
orientation change with a fixed tool tip, interpolation
between the rotary axis positions is linear.
With ORIWCS, the tool movement is not dependent
on the machine kinematics. With an orientation Plane created from
starting and end
change with a fixed tool tip, the tool moves in the vectors
plane set up by the start and end vectors.
Vector at
beginning of
block
Vector at
end of block
Siemens AG, 2002. All rights reserved
7-274 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Additional notes
ORIWCS is the basic setting. If it is not immediately
obvious with a 5-axis program which machine it should
run on, always choose ORIWCS. Which movements
the machine actually executes depend on the machine
kinematics.
With ORIMCS, you can program actual machine
movements, for example, to avoid collisions with
devices, etc.
Machine data $MC_ORI_IPO_WITH_G_CODE
specifies the active interpolation mode:
ORIMCS/ORIWCS or ORIMACHAX/ORIVIRTAX
(see Subsection 7.1.4).
7.1.3 Singular positions and how to handle them
Notes on ORIWCS:
Orientation movements in the singular setting area
of the 5-axis machine require vast movements of the
machine axes. (For example, with a rotary swivel
head with C as the rotary axis and A as the swivel
axis, all positions with A = 0 are singular.)
To avoid overloading the machine axes, the velocity
control vastly reduces the tool path velocity near the
singular positions.
With machine data
$MC_TRAFO5_NON_POLE_LIMIT
$MC_TRAFO5_POLE_LIMIT
the transformation can be parameterized in such a
way that orientation movements close to the pole are
put through the pole and rapid machining is possible.
Note on SW 5.2:
As from SW5.2, singular positions will only be
handled by MD $MC_TRAFO5_POLE_LIMIT
(see Description of Functions Part 3, Sub-
section 2.8.4).
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-275
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1.4 Orientation axes (SW 5.2 and higher)
Programming
N.. ORIEULER or ORIRPY
or
N.. ORIVIRT1 or ORIVIRT2
N.. G1 X Y Z A2= B2= C2=
Explanation of the commands
ORIEULER Orientation programming using Euler angles
ORIRPY Orientation programming using RPY angles
ORIVIRT1 Orientation programming using virtual orientation axes
(definition 1), definition according to MD $MC_ORIAX_TURN_TAB_1
ORIVIRT2 Orientation programming using virtual orientation axes
(definition 2), definition according to MD $MC_ORIAX_TURN_TAB_2
G1 X Y Z A2= B2= C2= Angle programming of virtual axes
Programming
N.. ORIAXES or ORIVECT
N.. G1 X Y Z A B C
Explanation of the commands
ORIAXES Linear interpolation of orientation axes
ORIVECT Large circle interpolation
ORIMCS Rotation in the machine coordinate system
For description, see Subsection 7.1.2
ORIWCS Rotation in the workpiece coordinate system
For description, see Subsection 7.1.2
G1 X Y Z A B C Programming the machine axis position
Function
The orientation axis function describes the
orientation of the tool in space. This introduces an
additional third degree of freedom that describes the
rotation around itself. This is necessary for 6-axis
transformations.
Siemens AG, 2002. All rights reserved
7-276 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
MD $MC_ORI_DEF_WITH_G_CODE specifies how the
programmed angles A2, B2, C2 are defined:
The definition is made according to MD
$MC_ORIENTATION_IS_EULER
(default) or
the definition is made according to G_group 50
(ORIEULER, ORIRPY, ORIVIRT1, ORIVIRT2).
MD $MC_ORI_IPO_WITH_G_CODE specifies which
interpolation mode is active:
ORIWCS/ORIMCS or ORIAXES/ORIVECT.
JOG mode
Interpolation for orientation angles in this mode of
operation is always linear. During continuous and
incremental traversal via the traversing keys, only
one orientation axis can be traversed. Orientation
axes can be traversed simultaneously using the
handwheels.
For manual travel of the orientation axes, the
channel-specific feed override switch or the rapid
traverse override switch work at rapid traverse
override.
A separate velocity setting is possible with the
following machine data:
$MC_JOG_VELO_RAPID_GEO
$MC_JOG_VELO_GEO
$MC_JOG_VELO_RAPID_ORI
$MC_JOG_VELO_ORI
SW 6.3 and higher
In JOG mode, the cartesian manual travel function
can, for SINUMERIK 840D with the
"Handling transformation package" and for
Sinumerik 810D powerline from SW 6.1
set up separately the translation of the geometry
axes in the reference systems MCS, WCS and TCS.
Reference notes:
SINUMERIK 840D/FM-NC Description of Functions
(Part 3), "Handling transformation package".
/FB/ F2, 3-axis to 5-axis transformations
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-277
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Feed programming
FORI1 Feed for swiveling the orientation vector on the large circle
FORI2 Feed for the overlaid rotation around the swiveled orientation vector
With orientation movements, the programmable feed
corresponds to an angular velocity [degrees/min].
Effectiveness of the feed via G code:
When programming ORIAXES, the feed for an
orientation axis can be limited via the FL[ ]
instruction (feed limit).
When programming ORIVECT, the feed must be
programmed with FORI1 or FORI2. FORI1 and
FORI2 must only be programmed once in the NC
block. Traversal always takes the shortest path
during this programming.
The smallest feed always operates for the overlaid
motion of turning and swiveling. With orientation
movements, the feed corresponds to an angular
velocity [degrees/min].
If geometry axes and orientation axes traverse a
common path, the traversing movement is
determined from the smallest feed.
Siemens AG, 2002. All rights reserved
7-278 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1.5 Cartesian PTP travel (from SW 5.2)
Programming
N.. TRAORI
N.. STAT=`B10` TU=`B100` PTP
N.. CP
Explanation of the commands
PTP Point to Point (point to point movement)
The movement is executed as a synchronized axis movement; the slowest axis
involved in the movement is the dominating axis for the velocity.
CP Continuous path (path motion)
The movement is executed as cartesian path motion
STAT= Position of the articulated joints; this value is dependent on the transformation.
TU= TURN information
This makes it possible to clearly approach axis angles between -360 degrees and
+360 degrees.
Function
This function can be used to program a position in a
cartesian coordinate system, however, the
movement of the machine occurs in the machine
coordinates.
The function can be used, for example, when
changing the position of the articulated joint, if the
movement runs through a singularity.
Note:
The function is only useful in conjunction with an
active transformation. Furthermore, "PTP travel" is
only permissible in conjunction with G0 and G1.
Sequence
The commands PTP and CP effect the changeover
between cartesian traversal and traversing the
machine axes. These are modal. CP is the default
setting.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-279
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Programming the position (STAT=)
A machine position is not uniquely determined just
by positional data with cartesian coordinates and the
orientation of the tool. Depending on the kinematics
involved, there can by as many as eight different and
crucial articulated joint positions. These are specific
to the transformation. To be able to uniquely convert
a cartesian position into the axis angle, the position
of the articulated joints must be specified with the
command STAT=. The "STAT" command contains a
bit for each of the possible positions as a binary
value.
Reference notes:
The various transformations are included in the
document:
SINUMERIK 840D/FM-NC Description of Functions
(Part 3), "Handling transformation package".
The positional bits to be programmed for "STAT" are
included in the document:
SINUMERIK 840D/FM-NC Description of Functions
(Part 3), "3-axis to 5-axis transformation".
Programming the axis angle (TU=)
To be able to clearly approach by axis angles < ±360
degrees, this information must be programmed
using the command "TU=".
The command is non-modal.
The axes traverse by the shortest path:
• when no TU is programmed for a position
• with axes that have a traversing range > ±360
degrees
Siemens AG, 2002. All rights reserved
7-280 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
S tarting position
Example:
T he target position shown in the diagram can be
approached in the negative or positive direction. The
negative
direction is programmed under the address A1. direction
positive
A 1=225°, TU=bit 0, → positive direction direction
A1=−135°, TU=bit 1, → negative direction
Target position
Smoothing between CP and PTP motion
A programmable transition rounding between the
blocks is possible with G641.
T he size of the rounding area is the path in mm or
inch, from which or to which the block transition is to
be rounded. The size must be specified as follows:
• for G0 blocks with ADISPOS
• for all the other motion commands with ADIS.
T he path calculation corresponds to considering of
the F addresses for non-G0 blocks. The feed is kept
to the axes specified in FGROUP(..).
F eed calculation:
F or CP blocks, the cartesian axes of the basic
coordinate system are used for the calculation.
For PTP blocks, the corresponding axes of the
machine coordinate system are used for the
calculation.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-281
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Additional notes
Mode change
The "Cartesian PTP travel" function is only useful in
the AUTO and MDA modes of operation. When
changing the mode to JOG, the current setting is
retained.
When the G code PTP is set, the axes will traverse
in MCS. When the G code CP is set, the axes will
traverse in WCS.
P ower On / Reset
After a power ON or after a Reset, the setting is
dependent on the machine data
$MC_GCODE_RESET_VALUES[48]. The default traversal
mode setting is "CP".
Repositioning
I f the function "Cartesian PTP travel" was set during
the interruption block, PTP can also be used for
repositioning.
O verlaid movements
DRF offset or external zero offset are only possible
to a limited extent in cartesian PTP travel. When
changing from PTP to CP motion, there must be no
overrides in the BCS.
Siemens AG, 2002. All rights reserved
7-282 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Programming example Elbow up
A1
Y1 Z1
Elbow down
X1
N10 G0 X0 Y-30 Z60 A-30 F10000 S tarting position
→ Elbow up
N20 TRAORI(1) Transformation ON
N30 X1000 Y0 Z400 A0
N40 X1000 Z500 A0 STAT=´B10´ TU=´B100´ PTP R eorientation without
transformation
→ Elbow down
N 50 X1200 Z400 CP Transformation active again
N60 X1000 Z500 A20
N70 M30
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-283
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
7.1.6 Online tool length compensation (SW 6.4 and higher)
Programming
N.. TRAORI
N.. TOFFON(X,25)
N.. WHEN TRUE DO $AA_TOFF[X]
Explanation of the commands
TOFFON Tool Offset ON (activate online tool length compensation)
When activating, an offset value can be specified for the relevant direction of
compensation and this is immediately recovered.
TOFFOF Tool Offset OF (reset online tool length compensation)
The relevant compensation values are reset and a preprocessing stop is initiated.
X, Y, Z, Direction of compensation for the specified offset value
Function
Use the system variable $AA_TOFF[ ] to overlay the
effective tool lengths in accordance with the three
tool directions three-dimensionally in real time.
The three geometry axis identifiers are used as the
index. This defines the number of active directions of
compensation by the geometry axes active at the
same time.
All the overrides can be active simultaneously.
Application
T he online tool length compensation function can be
used for:
• orientation transformation TRAORI
• orientable toolholder TCARR
Note:
Online tool length compensation is an option, that
first has to be enabled. This function is only useful in
conjunction with an active orientation transformation
or an active orientable toolholder.
Siemens AG, 2002. All rights reserved
7-284 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations7.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Additional notes
Block preparation
During block preparation in preprocessing, the
current tool length offset active in the main run is
also taken into consideration. To allow extensive use
to be made of the maximum permissible axis
velocity, it is necessary to stop block preparation
with a STOPRE preprocessing stop while a tool
offset is set up.
T he tool offset is then always known at the time of
preprocessing if tool length compensations can no
longer be changed after program startup, or if,
following a change to the tool length compensations,
more blocks were executed than the IPO buffer
between preprocessing and main run can accept.
V ariable $AA_TOFF_PREP_DIFF
T he size of the difference between the current
compensation active in the interpolator and the
compensation active at the time the block was
prepared, can be queried in the
$AA_TOFF_PREP_DIFF[ ] variable.
Adjusting machine data and setting data
The following machine data is available for online
tool length compensation:
• MD 20610: ADD_MOVE_ACCEL_RESERVE
Reserve for velocity planning
• MD 21190: TOFF_MODE The content of the
system variable $AA_TOFF[ ] is recovered or
integrated as an absolute value.
• MD 21194: TOFF_VELO Velocity of the online
tool length compensation
• MD 21196: TOFF_ACCEL Acceleration of the
online tool length compensation
Setting data for presetting limit values
• SD 42970: TOFF_LIMIT Upper limit of the tool
length compensation value
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-285
7 Transformations 11.027.1 Three, four and five axis transformation: TRAORI 7
840D 840Di
NCU 572
NCU 573
Programming example
T ool length compensation selection
MD 21190: TOFF_MODE =1 ; Absolute values are approached
MD 21194: TOFF_VELO[0] =1000
M D 21196: TOFF_VELO[1] =1000
M D 21194: TOFF_VELO[2] =1000
MD 21196: TOFF_ACCEL[0] =1
MD 21196: TOFF_ACCEL[1] =1
MD 21196: TOFF_ACCEL[2] =1
N 5 DEF REAL XOFFSET
N10 TRAORI(1) ; Transformation ON
N 20 TOFFON(Z) ; Activation of online tool length offset
; for the Z tool direction
N30 WHEN TRUE DO $AA_TOFF[Z] = 10 ; For the Z tool direction, a tool length
G4 F5 ; offset of 10 is interpolated
. ..
N40 TOFFON(X) ; Activation of online tool length offset
; for the X tool direction
N50 ID=1 DO $AA_TOFF[X] = $AA_IW[X2] ; For the X tool direction, an offset is
G4 F5 ; executed subject to the position of axis
; X2
. ..
N100 XOFFSET = $AA_TOFF_VAL[X] ; Assign current offset in X direction
N120 TOFFON(X, -XOFFSET) ; For the X tool direction, the tool length
G4 F5 ; offset will be returned to 0 again
Tool length compensation deselection
N10 TRAORI(1) ; Transformation ON
N20 TOFFON(X) ; Activating the Z tool direction
N 30 WHEN TRUE DO $AA_TOFF[X] = 10 ; For the X tool direction, a tool length
G4 F5 ; offset of 10 is interpolated
...
N80 TOFFOF(X) ; Positional offset of the X tool direction
; is deleted: ...$AA_TOFF[X] = 0
; No axis is traversed
; To the current position in WCS, the
; positional offset is added in accordance
; with the current orientation
References
/FB/ F2, 3-axis to 5-axis transformations
Siemens AG, 2002. All rights reserved
7-286 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.2 Milling turned parts: TRANSMIT 7
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
7 .2 Milling turned parts: TRANSMIT
Programming
TRANSMIT or TRANSMIT(n)
TRAFOOF
Explanation of the commands
T RANSMIT Activates the first specified Transmit function
T RANSMIT(n) Activates the n-th specified Transmit function; the maximum for n is 2
(TRANSMIT(1) corresponds to TRANSMIT).
TRAFOOF Disables an active transformation
A n active TRANSMIT transformation is also disabled
if one of the remaining transformations is activated
in the particular channel (e.g. TRACYL, TRAANG,
TRAORI).
T he TRANSMIT function facilitates the following
performance:
• Machining the end face of turned parts clamped
for turning (holes, contours).
• A cartesian coordinate system can be used to
program this machining.
• The control transforms the programmed
traversing movements of the cartesian coordinate
system to the traversing movements of the real
machine axes (default situation):
– Rotary axis
– Infeed axis perpendicular to the rotary axis
– Longitudinal axis parallel to the rotary axis
The linear axes are positioned perpendicular
to one another.
• Tool center offset relative to the turning center is
permissible.
• The velocity control considers the limitations defined
for rotary motion.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-287
7 Transformations 11.02 7.2 Milling turned parts: TRANSMIT 7
8 40D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Rotary axis
The rotary axis cannot be programmed, as it is
assigned by a geometry axis and is thus not directly
programmable as a channel axis.
Pole
SW 3.x and lower
Traversing through the pole (the origin of the
cartesian coordinate system) is prevented. A
movement that runs through the pole stops at the
pole and an alarm is output. With milling center
offset, movement correspondingly stays at the edge
of the area not to be approached.
SW 4 and higher
There are two options for traversing through the
pole:
1. Traverse only the linear axis
2. Traverse to the pole, rotate the rotary axis at the
pole and traveling away from the pole
Make the selection using MD 24911 and 24951.
References
/FB/ M1 Kinematic transformations
Siemens AG, 2002. All rights reserved
7-288 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.2 Milling turned parts: TRANSMIT 7
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Programming example
Y
Z
N10 T1 D1 G54 G17 G90 F5000 G94 Tool selection
N20 G0 X20 Z10 SPOS=45 Approach initial position
N30 TRANSMIT Activate the Transmit function
N40 ROT RPL=–45 Adjust the frame
N50 ATRANS X–2 Y10
N60 G1 X10 Y–10 G41 OFFN=1 Square roughing; allowance 1mm
N70 X–10
N80 Y10
N90 X10
N100 Y–10
N110 G0 Z20 G40 OFFN=0 Tool change
N120 T2 D1 X15 Y–15
N130 Z10 G41
N140 G1 X10 Y–10 Square finishing
N150 X–10
N160 Y10
N170 X10
N180 Y–10
N190 Z20 G40 Deselect frame
N200 TRANS
N210 TRAFOOF
N220 G0 X20 Z10 SPOS=45 Approach initial position
N230 M30
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-289
X
7 Transformations 11.02 7.3 Cylinder surface transformation: TRACYL 7
8 40D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
7.3 Cylinder surface transformation: TRACYL
Programming
TRACYL(d) or TRACYL(d,t)
TRAFOOF
Explanation of the
commands
TRACYL(d) Activates the first TRACYL function specified in the channel machine
data. d is the parameter for the working diameter.
TRACYL(d,n) Activates the n-th TRACYL function specified in the channel machine
data. The maximum for n is 2, TRACYL(d,1) corresponds to TRACYL(d).
d Value for the working diameter. The working diameter is double the
distance between the tool tip and the turning center.
TRAFOOF Transformation OFF (BCS and MCS are once again identical).
OFFN Offset contour normal: Distance of the groove side from the programmed
reference contour
An active TRACYL transformation is also disabled if
one of the remaining transformations is activated in
the particular channel (e.g. TRANSMIT, TRAANG,
TRAORI).
Function
Cylinder peripheral curve transformation
TRACYL X
The TRACYL cylinder peripheral curve
transformation facilitates the following performance:
Machining
• longitudinal grooves on cylindrical structures,
Y
• transverse grooves on cylindrical structures,
• grooves in any direction on cylindrical structures.
T he progression of the grooves is programmed in Z
relation to the handled, even, peripheral surface of
the cylinder. W orkpiece coordinate system
Siemens AG, 2002. All rights reserved
7-290 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.3 Cylinder surface transformation: TRACYL 7
840D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
T here are two instances of cylinder surface
coordinate transformation:
• without groove side offset (TRAFO_TYPE_n=512)
• with groove side offset (TRAFO_TYPE_n=513)
Y or CM
Without groove side offset:
ASM
The control transforms the programmed traversing
movements of the cylinder coordinate system to the Z or ZM
traversing movements of the real machine axes: XM
– Rotary axis
– Infeed axis perpendicular to the rotary axis
– Longitudinal axis parallel to the rotary axis.
T he linear axes are positioned perpendicular to one
another. The infeed axis cuts the rotary axis.
Machine coordinate system
W ith groove side offset:
Kinematics as above, but in addition
– longitudinal axis parallel to the peripheral direction.
Y or CM
The linear axes are positioned perpendicular to one
Z or ZM
another. YM
ASM
The velocity control considers the limitations defined X M
for rotary motion.
M achine coordinate system
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-291
7 Transformations 11.02 7.3 Cylinder surface transformation: TRACYL 7
8 40D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Groove cross section
I n axis configuration 1, grooves alongside the rotary
axis are only limited in parallel if the groove width
corresponds exactly to the tool radius.
Grooves parallel to the circumference (transverse
grooves) are not parallel at the start and at the end.
Longitudinal Transverse Longitudinal groove
groove groove limited in parallel
with groove wall
compensation
without groove wall TRAFO_TYPE_n = 513
compensation
TRAFO_TYPE_n = 512
Offset contour normal OFFN (513)
To mill grooves with TRACYL, in
• the parts program the groove center line
• is programmed via OFFN half the width of the
groove. Programmed
OFFN is only effective when tool radius compensation OFFN contour
is selected, to avoid damaging the groove side.
Furthermore, OFFN>=tool radius should also be
the case to stop damage occurring to the
opposite side of the groove.
A parts program for milling a groove generally
comprises the following steps:
1. Select tool
2. Select TRACYL
3. Select suitable coordinate offset (frame)
4. Position
5. Program OFFN
6. Select TRC
7. Approach block (position TRC and approach
groove side)
8. Groove center line contour
9. Deselect TRC
10. Retraction block (retract TRC and move away
from groove side)
11. Position
12. TRAFOOF
13. Re-select original coordinate shift (frame)
Siemens AG, 2002. All rights reserved
7-292 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.3 Cylinder surface transformation: TRACYL 7
8 40D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Special features:
• TRC selection:
TRC is not programmed in relation to the groove
side, but relative to to the programmed groove
center line. To prevent the tool traveling to the left
of the groove side, G42 is entered (instead of
G41). You avoid this if in OFFN, the groove width
is entered with a negative sign.
• OFFN acts differently with TRACYL than it does
without TRACYL. As, even without TRACYL,
OFFN is included when TRC is active, OFFN
should be reset to zero after TRAFOOF.
• It is possible to change OFFN within a parts
program. This could be used to shift the groove
center line from the center (see diagram).
• Guiding grooves:
TRACYL does not create the same groove for
guiding grooves as it would be with a tool with the
diameter producing the width of the groove.
It is basically not possible to create the same
groove side geometry with a smaller cylindrical
tool as it is with a larger one.
TRACYL minimizes the error. To avoid problems
of accuracy, the tool radius should only be slightly
smaller than half the groove width.
Note:
OFFN and TRC
• With TRAFO_TYPE_n = 512, the value acts
under OFFN as an allowance for TRC.
• With TRAFO_TYPE_n = 513, half the groove
width is programmed in OFFN. The contour is
retracted with OFFN-TRC.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-293
7 Transformations 11.02 7 .3 Cylinder surface transformation: TRACYL 7
840D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
For cylinder peripheral curve transformation with
groove side compensation, the axis used for
compensation should be positioned at zero (y=0), so
that the groove centric to the programmed groove
center line is finished.
Rotary axis
The rotary axis cannot be programmed, as it is
assigned by a geometry axis and is thus not directly
programmable as a channel axis.
Axis utilization
T he following axes cannot be used as a positioning
axis or a reciprocating axis:
• the geometry axis in the peripheral direction of
the cylinder peripheral surface (Y axis)
• the additional linear axis for groove side
compensation (Z axis).
Tool definition
The following example is suitable for testing the
parameterization of the TRACYL cylinder
transformation:
Tool parameters Meaning Comment
number (DP)
$TC_DP1[1,1]=120 Tool type Milling cutter
$TC_DP2[1,1]=0 Tool point direction For turning tools only
Geometry Tool length compensation
$TC_DP3[1,1]=8. Length compensation vector Calculation depending
$TC_DP4[1,1]=9. on type and plane
$TC_DP5[1,1]=7.
Geometry Radius
$TC_DP6[1,1]=6. Radius Tool radius
$TC_DP7[1,1]=0 Slot width b for slotting saw, rounding radius
for milling tools
$TC_DP8[1,1]=0 Overhang k For slotting saw only
$TC_DP9[1,1]=0
$TC_DP10[1,1]=0
$TC_DP11[1,1]=0 Angle for cone milling tools
Wear Tool length and radius compensation
$TC_DP12[1,1]=0 Remaining parameters to $TC_DP24=0 Base dimensions/
adapter
Siemens AG, 2002. All rights reserved
7-294 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.3 Cylinder surface transformation: TRACYL 7
8 40D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Programming example
X
Y
Z
N 10 T1 D1 G54 G90 F5000 G94 T ool selection, clamping compensation
N 20 SPOS=0 A pproach initial position
N30 G0 X25 Y0 Z105 CC=200
N 40 TRACYL (40) Enable cylinder peripheral curve
transformation
N50 G19 Plane selection
M aking a hook-shaped groove:
N60 G1 X20 I nfeed tool to groove base
N70 OFFN=12 Define 12mm groove side spacing
relative to groove center line
N80 G1 Z100 G42 Approach right side of groove
N90 G1 Z50 Groove cut parallel to cylinder axis
N 100 G1 Y10 Groove cut parallel to circumference
N110 OFFN=4 G42 Approach left side of the groove; define
4mm groove side spacing relative to the
groove center line
N120 G1 Y70 G roove cut parallel to circumference
N130 G1 Z100 Groove cut parallel to cylinder axis
N140 G1 Z105 G40 Return from groove side
N150 G1 X25 Retraction
N160 TRAFOOF
N170 G0 X25 Y0 Z105 CC=200 Approach initial position
N180 M30
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-295
7 Transformations 11.02 7 .4 Inclined axis: TRAANG 7
8 40 D 810D 840Di
NCU 572
NCU 573
7 .4 Inclined axis: TRAANG
Programming
T RAANG(α) or TRAANG(α,n)
TRAFOOF
Explanation of the commands
TRAANG If angle α is omitted or zero is entered, the
transformation is activated with the
parameterization of the previous selection.
The default selection according to the
machine data applies for the initial
selection.
TRAANG(α) Activates the first specified inclined axis
transformation
TRAANG(α,n) A ctivates the n-th specified transformation
Inclined axis. the maximum for n is 2.
TRAANG(α,1) corresponds to TRAANG(α).
α Angle of the inclined axis
TRAFOOF T ransformation OFF
If α (angle) is omitted or zero is entered, the
transformation is activated with the parameterization
of the previous selection. The default selection
according to the machine data applies for the initial
selection. (response up to SW < 6.4, for later
versions, see below).
An active TRAANG transformation is also disabled if
one of the remaining transformations is activated in the
particular channel.
(e.g. TRACYL, TRANSMIT, TRAORI).
Siemens AG, 2002. All rights reserved
7-296 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.4 Inclined axis: TRAANG 7
840D 810D 840Di
NCU 572
NCU 573
( response from SW < 6.4)
If α (angle) is omitted (e.g. TRAANG(), TRAANG(,n)),
the transformation is activated with the parameterization
of the previous selection. The default selection
according to the machine data applies for the initial
selection.
A n angle α = 0 (e.g. TRAANG(0), TRAANG(0,n)) is
a valid parameter setting and no longer corresponds
to omitting the parameter as it did in former versions.
Permissible values for α are:
-90 degrees < α < + 90 degrees
Function
The inclined axis function is intended for grinding MU
α
technology and facilitates the following performance: X
• Machining with an oblique infeed axis
• A cartesian coordinate system can be used for
programming. Grinding
wheel
• The control transforms the programmed
traversing movements of the cartesian coordinate
Z MZ
system to the traversing movements of the real C AS
machine axes (default situation): inclined infeed Workpiece
axis.
The following machining operations are possible:
1. longitudinal grinding 3
2. face grinding
1
3. grinding a specific contour
2
4. oblique plunge-cut grinding
4
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-297
7 Transformations 11.02 7.4 Inclined axis: TRAANG 7
840 D 8 10D 840Di
NCU 572
NCU 573
The following settings are defined in machine data:
• the angle between a machine axis and the
oblique axis
• the position of the zero point of the tool relative to
the origin of the coordinate system specified by
the "inclined axis" function
• the velocity reserve held ready on the parallel
axis for the compensating movement.
• the axis acceleration reserve held ready on
the parallel axis for the compensating movement.
Axis configuration
To be able to program in the cartesian coordinate
system, the control must be told the relationship
between this coordinate system and the actually
existing machine axes (MU, MZ):
• Geometry axes designation
• Assignment of geometry axes to channel axes
– general situation (inclined axis not active)
– inclined axis active
• Assignment of channel axes to machine axis
numbers
• Spindle identification
• Machine axis name assignment.
Apart from "inclined axis active", the procedure
corresponds to the procedure for normal axis
configuration.
Siemens AG, 2002. All rights reserved
7-298 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.4 Inclined axis: TRAANG 7
8 40D 810D 840Di
NCU 572
NCU 573
Programming example
MU
α
X
Grinding
wheel
C Z AS MZ
Workpiece
N 10 G0 G90 Z0 MU=10 G54 F5000 -> Tool selection, clamping compensation
- > G18 G64 T1 D1 P lane selection
N20 TRAANG(45) Enable inclined axis transformation
N30 G0 Z10 X5 Approach initial position
N40 WAITP(Z) Enable axis for reciprocation
N 50 OSP[Z]=10 OSP2[Z]=5 OST1[Z]=–2 -> Reciprocation, until dimension reached
- > OST2[Z]=–2 FA[Z]=5000 (for reciprocation, see chapter 9)
N60 OS[Z]=1
N70 POS[X]=4.5 FA[X]=50
N 80 OS[Z]=0
N90 WAITP(Z) Enable reciprocating axes as positioning
axes
N100 TRAFOOF Switch off transformation
N110 G0 Z10 MU=10 Retraction
N120 M30
-> program in a single block
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-299
7 Transformations 11.02 7 .4 Inclined axis: TRAANG 7
840 D 810D 840Di
NCU 572
NCU 573
7.4.1 Inclined axis programming: G05, G07 (SW 5.3 and higher)
Programming
G07
G05
Explanation of the commands
G 07 Approach starting position
G05 A ctivates oblique plunge-cutting
The commands G07/G05 are used to make it easier
to program the inclined axes.
Positions can be programmed and displayed in the
cartesian coordinate system. Tool compensation and
zero offset are included in cartesian coordinates. After
the angle for the inclined axis is programmed in the NC-
program, the starting position can be approached (G07)
and then the oblique plunge-cutting (G05) performed.
In Jog-mode, the movement of the grinding wheel
can either be cartesian or in the direction of the
inclined axis (the display stays cartesian).
All that moves is the real U-axis, the Z-axis display is
updated.
• In jog-mode, repos-offsets must be returned
using cartesian coordinates.
• In jog-mode with active "PTP-travel", the
cartesian operating range limit is monitored for
overtravel and the relevant axis is braked
beforehand. If "PTP-travel" is not active, the axis
can be traversed right up to the operating range
limit.
References: /FB2/ F2: 3-5-axis transformation,
Chapter 2 "Cartesian PTP-travel".
Siemens AG, 2002. All rights reserved
7-300 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.4 Inclined axis: TRAANG 7
840D 810D 840Di
NCU 572
NCU 573
Programming example
U
α
X
N50
N60
Grinding
wheel
C Z AS
Workpiece
N.. P rogram angle for inclined axis
N20 G07 X70 Z40 F4000 A pproach starting position
N30 G05 X70 F100 Oblique plunge-cutting
N40 ...
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-301
7 Transformations 11.02 7.5 Constraints when selecting a transformation 7
840 D 810D 8 40Di
NCU 572
NCU 573
7.5 Constraints when selecting a transformation
T ransformations can be selected via a parts
program or MDA. Please note the following
• No intermediate movement block is inserted
(chamfer/radii).
• Spline block sequences must be excluded; if not,
a message is displayed.
• Fine tool compensation must be deselected
(FTOCOF); if not a message is displayed.
• Tool radius compensation must be deselected
(G40); if not a message is displayed.
• The control adopts an activated tool length
compensation into the transformation.
• The control deselects the current frame active
before the transformation.
• The control deselects an active operating range
limit for axes affected by the transformation
(corresponds to WALIMOF).
• Protection zone monitoring is deselected.
• Continuous-path mode and smoothing are
interrupted.
• DRF offsets in the axes involved in the
transformation must not change between
processing in preprocessing and in main run
(SW 3 and earlier).
• All the axes specified in the machine data must
be synchronized relative to a block.
• Axes that are exchanged are exchanged back; if
not, a message is displayed.
• A message is output for dependent axes.
Tool change
A tool change is only permissible if tool radius
compensation is deselected.
A change of tool length compensation and a tool
radius compensation selection/deselection must not
be programmed in the same block.
Siemens AG, 2002. All rights reserved
7-302 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.5 Constraints when selecting a transformation 7
840D 810D 8 40Di
NCU 572
NCU 573
F rame change
All instructions that only relate to the basic
coordinate system are legal (frame, tool radius
compensation). However, a frame change with G91
(incremental dimension) – unlike with an inactive
transformation – is not handled separately. The
increment to be traveled is evaluated in the
workpiece coordinate system of the new frame –
regardless of which frame was effective in the
previous block.
Exclusions
Axes affected by the transformation cannot be used
• as the preset axis (alarm)
• for approaching a checkpoint (alarm)
• for referencing (alarm).
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-303
7 Transformations 11.02 7 .6 Deselect transformation: TRAFOOF 7
840 D 810D 8 40Di
NCU 572
NCU 573
7.6 Deselect transformation: TRAFOOF
Programming
T RAFOOF
E xplanation of the commands
TRAFOOF Disables all the active transformations/frames
Function
The TRAFOOF command disables all the active
transformations and frames.
F rames required after this must be activated by
renewed programming.
P lease note the following:
T he same restrictions as for selection are applicable to
deselecting the transformation (see previous section
"Constraints when selecting a transformation").
Siemens AG, 2002. All rights reserved
7-304 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.7 Chained transformations 7
8 40D 810D 8 40Di
NCU 572
NCU 573
7 .7 Chained transformations
As from SW 5, two transformations can always be
enabled in succession (chained), so that the motion
components for the axes from the first transformation
are the input data for the chained second
transformation. The motion components from the
second transformation act on the machine axes.
• In SW 5, the chain can consist of two
transformations.
• The second transformation must be "inclined
axis" (TRAANG).
• Possible first transformations include:
- orientation transformations (TRAORI),
incl. universal milling head
- TRANSMIT
- TRACYL
- TRAANG.
Applications
- Grinding contours that have been programmed as
the surface line of a cylinder development
(TRACYL) with an obliquely positioned grinding
wheel, e.g. tool grinding.
- Finishing a contour generated with TRANSMIT that
is not round with an obliquely positioned grinding
wheel.
It is a condition of using the activate command for a
chained transformation that the individual
transformations to be chained and the chained
transformation to be activated are defined by the
machine data.
The constraints and special cases specified in the
individual descriptions for the transformations must
also be observed when they are used within a chain.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-305
7 Transformations 11.02 7.7 Chained transformations 7
840 D 8 10D 8 40Di
NCU 572
NCU 573
Additional notes
Information on configuring the machine data of the
transformations can be found in the descriptions of
the functions: M1 and F2.
Machine manufacturer (MH7.1)
Take note of information provided by the machine
manufacturer on any transformations predefined by
the machine data.
Transformations and chained transformations are
options. The current catalog always provides
information about the availability of specific
transformations in the chain in specific controls.
The commands available for chained
transformations are:
TRACON to activate and
TRAFOOF to deactivate.
Activate
Programming
TRACON(trf, par) This activates a chained transformation.
Explanation of the parameters
trf The number of the chained transformation:
0 or 1 for the first/only chained
transformation.
If nothing is programmed in this position, this
means the same as specifying the value 0 or
1, i.e. the first/only transformation is
activated.
2 for the second chained transformation.
(values not equal to 0–2 generate an error
alarm).
Siemens AG, 2002. All rights reserved
7-306 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.7 Chained transformations 7
8 40D 8 10D 840Di
NCU 572
NCU 573
par one or more parameters separated by a
comma for the transformations in the
chain expecting parameters. For
example, the angle of the inclined axis. If
parameters are not set, the defaults or
the parameters last used take effect.
Commas must be used to ensure that the
specified parameters are evaluated in the
sequence in which they are expected, if
defaults are to act for previous
parameters. It is particularly important
when specifying at least one parameter
that this is preceded by a comma, even if
it is not necessary to specify trf, thus for
example TRACON( , 3.7).
Function
This activates the chained transformation. A
previously activated other transformation is implicitly
disabled by TRACON().
A tool is always assigned to the first transformation
of a chain. The subsequent transformation then
behaves as if the active tool length were zero. Only
the base lengths of a tool (_BASE_TOOL_) set via
machine data are active for the first transformation
of the chain.
Deactivate
Programming
TRAFOOF
Function
The command deactivates the last active (chained)
transformation.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-307
7 Transformations 11.02 7.8 Switchable geometry axes, GEOAX 7
840 D 8 10D 8 40Di
NCU 572
NCU 573
7.8 Switchable geometry axes, GEOAX
Programming
GEOAX(n,channel axis,n,channel axis,…)
GEOAX()
Explanation of the parameters
GEOAX(n,channel axis,n,channel Switch the geometry axes.
axis,…)
GEOAX() Call the basic configuration of the geometry axes
n Number of the geometry axis (n=1, 2 or 3) to be
assigned to another channel axis.
n=0: remove the specified channel axis from the
geometry axis grouping without replacement.
Channel axis Name of the channel axis to be accepted into
the geometry axis grouping.
Function
The "switchable geometry axes" function allows the
geometry axis grouping configured via machine data
to be modified from the parts program. A channel Z1
Z2
axis defined as a synchronized special axis can
replace any geometry axis.
Y1
X1
Example: Y
Z
A tool carriage can be traversed over channel axes X
X1, Y1, Z1, Z2. In the parts program, axes Z1 and
Z2 should be used alternately as geometry axis Z.
GEOAX is used in the parts program to switch
between the axes.
After activation, the connection
X1, Y1, Z1 is effective (adjustable via MD).
N100 GEOAX (3,Z2) Channel axis Z2 functions as the Z axis
N110 G1 .....
N120 GEOAX (3,Z1) Channel axis Z1 functions as the Z axis
Siemens AG, 2002. All rights reserved
7-308 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.8 Switchable geometry axes, GEOAX 7
840D 8 10D 8 40Di
NCU 572
NCU 573
Sequence
Geometry axis number
In the command GEOAX(n,channel axis...) the
number n designates the geometry axis to which the
subsequently specified channel axis is to be
assigned.
Geometry axis numbers 1 to 3 (X, Y, Z axis) are
permissible for loading a channel axis.
n = 0 removes an assigned channel axis from the
geometry axis grouping without reassigning the
geometry axis.
After the transition, an axis replaced by switching in
the geometry axis grouping is programmable as a
special axis via its channel name.
Switching over the geometry axes deletes all the
frames, protection zones and operating range limits.
Polar coordinates:
As with a change of plane (G17–G19), replacing
geometry axes with GEOAX sets the modal polar
coordinates to the value 0.
DRF, ZO:
Any existing handwheel offset (DRF) or an external
zero offset, will stay active after the switchover.
Exchange axis positions
It is also possible to change positions within the
geometry axis grouping by reassigning the axis
numbers to already assigned channel axes.
N... GEOAX (1, XX, 2, YY, 3, ZZ) Channel axis XX is the first, YY the
second and ZZ the third geometry axis,
N... GEOAX (1, U, 2, V, 3, W) Channel axis U is the first, V the second
and W the third geometry axis.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-309
7 Transformations 11.02 7 .8 Switchable geometry axes, GEOAX 7
8 40 D 810D 840Di
NCU 572
NCU 573
Prerequisites and restrictions
1. It is not possible to switch the geometry axes
over during:
- an active transformation,
- an active spline interpolation,
- an active tool radius compensation, (Programming Guide Fundamentals:
- an active fine tool compensation Chapter 8)
2. If the geometry axis and the channel axis have (Programming Guide Fundamentals:
the same name, it is not possible to change the Chapter 8)
particular geometry axis.
3. None of the axes involved in the switchover can
be involved in an action that might persist beyond
the block limits, as is the case, for example, with
positioning axes of type A or with following axes.
4. The GEOAX command can only be used to
replace geometry axes that already existed at
power ON (i.e. no newly defined ones).
5. Using GEOAX for axis replacement while
preparing the contour table (CONTPRON,
CONTDCON) produces an alarm.
Deactivating switchover
The command GEOAX() calls the basic
configuration of the geometry axis grouping.
After POWER ON and when switching over to
reference point approach mode, the basic
configuration is reset automatically.
Additional notes
Transition and tool length compensation
An active tool length compensation is also effective
after the transition. However, for the newly adopted
or repositioned geometry axes, it counts as not
retracted.
So accordingly, at the first motion command for
these geometry axes, the resultant travel path
comprises the sum of the tool length compensation
and the programmed travel path.
Siemens AG, 2002. All rights reserved
7-310 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
7 11.02 Transformations 7.8 Switchable geometry axes, GEOAX 7
840D 810D 8 40Di
NCU 572
NCU 573
Geometry axes that retain their position in the axis
grouping during a switchover, also keep their status
with regard to tool length compensation.
Geometry axis configuration and transformation
change
The geometry axis configuration applicable in an
active transformation (defined via the machine data)
cannot be modified by using the "switchable
geometry axes" function.
If it is necessary to change the geometry axis
configuration in connection with transformations, this
is only possible via an additional transformation.
A geometry axis configuration modified via GEOAX
is deleted by activating a transformation.
If the machine data settings for the transformation
and for switching over the geometry axes contradict
one another, the settings in the transformation take
precedence.
Example:
A transformation is active. According to the machine
data, the transformation should be retained during a
RESET, however, at the same time, a RESET
should produce the basic configuration of the
geometry axes. In this case, the geometry axis
configuration is retained as specified by the
transformation.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 7-311
7 Transformations 11.02 7 .8 Switchable geometry axes, GEOAX 7
840 D 8 10D 8 40Di
NCU 572
NCU 573
Programming example
A machine has six channel axes called XX, YY, ZZ,
U, V ,W. The basic setting of the geometry axis
configuration via the machine data is:
Channel axis XX = 1st geometry axis (X axis)
Channel axis YY = 2nd geometry axis (Y axis)
Channel axis ZZ = 3rd geometry axis (Z axis)
N10 GEOAX() The basic configuration of the geometry axes is effective.
N20 G0 X0 Y0 Z0 U0 V0 W0 All the axes in rapid traverse to position 0.
N30 GEOAX(1,U,2,V,3,W) Channel axis U becomes the first (X), V the second (Y),
W the third geometry axis (Z).
N40 GEOAX(1,XX,3,ZZ) Channel axis XX becomes the first (X), ZZ the third
geometry axis (Z). Channel axis V stays as the second
geometry axis (Y).
N50 G17 G2 X20 I10 F1000 Full circle in the X, Y plane. Channel axes XX and V
traverse
N60 GEOAX(2,W) Channel axis W becomes the second geometry axis (Y).
N80 G17 G2 X20 I10 F1000 Full circle in the X, Y plane. Channel axes XX and W
traverse.
N90 GEOAX() Reset to initial state
N100 GEOAX(1,U,2,V,3,W) Channel axis U becomes the first (X), V the second (Y),
W the third geometry axis (Z).
N110 G1 X10 Y10 Z10 XX=25 Channel axes U, V, W each traverse to position 10, XX
as the special axis traverses to position 25.
N120 GEOAX(0,V) V is removed from the geometry axis grouping. U and W
are still the first (X) and third geometry axis (Z). The
second geometry axis (Y) remains unassigned.
N130 GEOAX(1,U,2,V,3,W) Channel axis U stays the first (X), V becomes the second
(Y), W stays the third geometry axis (Z).
N140 GEOAX(3,V) V becomes the third geometry axis (Z), which overwrites
W and thus removes it from the geometry axis grouping.
The second geometry axis (Y) is still unassigned.
Siemens AG, 2002. All rights reserved
7-312 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8
Tool Offsets
8.1 Offset memory............................................................................................................... 8-314
8.2 Language commands for tool management ................................................................. 8-316
8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF ................................. 8-319
8.4 Maintain tool radius compensation at constant level, CUTCONON
(SW 4 and higher) ......................................................................................................... 8-325
8.5 Activate 3D tool offsets ................................................................................................. 8-328
8.6 Tool orientation.............................................................................................................. 8-336
8.7 Free assignment of D numbers, cutting edge number CE (SW 5 and higher) ............. 8-341
8.7.1 Check D numbers (CHKDNO) ............................................................................... 8-342
8.7.2 Renaming D numbers (GETDNO, SETDNO)........................................................ 8-343
8.7.3 T numbers for the specified D number (GETACTTD) ........................................... 8-344
8.7.4 Set final D numbers to invalid ................................................................................ 8-345
8.8 Toolholder kinematics ................................................................................................... 8-346
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-313
8 Tool Offsets 11.028.1 Offset memory 8
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
8.1 Offset memory
Structure of the offset memory
Every data field can be invoked with a T and D
number (except "Flat D No."); in addition to the
geometrical data for the tool, it contains other
information such as the tool type.
SW 4 and higher
The "Flat D No. structure" is used if tool
management takes place outside the NCK. In this
case, the D numbers are generated with the
associated tool offset blocks without being assigned
to tools.
You can still program in the parts program using T.
However, this T does not relate to the programmed
D number.
Several entries exist for the geometric variables (e.g.
length 1 or radius). These are added together to
produce a value (e.g. total length 1, total radius)
which is then used for the calculations.
Offset values not required must be assigned the
value zero.
The individual values of the offset memories P1 to
P25 can be read from and written to the program via
system variable.
Siemens AG, 2002. All rights reserved
8-314 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets8.1 Offset memory 8
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Tool parameters Meaning Comment
Number (DP)
$TC_DP 1 Tool type For overview see list
$TC_DP 2 Tool point direction For turning tools only
Geometry Tool length compensation
$TC_DP 3 Length 1 Calculation depending
$TC_DP 4 Length 2 on type and plane
$TC_DP 5 Length 3
Geometry Radius
$TC_DP 6 Radius
$TC_DP 7 Slot width b for slotting saw, rounding radius
for milling tools
$TC_DP 8 Overhang k For slotting saw only
$TC_DP 11 Angle for cone milling tools
Wear Tool length and radius compensation
$TC_DP 12 Length 1
$TC_DP 13 Length 2
$TC_DP 14 Length 3
$TC_DP 15 Radius
$TC_DP 16 Slot width b for slotting saw, rounding radius
for milling tools
$TC_DP 17 Overhang k For slotting saw only
$TC_DP 20 Angle for cone milling tools
Base dimensions/ Tool length compensation
adapter
$TC_DP 21 Length 1
$TC_DP 22 Length 2
$TC_DP 23 Length 3
Technology
$TC_DP 24 Clearance angle For turning tools
Additional notes
All other parameters are reserved.
Machine manufacturer
User cutting edge data can be configured via MD.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-315
8 Tool Offsets 11.028.2 Language commands for tool management 8
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
8.2 Language commands for tool management
Explanation of the commands
T="WZ" Select tool with name
NEWT("WZ",DUPLO_NO) Create new tool, duplo number optional
DELT("WZ",DUPLO_NO) Delete tool, duplo number optional
GETT("WZ",DUPLO_NO) Determine T number
SETPIECE(x,y) Set piece number
GETSELT(x) Read preselected tool number (T No.)
"WZ" Tool name
DUPLO_NO Quantity
x Spindle number, entry optional
If you use the tool manager you can create and call
tools by name, e.g. T="DRILL" or T="123".
NEWT function
With the NEWT function you can create a new tool
with name in the NC program. The function
automatically returns the T number created, which
can subsequently be used to address the tool.
Return parameter=NEWT("WZ", DUPLO_NO)
If no duplo number is specified, this is generated
automatically by the tool manager.
Example:
DEF INT DUPLO_NO
DEF INT T_NO
DUPLO_NO = 7
T_NO=NEWT("DRILL", DUPLO_NO) Create new tool "DRILL" with duplo number 7. The T
number created is stored in T_NO.
DELT function
The DELT function can be used to delete a tool
without referring to the T number.
DELT("WZ",DUPLO_NO)
Siemens AG, 2002. All rights reserved
8-316 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets8.2 Language commands for tool management 8
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
GETT function
The GETT function returns the T number required to
set the tool data for a tool known only by its name.
Return parameter=GETT("WZ", DUPLO_NO)
If several tools with the specified name exist, the T
number of the first possible tool is returned.
Return parameter = –1: The tool name or duplo
number cannot be assigned to a tool.
Examples:
T="DRILL"
R10=GETT("DRILL", DUPLO_NO) Return T number for DRILL with duplo
number = DUPLO_NO
The "DRILL" must first be declared with NEWT or
$TC_TP1[ ].
$TC_DP1[GETT("DRILL", Write a tool parameter with tool name
DUPLO_NO),1]=100
SETPIECE function
This function is used to update the piece number
monitoring data.
The function counts all of the tool edges which have
been changed since the last activation of SETPIECE
for the stated spindle number.
SETPIECE(x,y)
x Number of completed workpieces
y y spindle number, 0 stands for master spindle (default setting)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-317
8 Tool Offsets 11.028.2 Language commands for tool management 8
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
GETSELT function
This function returns the T number of the tool
preselected for the spindle.
This function allows access to the tool offset data
before M6 and thus establishes main run
synchronization slightly earlier.
Example for tool change with tool management
T1 Preselect tool, i.e. the tool magazine can be
brought into the tool position parallel to
machining.
M6 Load preselected tool (depending on the
setting in the machine data you can also
program without M6).
Example:
T1 M6 Load tool 1
D1 Select tool length compensation
G1 X10 … Machining with T1
T="DRILL" Preselect drill
D2 Y20 … Change cutting edge T1
X10 … Machining with T1
M6 Load tool drill
SETPIECE(4) Number of completed workpieces
D1 G1 X10 … Machining with drill
A complete list of all variables required for tool
management is given in the list of system variables
in the Appendix.
Siemens AG, 2002. All rights reserved
8-318 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF
Programming:
FCTDEF(Polynomial no., LLimit, ULimit,a0,a1,a2,a3)
PUTFTOCF(Polynomial No., Ref_value, Length1_2_3, Channel, Spindle)
PUTFTOC(Value, Length1_2_3, Channel, Spindle)
FTOCON
FTOCOF
Explanation of the commands
PUTFTOCF Write online tool offsets continuously
FCTDEF Define parameters for PUTFTOCF function
PUTFTOC Write online tool offsets discretely
FTOCON Activate online tool offsets
FTOCOF Deactivate online tool offsets
Explanation of the parameters
Polynomial_No. Values 1-3: A maximum of three polynomials can be programmed at the
same time; polynomials up to 3rd degree
Ref_value Reference value from which the offset is derived
Length1_2_3 Wear parameter into which the tool offset value is added
Channel Number of channel in which the tool offset is activated; specified only if
the channel is different to the present one
Spindle Number of the spindle on which the online tool offset acts; only needs to
be specified for inactive grinding wheels
LLimit Lower limit
ULimit Upper limit
a0,a1,a2,a3 Coefficients of polynomial function
Value Value added in the wear parameter
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-319
8 Tool Offsets 11.028.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
Function
The function makes immediate allowance for tool
offsets resulting from machining by means of online
tool length compensation (e. g. CD dressing: The Dressing roll
grinding wheel is dressed parallel to machining). The
tool length compensation can be changed from the Dressing amount Grinding
machining channel or a parallel channel (dresser wheel
channel).
Online tool offset can be applied only to grinding
Workpiece
tools.
General information about online TO
Depending on the timing of the dressing process, the
following functions are used to write the online tool
offsets:
• Continuous write, non-modal: PUTFTOCF
• Continuous write, modally: ID=1 DO FTOC
(see section synchronized actions)
• Discrete write: PUTFTOC
In the case of a continuous write (for each
interpolation pulse) following activation of the
evaluation function each change is calculated
additively in the wear memory in order to prevent
setpoint jumps.
I n both cases:
T he online tool offset can act on each spindle and
lengths 1, 2 or 3 of the wear parameters.
The assignment of the lengths to the geometry axes
is made with reference to the current plane.
T he assignment of the spindle to the tool is made
with reference to the tool data with GWPSON or
TMON as long as it is not the active grinding wheel
(see Programming Guide "Fundamentals").
Siemens AG, 2002. All rights reserved
8-320 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
Length 1
8 11.02 Tool Offsets8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
A n offset is always applied for the wear parameters
for the current tool side or for the left-hand tool side
on inactive tools.
W here the offset is identical for several tool sides,
the values should be transferred automatically to the
second tool side by means of a chaining rule (see
Operator's Guide for description).
I f online offsets are defined for a machining channel,
you cannot change the wear values for the current
tool on this channel from the machining program or
by means of an operator action.
T he online tool offset is also applied with respect to
the constant grinding wheel peripheral speed
(GWPS) in addition to tool monitoring (TMON) and
centerless grinding (CLGON).
Sequence
PUTFTOCF = Continuous write
T he dressing process is performed at the same time
as machining:
Dress across complete grinding wheel width with
dresser roll or dresser diamond from one side of a
grinding wheel to the other.
M achining and dressing can be performed on
different channels. If no channel is programmed, the
offset takes effect in the active channel.
PUTFTOCF(Polynomial_No., Ref_value, Length1_2_3, Channel, Spindle)
T ool offset is changed continuously on the
machining channel according to a polynomial
function of the first, second or third degree, which
must have been defined previously with FCTDEF.
The offset, e.g. changing actual value, is derived
from the "Reference value“ variable.
I f a spindle number is not programmed, the offset
applies to the active tool.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-321
8 Tool Offsets 11.028.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
Set parameters for FCTDEF function
The parameters are defined in a separate block:
FCTDEF(Polynomial_NO., LLimit, ULimit,a0,a1,a2,a3)
T he polynomial can be a 1st, 2nd or 3rd degree
polynomial.
The limit identifies the limit values (LLimit = lower
limit, ULimit = upper limit).
E xample:
Straight line (y = a0 + a1x) with gradient 1 Y
FCTDEF(1, -1000, 1000, -$AA_IW[X], 1) a1
1
Write online offset discretely: PUTFTOC
T his command can be used to write an offset value a0
once. The offset is activated immediately on the X
target channel.
A pplication of PUTFTOC:
The grinding wheel is dressed from a parallel
channel, but not at the same time as machining.
PUTFTOC(Value, Length1_2_3, Channel,
Spindle)
The online tool offset for the specified length 1, 2 or
3 is changed by the specified value, i.e. the value is
added to the wear parameter.
Include online tool offset: FTOCON, FTOCOF
The target channel can only receive online tool
offsets when FTOCON is active.
• FTOCON must be written in the channel on
which the offset is to be activated.
With FTOCOF, the offset is no longer applied,
however the complete value written with
PUTFTOC is corrected in the tool edge-specific
offset data.
• FTOCOF is always the reset setting.
• PUTFTOCF always acts on the subsequent
traversing block.
• The online tool offset can also be selected modally
with FTOC. Please refer to Section "Motion-
synchronized actions" for more information.
Siemens AG, 2002. All rights reserved
8-322 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets8.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
Programming example
Y
T ask
On a surface grinding machine with the following
Dressing roll
parameters, the grinding wheel is to be dressed by
the amount 0.05 after the start of the grinding
movement at X100. The dressing amount is to be 0.05 Grinding
wheel
active with write online offset continuously.
Y: Infeed axis for the grinding wheel
V: Infeed axis for the dresser roll
Workpiece X
M achine: Channel 1 with axes X, Z, Y
100
Dress: Channel 2 with axis V
M achining program in channel 1:
%_N_MACH_MPF
…
N 110 G1 G18 F10 G90 Basic position
N120 T1 D1 Select current tool
N130 S100 M3 X100 Spindle on, travel to starting position
N140 INIT (2, "DRESS", "S") Select dressing program on channel 2
N 150 START (2) S tart dressing program on channel 2
N160 X200 Travel to destination position
N170 FTOCON A ctivate online offset
N … G1 X100 Continue machining
N…M30
D ressing program in channel 2:
%_N_DRESS_MPF
…
N40 FCTDEF (1, –1000, 1000, –$AA_IW[V], 1) Define function: Straight line
N50 PUTFTOCF (1, $AA_IW[V], 3, 1) Write online offset continuously:
L ength 3 of the current grinding wheel is
derived from the movement of the V axis
and corrected in channel 1.
N60 V–0.05 G1 F0.01 G91 Infeed movement for dressing, PUTFTOCF
is only effective in this block
…
N… M30
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-323
8 Tool Offsets 11.028.3 Online tool offset PUTFTOCF, PUTFTOC, FTOCON, FTOCOF 8
840D 840Di
NCU 572
NCU 573
D ressing program, modal:
%_N_DRESS_MPF
FCTDEF(1,-1000,1000,-$AA_IW[V],1) Define function:
ID=1 DO FTOC(1,$AA_IW[V],3,1) Select online tool offset:
Actual value of the V axis is the input value
for polynomial 1; the result is added length 3
of the active grinding wheel in channel 1 as
the offset value.
WAITM(1,1,2) Synchronization with machining channel
G1 V-0.05 F0.01, G91 Infeed movement for dressing
G1 V-0.05 F0.02
...
CANCEL(1) Deselect online offset
...
Siemens AG, 2002. All rights reserved
8-324 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8 .4 Maintain tool radius compensation at constant level, CUTCONON 8
8 40D 840Di
NCU 572
NCU 573
8.4 Maintain tool radius compensation at constant level, CUTCONON
(SW 4 and higher)
Programming:
CUTCONON
CUTCONOF
Explanation
CUTCONON Activate the tool radius compensation constant function
CUTCONOF Deactivate the constant function (default setting)
Function
The "tool radius compensation constant" function is
used to suppress the tool radius compensation for a
number of blocks while retaining the difference
between the programmed and actual path of the tool
center point accumulated in previous blocks as an
offset.
This can be practical, for example, if several motion
blocks are required at the reversal points during line-
by-line milling but the contours (bypass strategies)
generated by the tool radius compensation are not
desirable.
It can be used according to the type of tool radius
compensation (21/2D, 3D face milling, 3D
circumferential milling).
Sequence
Tool radius compensation is normally active before
the compensation suppression and is still active
when the compensation suppression is deactivated
again.
The offset point at the end of block position is
approached in the last motion block before
CUTCONON.
All following blocks in which the compensation
suppression is active are executed without
compensation.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-325
8 Tool Offsets 11.02 8 .4 Maintain tool radius compensation at constant level, CUTCONON 8
8 40D 840Di
NCU 572
NCU 573
They are displaced, however, by the vector from the
end point of the last compensation block to its offset
point.
The interpolation type of these blocks (linear,
circular, polynomial) is arbitrary.
The deactivation block of the compensation
suppression, i.e. the block containing CUTCONOF,
is usually corrected; it begins at the offset point of
the start point.
A linear block is inserted between this point and the
end point of the previous block, i.e. the last
programmed motion block with active CUTCONON.
Circle blocks in which the circle plane is
perpendicular to the compensation plane (vertical
circles) are treated as if CUTCONON had been
programmed in the blocks.
This implicit activation of compensation suppression
is automatically canceled in the first motion block
which is not a circle of this type but which contains a
traversing movement in the compensation plane.
Vertical circles of this type can only occur with
circumferential milling.
Example
N10 ; D efinition of tool d1
N20 $TC_DP1[1,1]= 110 ; Type
N30 $TC_DP6[1,1]= 10. ; Radius
N40
N50 X0 Y0 Z0 G1 G17 T1 D1 F10000
N60
N70 X20 G42 NORM
N80 X30
N90 Y20
N100 X10 CUTCONON; Activate compensation suppression
N110 Y30 CONT ; I nsert bypass circle if necessary on deactivation
of contour suppression
N120 X-10 CUTCONOF
N130 Y20 NORM ; N o bypass circle on deactivation of TRC
N140 X0 Y0 G40
N150 M30
Siemens AG, 2002. All rights reserved
8-326 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.4 Maintain tool radius compensation at constant level, CUTCONON 8
8 40D 840Di
NCU 572
NCU 573
Y
Contour without TRC
N120
N110
N130
Contour with TRC N100
N90
N140
N70 N80
50 X
-10
Additional notes
1. CUTCONON has no effect if tool radius
compensation is not active (G40). An alarm is
output.
The G code remains active, however. This is
significant if tool radius compensation is to be
activated in a subsequent block with G41 or G42.
2. It is possible to change the G code in the 7th G
code group (tool radius compensation; G40 / G41
/ G42) when CUTCONON is active. A change to
G40 is effective immediately.
The offset with which the previous blocks were
traversed is applied.
3. If CUTCONON or CUTCONOF is programmed in
a block without a traversing movement in the
active compensation plane, the change does not
become effective until the next block with such a
traversing movement.
Further information: /FB/, W1 Tool Offset
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-327
8 Tool Offsets 11.02 8.5 Activate 3D tool offsets 8
840D 8 40Di
NCU 572
NCU 573
8.5 Activate 3D tool offsets
Explanation
CUT3DC Activation of 3D radius offset for circumferential milling
CUT3DFS 3D tool offset for face milling with constant orientation. The tool
orientation is determined by G17-G19 and is not influenced by Frames.
C UT3DFF 3 D tool offset for face milling with constant orientation. The tool
orientation is the direction determined by G17-G19 and possibly turned
by a Frame.
C UT3DF 3 D tool offset for face milling with orientation change (only with active
5-axes transformation).
G 40 X Y Z T o deactivate: Linear block G0/G1 with geometry axes
ISD=Value Insertion depth
T he commands are modal and are in the same
group as CUT2D and CUT2DF.
T he command is not deselected until the next
movement in the current plane is performed. This
always applies to G40 and is independent of the
CUT command.
Function
T ool orientation change is taken into account in tool
radius compensation for cylindrical tools.
The same programming commands apply to 3D tool
radius compensation as to 2D tool radius
compensation. With G41/G42, the left/right-hand
compensation is specified in the direction of
movement. The approach method is always NORM.
Siemens AG, 2002. All rights reserved
8-328 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.5 Activate 3D tool offsets 8
840D 8 40Di
NCU 572
NCU 573
Example
N10 A0 B0 X0 Y0 Z0 F5000
N20 T1 D1 T ool call, call tool offset values
N30 TRAORI(1) Transformation selection
N 40 CUT3DC 3D tool radius compensation selection
N50 G42 X10 Y10 Tool radius compensation selection
N60 X60
N70 …
Additional notes
I ntermediate blocks are permitted with 3D tool radius
compensation. The rules for 2 ½ D tool radius
compensation apply.
3D tool radius compensation is only active when
five-axis transformation is selected.
A circle block is always inserted at outside corners.
G450/G451 have no effect.
The DISC command is ignored.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-329
8 Tool Offsets 11.02 8 .5 Activate 3D tool offsets 8
8 40D 8 40Di
NCU 572
NCU 573
D ifference between 2 ½ D and 3D tool radius
compensation
I n 3D tool radius compensation tool orientation can
be changed. Workpiece
contour
2 ½ D tool radius compensation assumes the use of
a tool with constant orientation.
Path of tool center point
equidistant from contour
3 D tool radius compensation is also called 5D tool
radius compensation, because in this case 5 L R
degrees of freedom are available for the orientation
of the tool in space.
C ircumferential milling
T he type of milling used here is implemented by Circumferential milling
defining a path (guide line) and the corresponding A
orientation. In this type of machining, the shape of B
the tool on the path is not relevant. The only deciding
factor is the radius at the tool insertion point.
The 3D TRC function is limited to cylindrical tools.
Z
X
Y
Siemens AG, 2002. All rights reserved
8-330 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
ISD
8 11.02 Tool Offsets 8.5 Activate 3D tool offsets 8
8 40D 840Di
NCU 572
NCU 573
F ace milling
For this type of 3D milling, you require line-by-line
definition of 3D paths on the workpiece surface.
The tool shape and dimensions are taken into
account in the calculations that are normally
performed in CAM.
In addition to the NC blocks, the postprocessor
writes the tool orientations (when five-axis
transformation is active) and the G code for the
desired 3D tool offset into the parts program.
This feature offers the machine operator the option
of using slightly smaller tools than that used to
calculate the NC paths.
Example:
NC blocks have been calculated with a 10mm mill.
In this case, the workpiece could also be machined
with a mill diameter of 9.9mm, although this would
result in a different surface profile.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-331
8 Tool Offsets 11.02 8.5 Activate 3D tool offsets 8
840D 8 40Di
NCU 572
NCU 573
M ill shapes, tool data
T he table below gives an overview of the tool shapes R R
which may be used in face milling operations as well
as tool data limit values.
The shape of the tool shaft is not taken into Cylindr. Ball end
die-sinking mill
consideration – the tools 120 and 155 are identical in cutter (type 111)
(type 110)
their effect. a
If a different type number is used in the NC program
than the one listed in the table, the system R R
automatically uses tool type 110 die-sinking cutter.
r
An alarm is output if the tool data limit values are R
violated. End mill End mill with Truncated cone mill
(type 120, 130) corner round.
(type 155)(type 121, 131)
Milling tool type T ype No. R r a
C ylindrical miller 1 10 >0 X X
B all end mill 111 >0 >R X
E nd mill, angle head cutter 1 20, 130 >0 X X
E nd mill, angle head cutter with corner rounding 1 21, 131 >r >0 X
T runcated cone mill 155 >0 X >0
X =is not evaluated
T ool length compensation
The tool tip is the reference point for length
compensation (intersection longitudinal
axis/surface).
Siemens AG, 2002. All rights reserved
8-332 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
r
8 11.02 Tool Offsets 8.5 Activate 3D tool offsets 8
8 40D 8 40Di
NCU 572
NCU 573
3D tool offset, tool change
A new tool with changed dimensions (R, r, a) or a
different shape may be specified only through
programming G41 or G42 (transition G40 to G41 or
G42, reprogramming of G41 of G42).
T his rule does not apply to any other tool data, e.g.
tool lengths, so that tools to which such data apply
can be fitted without reprogramming G41 or G42.
Correction of the path
With respect to face milling, it is advisable to
examine what happens when the contact point
"jumps" on the tool surface as shown in the example
on the right where a convex surface is being
machined with a vertically positioned tool.
As a general rule, it is advisable to select a tool
shape and tool orientation that are suitable for
producing the required surface profile.
The application shown in the example should
therefore be regarded as a borderline case. Single point
This borderline case is monitored by the control that
detects abrupt changes in the machining point on
the basis of angular approach motions between the
tool and normal surface vectors. The control inserts
linear blocks at these positions so that the motion
can be executed.
These linear blocks are calculated on the basis of
permissible angular ranges for the side angle stored
in the machine data.
The system outputs an alarm if the limit values
stored in the machine data are violated.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-333
8 Tool Offsets 11.02 8 .5 Activate 3D tool offsets 8
840D 840Di
NCU 572
NCU 573
P ath curvature
P ath curvature is not monitored. In such cases, it is
also advisable to use only tools of a type that do not
violate the contour.
I nsertion depth (ISD)
Program command ISD (insertion depth) is used to
program the tool insertion depth for peripheral milling
operations. This makes it possible to change the
position of the machining point on the outer surface
of the tool.
ISD specifies the distance between the cutter tip
FH
(FS) and the cutter reference point (FH). The point
FH is produced by projecting the programmed
machining point along the tool axis. ISD is only
FS
evaluated when 3D tool radius compensation is
active.
Inside corners/outside corners
Inside and outside corners are handled separately.
The term inside or outside corner depends on the
tool orientation.
When changes occur in the orientation at a corner,
the corner type can change during machining. If this
happens, machining stops and an error message is
generated.
Direction of machining
Siemens AG, 2002. All rights reserved
8-334 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
ISD
8 11.02 Tool Offsets 8.5 Activate 3D tool offsets 8
840D 840Di
NCU 572
NCU 573
Intersection procedure for 3D compensation
(SW 5 and higher)
W ith 3D circumferential milling, G code G450/G451
is now evaluated at the outside corners; this means
that the intersection of the offset curves can be
approached. With SW 4 a circle was always inserted
at the outside corners.
The new functionality is particularly advantageous
for typical CAD-generated 3D programs. They often
consist of short straight blocks (to approximate
smooth curves), where the transitions are almost
tangential between adjacent blocks.
U p to now, with tool radius compensation on the
outside of the contour, circles were generally
inserted to circumnavigate the outside corners.
These blocks can be very short with almost
tangential transitions, resulting in undesired drops in
velocity.
I n these cases, as with 2½ D radius compensation,
both of the curves involved are lengthened and the
intersection of both lengthened curves is
approached.
T he intersection is determined by extending the
offset curves of both blocks and defining their
intersection a the corner in the plane perpendicular
to the tool orientation. If there is no such
intersection, the corner is handled as previously, that
is, a circle is inserted.
F or more information about intersection procedure,
see /FB/ W5, 3D Tool Radius Compensation
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-335
8 Tool Offsets 11.02 8.6 Tool orientation 8
840D 840Di
NCU 572
NCU 573
8.6 Tool orientation
T ool orientation is the term given to the geometrical
alignment of the tool in space. Z
O n a 5-axis machine tool, the tool orientation can be
controlled with program commands.
Direction
vector
X
Y
P rogramming tool orientation
A change in tool orientation can be programmed by:
• Direct programming of the rotary axes Change in
orientation
• Euler or RPY angle
• Direction vector
• LEAD/TILT (face milling)
T he reference coordinate system is either the
machine coordinate system (ORIMCS) or the current
workpiece coordinate system (ORIWCS).
A change in orientation can be controlled by the
following:
ORIC Orientation and path movement in parallel
O RID Orientation and path movement consecutively
OSOF No orientation smoothing
OSC Orientation constantly
OSS Orientation smoothing only at beginning of block
O SSE O rientation smoothing at beginning and end of block
O RIS Speed of orientation change with active orientation smoothing in
degrees per mm; valid for OSS and OSSE
Siemens AG, 2002. All rights reserved
8-336 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.6 Tool orientation 8
8 40D 840Di
NCU 572
NCU 573
B ehavior at outside corners
A circle block is inserted
A circle block with the radius of the cutter is always between block N1 and N2
inserted at an outside corner.
The program commands ORIC and ORID can be N2
used to define whether changes in orientation
programmed between blocks N1 and N2 are
executed before the beginning of the inserted circle N1
block or at the same time.
R
I f an orientation change is required at outside corners,
this can be performed either at the same time as
interpolation or separately together with the path
movement.
With ORID, the inserted blocks are executed initially
without a path movement. The circle block
generating the corner is inserted immediately before
the second of the two traversing blocks.
I f several orientation blocks are inserted at an
external corner and ORIC is selected, the circular
movement is divided among the individual inserted
blocks according to the values of the orientation
changes.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-337
8 Tool Offsets 11.02 8.6 Tool orientation 8
8 40D 8 40Di
NCU 572
NCU 573
Programming example for ORIC
If two or more blocks with orientation changes (e.g.
N14
A2= B2= C2=) are programmed between traversing
blocks N10 and N20 and ORIC is active, the inserted N12 N20
circle block is divided among these intermediate
blocks according to the values of the angle changes.
N10
ORIC
N8 A2=… B2=… C2=…
N10 X… Y… Z…
N12 C2=… B2=… The circle block inserted at the external
N14 C2=… B2=… corner is divided among N12 and N14 in
accordance with the change in orientation.
The circular movement and the orientation
change are executed in parallel.
N 20 X =…Y=… Z=… G1 F200
Siemens AG, 2002. All rights reserved
8-338 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.6 Tool orientation 8
840D 8 40Di
NCU 572
NCU 573
Programming example for ORID
I f ORID is active, all the blocks between the two Execute N12 and N14
traversing blocks are executed at the end of the first
traversing block. The circle block with constant N20
orientation is executed immediately before the
second traversing block.
N10
ORID
N8 A2=… B2=… C2=…
N10 X… Y… Z…
N12 A2=… B2=… C2=… Blocks N12 and N14 are executed at the
end of N10. The circle block with the current
orientation is subsequently traversed.
N14 M20 Auxiliary functions, etc.
N20 X… Y… Z…
T he program command which is active in the first
traversing block of an external corner determines the
type of orientation change.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-339
8 Tool Offsets 11.02 8.6 Tool orientation 8
8 40D 8 40Di
NCU 572
NCU 573
W ithout orientation change
I f the orientation is not changed at the block
boundary, the cross-section of the tool is a circle
which touches both of the contours.
Programming example
Change the orientation at an internal corner
N15
N12
N10
TRC
O RIC
N10 X …Y… Z… G1 F500
N12 X …Y… Z… A2=… B2=…, C2=…
N15 X Y Z A2 B2 C2
Siemens AG, 2002. All rights reserved
8-340 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8 .7 Free assignment of D numbers, cutting edge number CE 8
8 40D 840Di
NCU 572
NCU 573
8 .7 Free assignment of D numbers, cutting edge number CE
(SW 5 and higher)
A s of SW 5, you can use the D numbers as contour
numbers. You can also address the number of the
cutting edge via the address CE.
Y ou can use the system parameter $TC_DPCE to
describe the cutting edge number.
Preset: Offset No. == Cutting edge No.
References: FB, W1 (Tool Offset)
Machine manufacturer (MH 8.12)
The maximum number of D numbers (cutting edge
numbers) and maximum number of cutting edges
per tool are defined via the machine data. The
following commands only make sense when the
maximum number of cutting edges (MD 18105) is
greater than the number of cutting edges per tool
(MD 18106). Please refer to the data of the machine
tool manufacturer.
Additional notes
Besides the relative D number, you can also assign
D numbers al 'flat' or 'absolute' D numbers
(1–32000) without assigning a reference to a T
number (inside the function 'flat D number
structure').
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-341
8 Tool Offsets 11.02 8 .7 Free assignment of D numbers, cutting edge number CE 8
840D 840Di
NCU 572
NCU 573
8.7.1 Check D numbers (CHKDNO)
Programming:
s tate=CHKDNO(Tno1,Tno2,Dno)
Explanation of the parameters
s tate TRUE: The D numbers are assigned uniquely to the checked
areas.
FALSE: There was a D number collision or the parameters are
invalid. Tno1, Tno2 and Dno return the parameters that
caused the collision. These data can now be evaluated in
the parts program.
C HKDNO(Tno1,Tno2) All D numbers of the part specified are checked.
CHKDNO(Tno1) All D numbers of Tno1 are checked against all other tools.
CHKDNO A ll D numbers of all tools are checked against all other tools.
Function
CKKDNO checks whether the available D numbers
assigned are unique.
The D numbers of all tools defined in a TO unit must
only be present once. Replacement tools are not
considered.
Siemens AG, 2002. All rights reserved
8-342 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.7 Free assignment of D numbers, cutting edge number CE 8
840D 840Di
NCU 572
NCU 573
8 .7.2 Renaming D numbers (GETDNO, SETDNO)
Programming:
d = GETDNO(t,ce)
state = SETDNO(t,ce,d)
Explanation of the parameters
d D number of the cutting edge of the tool
t T number of the tool
ce Cutting edge number (CE number) of the tool
s tate Indicates whether the command could be executed (TRUE or FALSE).
Function
GETDNO
T his command returns the D number of a particular
cutting edge (ce) of a tool with tool number t.
If there is no D number for the specified parameters,
d is set to 0. If the D number is invalid, a value
greater than 32000 is returned.
SETDNO
This commands assigns the value d of the D number
to a cutting edge ce of tool t. The result of this
statement is returned via state (TRUE or FALSE)
If there is no data block for the specified parameter,
the value FALSE is returned. Syntax errors produce
an alarm. The D number cannot be set to 0 explicitly.
E xample: (renaming a D number)
$TC_DP2[1,2] = 120
$ TC_DP3[1,2] = 5.5
$ TC_DPCE[1,2] = 3; cutting edge
number CE
. ..
N10 def int DNoOld, DNoNew = 17
N 20 DNoOld = GETDNO(1,3)
N30 SETDNO(1,3,DNoNew)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-343
8 Tool Offsets 11.02 8.7 Free assignment of D numbers, cutting edge number CE 8
840D 840Di
NCU 572
NCU 573
T his assigns cutting edge CE=3 the new D value 17.
Now, these data for the cutting edge are addressed
via D-number 17; both via the system parameters
and in the programming with the NC address.
Additional notes
You must assign unique D numbers. Two different
cutting edges of a tool must not have the same D
number.
8 .7.3 T numbers for the specified D number (GETACTTD)
Programming:
status = GETACTTD(Tno, Dno)
Explanation of the parameters
Dno D number to be looked for for the T number.
Tno T number found
status 0: The T number was found. Tno contains the value of the T number.
-1: The specified D number does not have a T number; Tno=0.
-2: The D number is not absolute. Tno contains the value of the first tool found
that contains the D number with the value Dno.
-5: Unable to perform the function for another reason.
Function
For an absolute D number, GETACTTD determines
the associated T number. There is not check for
uniqueness. If there are several identical D numbers
within a TO unit, the T number of the first tool found
is returned. If 'flat' D numbers are used, it does not
make sense to use the command because the value
1 is always returned (no T number in database).
Siemens AG, 2002. All rights reserved
8-344 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.7 Free assignment of D numbers, cutting edge number CE 8
840D 840Di
NCU 572
NCU 573
8 .7.4 Set final D numbers to invalid
Programming:
D ZERO
Explanation
D ZERO M arks all D number of the TO unit as invalid
Function
T he command is used for support during upgrading.
Offset block marked in this way are no longer
checked by the language command CHKDNO.
To regain access, you must set the D number to
SETDNO again
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-345
8 Tool Offsets 11.02 8 .8 Toolholder kinematics 8
840D 8 40Di
NCU 572
NCU 573
8 .8 Toolholder kinematics
T he toolholder kinematics with up to two rotary axes is
programmed by means of 17 system variables
$TC_CARR1[m] to $TC_CARR17[m]. The description
l1
of the toolholder consists of:
• The vectorial distance between the first rotary axis
and the toolholder reference point l1, the vectorial
V1
α
1 l2
distance between the first and the second rotary
axis l2, the vectorial distance between the second
rotary axis and the tool reference point l3.
• The reference vectors of both rotary axes v1, v2.
l3
• The rotation angles α1, α2 around both axes. The
rotation angles are counted in viewing direction of α
2
V
the rotary axis vectors, positive, in clockwise 2
direction of rotation.
Resolved kinematics as of SW 5.3
For machines with resolved kinematics (both the tool
and the part can rotate), the system variables have
been extended to include the entries $TC_CARR18[m]
to $TC_CARR23[m] are described as follows:
The rotatable tool table consisting of:
• The vector distance between the second rotary axis
v2 and the reference point of a rotatable tool table l4
of the third rotary axis.
The rotary axes consisting of:
• The two channel identifiers for the reference to the
rotary axes v1 and v2. These positions are accessed
as required to determine the orientation of the
orientable toolholder.
The type of kinematics with one of the values T, P or M:
• Type of kinematics T: Only tool can rotate.
• Type of kinematics P: Only part can rotate.
• Type of kinematics M: Tool and part can rotate.
Siemens AG, 2002. All rights reserved
8-346 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.8 Toolholder kinematics 8
8 40D 8 40Di
NCU 572
NCU 573
Function of the system parameter for orientable toolholders
Designation x components y components z components
l1 offset vector $TC_CARR1[m] $TC_CARR2[m] $TC_CARR3[m]
l2 offset vector $TC_CARR4[m] $TC_CARR5[m] $TC_CARR6[m]
v1 rotary axis $TC_CARR7[m] $TC_CARR8[m] $TC_CARR9[m]
v2 rotary axis $TC_CARR10[m] $TC_CARR11[m] $TC_CARR12[m]
α1 rotation angle $TC_CARR13[m]
α2 rotation angle $TC_CARR14[m]
l3 offset vector $TC_CARR15[m] $TC_CARR16[m] $TC_CARR17[m]
l4 offset vector $TC_CARR18[m] $TC_CARR19[m] $TC_CARR20[m]
Axis identifier Axis identifier for rotary axes v1 and v2 (default is zero)
for rotary axis v1 $TC_CARR21[m]
for rotary axis v2 $TC_CARR22[m]
Type of $TC_CARR23[m]
kinematics Type of kinematics T Type of kinematics P Type of Kinematics M
Default T Only the Tool can be Only the Part can be Part and tool Mixed
rotated rotated mode can be rotated
Offset for Angle in degrees of rotary axes v1 and v2 when assuming the initial setting
rotary axis v1 $TC_CARR24[m]
rotary axis v2 $TC_CARR25[m]
Angle offset for Offset of Hirth tooth system in degrees for rotary axes v1 and v2
rotary axis v1 $TC_CARR26[m]
rotary axis v2 $TC_CARR27[m]
Angle increment Increment of Hirth tooth system in degrees for rotary axes v1 and v2
v1 rotary axis $TC_CARR28[m]
v2 rotary axis $TC_CARR29[m]
Minimum position Software limit for minimum position for rotary axes v1 and v2
rotary axis v1 $TC_CARR30[m]
rotary axis v2 $TC_CARR31[m]
Maximum Software limits for maximum position for rotary axes v1 and v2
position $TC_CARR32[m]
rotary axis v1 $TC_CARR33[m]
rotary axis v2
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-347
8 Tool Offsets 11.02 8 .8 Toolholder kinematics 8
8 40D 840Di
NCU 572
NCU 573
Parameters of the rotary axes from SW 6.1
The system variables are extended by the entries
$TC_CARR24[m] to $TC_CARR33[m] and described
as follows:
The offset of the rotary axes
• Changing the position of rotary axis v1 or v2 during
initial setting of the orientable toolholder.
The angle offset/angle increment of the rotary axes
• Offset or angle increment of Hirth tooth system of
rotary axes v1 and v2. Programmed or calculated
angle is rounded up to the next value that results
from phi = s + n * d when n is an integer.
The minimum position/maximum position of the
rotary axis
• Limit angle (software limit) for rotary axis v1 and v2.
Additional notes
The number of the respective toolholder to be
programmed is specified with "m.
The start/endpoints of the distance vectors on the axes
can be freely selected. The rotation angles α1, α2
around the two axes are defined in the initial state of
the toolholder by 0°. In this way, the kinematics of a
toolholder can be programmed for any number of
possibilities.
Toolholders with only one or no rotary axis at all can
be described by setting the direction vectors of one
or both rotary axes to zero. With a toolholder without
rotary axis the distance vectors act as additional tool
offsets whose components cannot be affected by a
change of machining plane (G17 to G19).
Siemens AG, 2002. All rights reserved
8-348 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
8 11.02 Tool Offsets 8.8 Toolholder kinematics 8
8 40D 840Di
NCU 572
NCU 573
Clearing the toolholder data
The data of all toolholder data sets is cleared via
$TC_CARR1[0] = 0.
SW 5.3 and higher
The type of kinematics $TC_CARR23[T] = T must
be assigned one of the three permissible uppercase
or lowercase letter (T,P,M) and should not be
deleted.
Changing the toolholder data
Each of the described values can be modified by
assigning a new value in the parts program.
Any character other than T, P or M causes an alarm
when you attempt to activate the orientable
toolholder.
Reading the toolholder data
Each of the described values can be read by
assigning it to a variable in the parts program.
Supplementary conditions
A toolholder can only orientate a tool in every possible
direction in space if
- two rotary axes v1 and v2 are available.
- the rotary axes are positioned perpendicular to one
another.
- the tool length axis is perpendicular to the
second rotary axis v2.
SW 5.3 and higher
In addition, the following requirement is applicable to
machines for which all possible orientations have to
be settable:
- Tool orientation must be perpendicular to the first
rotary axis v1.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 8-349
8 Tool Offsets 11.02 8.8 Toolholder kinematics 8
8 40D 840Di
NCU 572
NCU 573
Programming example
The toolholder used in the following example can be
z
fully described by a rotation around the Y axis.
z
Z Y
Y
Z
X
Y
X
X
X
N10 $TC_CARR8[1]=1 Definition of the Y components of the first
rotary axis of toolholder 1
N20 $TC_DP1[1,1]=120 Definition of an end mill
N30 $TC_DP3[1,1]=20 with length 20mm
N40 $TC_DP6[1,1]=5 and with radius 5mm
N50 ROT Y37 Frame definition with 37° rotation around the
Y axis
N60 X0 Y0 Z0 F10000 Approach initial position
N70 G42 CUT2DF TCOFR TCARR=1 T1 D1 X10 Set radius compensation, tool length
compensation in rotated frame, select
toolholder 1, tool 1
N80 X40 Execute machining under a 37° rotation
N90 Y40
N100 X0
N110 Y0
N120 M30
■
Siemens AG, 2002. All rights reserved
8-350 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9
Path Traversing Behavior
9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL......................................... 9-352
9.2 Coupled motion TRAILON, TRAILOF ........................................................................... 9-358
9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, CTABSSV,
CTABSEV...................................................................................................................... 9-362
9.4 Axial leading value coupling, LEADON, LEADOF......................................................... 9-375
9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO.......................................................... 9-381
9.6 Program run with preprocessing memory, STARTFIFO, STOPFIFO, STOPRE.......... 9-386
9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH .......................... 9-388
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-351
9 Path Traversing Behavior 11.029.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL
Programming
TANG (FAxisF,LAxis1,LAxis2,Coupling,CS)
TANGON (FAxis,Angle)
TANGOF (FAxis)
TLIFT (FAxis)
TANGDEL (FAxis)
Explanation of the commands
TANG Preparatory instruction for the definition of a tangential follow-up
TANGON Activate tangential control specifying following axis and offset angle
TANGOF Deactivate tangential control specifying following axis
TLIFT Insert intermediate block at contour corners
TANGDEL Delete definition of a tangential follow-up
Explanation of the parameters
FAxis Following axis: additional tangential following rotary axis
LAxis1, LAxis2 Leading axes: path axes which determine the tangent for the following axis
Coupling Coupling factor: relationship between the angle change of the tangent
and the following axis.
Parameter optional; default: 1
CS Identifier for coordinate system
"B" = basic coordinate system; data optional; default
["W" = workpiece coordinate system]
Angle Offset angle of following axis
Siemens AG, 2002. All rights reserved
9-352 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
Function
A rotary axis (= following axis) follows the
programmed path of two leading axes. The following
axis is located at a defined offset angle to the path
tangent.
Applications
Tangential control can be used in applications such
as: Y
• Tangential positioning of a rotatable tool during
nibbling
• Follow-up of the tool orientation on a band saw
• Positioning of a dresser tool on a grinding wheel
(see diagram)
• Positioning of a cutting wheel for glass or paper
working Workpiece
• Tangential infeed of a wire in five-axis welding Band saw
X
Sequence
D efining following axis and leading axis
T ANG is used to define the following and leading
axes.
A coupling factor specifies the relationship between
an angle change on the tangent and the following
axis. Its value is generally 1 (default).
T he follow-up can be performed in the basic
coordinate system "B" (default) or the workpiece
coordinate system "W".
Example:
TANG(C,X,Y,1,"B")
Meaning:
R otary axis C follows geometry axes X and Y.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-353
9 Path Traversing Behavior 11.029.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
Activating/deactivating tangential control:
T ANGON, TANGOF
T angential control is called with TANGON specifying
the following axis and the desired offset angle of the
following axis:
TANGON(C,90)
M eaning: Y
C axis is the following axis. On every movement of
the path axes, it is rotated into a position at 90° to
the path tangent.
T he following axis is specified in order to deactivate
the tangential control:
T ANGOF(C)
X
Angle limit through working area limitation
Y
For path movements which oscillate back and forth,
the tangent jumps through 180° at the turning point ∝
on the path and the orientation of the following axis ∝
changes accordingly.
This behavior is generally inappropriate: the return ∝ Unsuitable return
movement should be traversed at the same negative movement
X
offset angle as the approach movement. Y
This can be achieved by limiting the working area of -∝
the following axis (G25, G26). The working area
limitation must be active at the instant of path
Ideal return
reversal (WALIMON). movement
X
If the offset angle lies outside the working area limit,
an attempt is made to return to the permissible
working area with the negative offset angle.
Siemens AG, 2002. All rights reserved
9-354 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
Insert intermediate block at contour corners,
TLIFT
A t one corner of the contour the tangent changes
and thus the setpoint position of the following axis.
The axis normally tries to compensate this step
change at its maximum possible velocity. However,
this causes a deviation from the desired tangential
position over a certain distance on the contour after
the corner. If such a deviation is unacceptable for
technological reasons, the instruction TILIFT can be
used to force the control to stop at the corner and to
turn the following axis to the new tangent direction in
an automatically generated intermediate block. The
axis is rotated at its maximum possible velocity.
The TLIFT(...) instruction must be programmed
immediately after the axis assignment with
TANG(...).
Example:
TANG(C,X,Y…)
T LIFT(C)
Deactivate TLIFT
To deactivate TLIFT, repeat the axis assignment
TANG(...) without inserting TLIFT(...) afterwards.
T he angular change limit at which an intermediate
block is automatically inserted is defined via
machine data
$MA_EPS_TLIFT_TANG_STEP.
Delete definition of a tangential follow-up
An existing user-defined tangential follow-up must
be deleted if a new tangential follow-up with the
same following axis is defined in the preparation call
TANG.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-355
9 Path Traversing Behavior 11.029.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
TANGDEL (FAxis) Delete tangential follow-up
Deletion is only possible if the coupling with
TANGOF(Faxis) is deactivated.
Programming example
Example of plane change
N10 TANG(A, X, Y,1) 1st definition of the tang. follow-up
N20 TANGON(A) Activation of the coupling
N30 X10 Y20
...
N80 TANGOF(A)
Deactivate 1st coupling
N90 TANGDEL(A)
Delete 1st definition
...
TANG(A, X, Z)
2nd definition of the tang. follow-up
TANGON(A)
... Activation of the new coupling
N200 M30
Programming example
An alarm is output.
With geometry axis switchover and TANGDEL
N10 GEOAX(2,Y1) Y1 is geo axis 2
N20 TANG(A, X, Y)
N30 TANGON(A, 90)
N40 G2 F8000 X0 Y0 I0 J50
N50 TANGOF(A)
Deactivation of follow-up with Y1
N60 TANGDEL(A)
Delete 1st definition
N70 GEOAX(2, Y2)
Y2 is the new geo axis 2
N80 TANG(A, X, Y)
2nd definition of the tang. follow-up
N90 TANGON(A, 90)
... Activation of the follow-up with 2nd def.
Siemens AG, 2002. All rights reserved
9-356 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.1 Tangential control TANG, TANGON, TANGOF, TANGDEL 9
840D 810D 840Di
NCU 572
NCU 573
Additional notes
Influence on transformations
The position of the following rotary axis can be an
input value for a transformation.
E xplicit positioning of the following axis
If an axis which is following your lead axes is
positioned explicitly the position is added to the
programmed offset angle.
All path definitions are possible: Path and positioning
axis movements.
C oupling status
Y ou can query the status of the coupling in the NC
program with the following system variable:
$AA_COUP_ACT[Axis]
0 No coupling active
1 ,2,3 Tangential follow-up active
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-357
9 Path Traversing Behavior 11.02 9.2 Coupled motion TRAILON, TRAILOF 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
9.2 Coupled motion TRAILON, TRAILOF
Programming
T RAILON(FAxis,LAxis,Coupling)
T RAILOF(FAxis,LAxis,Axis2)
Explanation of the commands and
parameters
TRAILON A ctivate and define coupled axes; modal
TRAILOF Deactivate coupled axes
F Axis Axis name of trailing axis
LAxis Axis name of trailing axis
C oupling C oupling factor = Path of coupled-motion axis/path of trailing axis
Default = 1
Function
W hen a defined leading axis is moved, the trailing
axes (= following axes) assigned to it traverse
through the distances described by the leading axis,
allowing for a coupling factor.
T ogether, the leading axis and following axis
represent coupled axes.
Applications
• Traversing of an axis by a simulated axis. The Axis
leading axis is a simulated axis and the trailing Y Axis
Axis V
axis is a real axis. The real axis can thus be Z
traversed with allowance for the coupling factor. Axis
W
• Two-sided machining with 2 combined axis pairs:
1st leading axis Y, trailing axis V
Axis
2nd leading axis Z, trailing axis W X
Siemens AG, 2002. All rights reserved
9-358 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.2 Coupled motion TRAILON, TRAILOF 9
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Sequence
Defining coupled-axis combinations, TRAILON
The coupled axes are defined and activated
simultaneously with the modal language command
TRAILON.
TRAILON(V,Y)
V = trailing axis, Y = leading axis
The number of coupled axes that can be activated
simultaneously is restricted only by the possible
combinations of axes on the machine.
Coupled motion always takes place in the basic
coordinate system (BCS).
Coupled axis types
A coupled-axis group can consist of any combination
of linear and rotary axes. A simulated axis can also
be defined as a leading axis.
Coupled-motion axes
Up to two leading axes can be assigned
simultaneously to a trailing axis. The assignment is
made in different combinations of coupled axes.
A trailing axis can be programmed with all the
available motion commands (G0, G1, G2, G3, ...). In
addition to paths defined independently, the trailing
axis also traverses the distances derived from its
leading axes, allowing for the coupling factors.
A trailing axis can also act as a leading axis for other
trailing axes. Various combinations of coupled axes
can be set up in this way.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-359
9 Path Traversing Behavior 11.02 9 .2 Coupled motion TRAILON, TRAILOF 9
840D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Coupling factor
The coupling factor specifies the desired ratio of the
paths of trailing axis and leading axis.
Path of trailing axis
Coupling factor =
Path of leading axis
If the coupling factor is not specified in the program,
a coupling factor of 1 is automatically taken as the
default.
The factor is entered as a decimal fraction (type
REAL). The input of a negative value causes
opposite traversing movements on the leading and
trailing axes.
Deactivate coupled axes
The following language command deactivates the
coupling with a leading axis:
TRAILOF(V,Y)
V = trailing axis, Y = leading axis
TRAILOF with 2 parameters deactivates the
coupling to only 1 leading axis.
If a trailing axis is assigned to 2 leading axes,
e.g. V=trailing axis and X,Y=leading axes,
TRAILOF can be called with 3 parameters to
deactivate the coupling:
TRAILOF(V,X,Y)
Siemens AG, 2002. All rights reserved
9-360 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.2 Coupled motion TRAILON, TRAILOF 9
840D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
Acceleration and velocity
The acceleration and velocity limits of the combined
axes are determined by the "weakest axis" in the
combined axis pair.
Coupling status
You can query the status of the coupling in the NC
program with the following system variable:
$AA_COUP_ACT[axis]
0 No coupling active
8 Coupled motion active
Programming example
The workpiece is to be machined on two sides with Axis
the axis configuration shown in the diagram. To do Y Axis
Axis V
this, you create 2 combinations of coupled axes. Z
Axis
W
Axis
X
…
N100 TRAILON(V,Y) Activate 1st combined axis pair
Activate 2nd combined axis pair, coupling
N110 TRAILON(W,Z,–1) factor negative: trailing axis traverses in
opposite direction to leading axis
N120 G0 Z10 Infeed of Z and W axes in opposite axis
directions
N130 G0 Y20 Infeed of Y and V axes in same axis
directions
…
N200 G1 Y22 V25 F200 Superimpose dependent and independent
movement of trailing axis "V"
…
TRAILOF(V,Y) Deactivate 1st coupled axis
TRAILOF(W,Z) Deactivate 2nd coupled axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-361
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV,
CTABSSV, CTABSEV
Programming
The following modal NC commands work with curve
tables:
(You will find explanations of the parameters at the
end of the list of functions.)
A) Main functions
Curve tables are defined in a parts program.
CTABDEF(Faxis,Laxis,n,applim, memType) Define beginning of curve table
CTABEND() Define end of curve table
CTABDEL(n) Delete a curve table
CTABDEL() Deletion of all curve tables, independently
of memType
CTABDEL(n, m) Deletion of a curve table range
CTABDEL(n, m, memType) Deletion of the curve tables of the curve
table range that are stored in memType
CTABDEL( , , memType) Deletion of all curve tables in the
specified memory
R10=CTAB(LW,n,degrees,FAxis,LAxis) Following value for a leading value
R10=CTABINV(FW,aproxLW,n,degrees,FAxis, Leading value to a following value
LAxis)
R10=CTABSSV(LV,n,degree,Faxis,Laxis) Starting value of the following axis in the
segment belonging to the LV
R10=CTABSEV(LV,n,degree,Faxis,Laxis) End value of the following axis in the
segment belonging to the LV
General form: Set a lock against deletion or
CTABLOCK(n, m, memType) overwriting.
CTABLOCK(n) Applications in the forms:
Curve table with number n
CTABLOCK(n, m) Curve tables in number range n to m
CTABLOCK() All curve tables irrespective of memory
type
CTABLOCK(, , memType) All curve tables in the specified memory
type
Siemens AG, 2002. All rights reserved
9-362 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
General form: Cancel a lock against deletion or
CTABUNLOCK(n, m, memType) overwriting.
CTABUNLOCK enables the tables
disabled with CTABLOCK. Tables that
function in an active coupling remain
disabled, i.e. they still cannot be deleted.
But the CTABLOCK lock is canceled, i.e,
as soon as locking via the active coupling
is canceled by deactivating the coupling,
this table can be deleted. It is not
necessary to call CTABUNLOCK again.
Applications in the forms:
CTABUNLOCK(n) Curve table with number n
CTABUNLOCK(n, m) Curve tables in number range n to m
CTABUNLOCK() All curve tables irrespective of memory
type
CTABUNLOCK(, , memType) All curve tables in the specified memory
type
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-363
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
For further information about leading and following
values, see Section "Axial leading value coupling"
and "Path leading value coupling" in this section.
Additional functions exist for diagnostics and
optimization of resource use. These are described in
the M3 Description of Functions.
Explanation
FAxis Following axis:
Axis that is programmed via the curve table.
LAxis Leading axis
Axis that is programmed with the leading value.
n, m Number of the curve table; n < m in CTABDEL(n, m)
The number of the curve table is unique and not dependent on the
memory type. Tables with the same number can be in the SRAM and
DRAM.
p Entry location (in memory range memType)
applim Identifier for table periodicity:
0 Table is not periodic
1 Table is periodic with regard to the leading axis
2 Table is periodic with regard to leading axis and following axis
LW Leading value
Positional value of the leading axis for which a following value is to be
calculated.
degrees Parameter name for gradient parameter
FW Following value
Positional value of the following axis for which a leading value is to be
calculated.
aproxLW Approximation solution for leading value if no specific leading value can
be determined for a following value.
FAxis,LAxis Optional specification of the following and/or leading axis
memType Optional specification of memory type of the NC: "DRAM" / "SRAM"
If no value is programmed for this parameter, the default memory type
set in MD 20905: CTAB_DEFAULT_MEMORY_TYPE is used.
Siemens AG, 2002. All rights reserved
9-364 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Function
You can use curve tables to program position and
velocity relationships between 2 axes. Y
x y
Example of substitution of mechanical cam: The 5 a0+a +a x21 2 ...
7 a +a x...
curve table forms the basis for the axial leading 0 112 ......
value coupling by creating the functional relationship
between the leading and the following value: X
With appropriate programming, the control
calculates a polynomial that corresponds to the cam
plate from the relative positions of the leading and
following axes.
Additional notes
To create curve tables the memory space must be
reserved by setting the machine data.
Definition of a curve table Following value
CTABDEF, CTABEND
= Intermediate positions
A curve table represents a parts program or a
section of a parts program which is enclosed by
CTABDEF at the beginning and CTABEND at the
end.
Within this parts program section, unique following Curve definition
axis positions are assigned to individual positions of
the leading axis by traverse statements and used as
Leading
intermediate positions in calculating the curve Definition range value
definition in the form of a polynomial up the 3rd Starting value End value
order.
As from SW 6, intermediate points for curve
definitions can be calculated in the form of an up to
5th order polynomial.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-365
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Starting and end value of the curve table:
The starting value for the beginning of the definition
range of the curve table are the first associated axis
positions specified (the first traverse statement)
within the curve table definition. The end value of the
definition range of the curve table is determined in
accordance with the last traverse command.
Within the definition of the curve table, you have use
of the entire NC language.
Additional notes
The following are not permissible:
• Preprocess stop
• Jumps in the leading axis movement (e.g. on
changing transformations)
• Traverse statement for the following axis only
• Reversal of the leading axis, i.e. position of the
leading axis must always be unique
• CTABDEF and CTABEND statement on various
program levels.
SW 6.3
Depending on MD 20900
CTAB_ENABLE_NO_LEADMOTION, jumps of the
following axis can be tolerated if leading axis motion
is missing. The other restrictions give in the notice
still apply.
Specification of the NC memory type can be used in
table creation and deletion.
A ll modal statements that are made within the curve
table definition are invalid when the table definition is
completed. The parts program in which the table
definition is made is therefore located in front of and
after the table definition in the same state.
R parameter assignments are reset.
Siemens AG, 2002. All rights reserved
9-366 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
E xample:
...
R10=5 R11=20
...
CTABDEF
G1 X=10 Y=20 F1000
R10=R11+5 ;R10=25
X=R10
CTABEND
... ;R10=5
Repeated use of curve tables
The function relation between the leading axis and
the following axis calculated through the curve table
is retained under the table number beyond the end
of the parts program and during power-off.
The curve table created can be applied to any axis
combinations of leading and following axes whatever
axes were used to create the curve table.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-367
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
B ehavior at the edges of the curve table
N on-periodic curve table Following value
If the leading value is outside the definition range,
the following value output is the upper or lower limit.
F
F
Leading
L Definition range L value
Periodic curve table Following value
If the leading value is outside the definition range,
the leading value is evaluated modulo of the
definition range and the corresponding following
value is output.
F
Leading
L value
Definition range
Siemens AG, 2002. All rights reserved
9-368 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Reading table positions, CTAB, CTABINV
With CTAB you can read the following value for a
leading value directly from the parts program or from Following value Following value
synchronized actions (Chapter 10).
degrees degrees
W ith CTABINV, you can read the leading value for a
FW FW
following value. This assignment does not always
have to be unique. CTABINV therefore requires an
approximate value (aproxLW) for the expected
leading value. CTABINV returns the leading value
that is closest to the approximate value. The
LW Leading LW Leading
approximate value can be the leading value from the value value
previous interpolation cycle. approx.
B oth functions also output the gradient of the table
function at the correct position to the gradient
parameter (degrees). In this way, the you can
calculate the speed of the leading or following axis at
the corresponding position.
Reading segment positions, CTABSSV,
CTABSEV
C TABSSV can be used to read the starting value of
the curve segment belonging to the specified leading
value directly from the parts program or from
synchronous actions (Chapter 10).
C TABSEV can be used to read the end value of the
curve segment belonging to the specified leading
value directly from the parts program or from
synchronous actions (Chapter 10).
Additional notes
Optional specification of the leading or following axis
for CTAB/CTABINV/CTABSSV/CTABSEV is
important if the leading and following axes are
configured in different length units.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-369
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
Use of CTABSSV and CTABSEV
N10 DEF REAL STARTPOS
N20 DEF REAL ENDPOS
N30 DEF REAL GRADIENT
...
Beginning of table definitionN100 CTABDEF(Y,X,1,0)
N110 X0 Y0 Starting position 1st table segment
N120 X20 Y10 E nd position 1st table segment = start
N130 X40 Y40 position 2nd table segment ...
N140 X60 Y10
N150 X80 Y0
N 160 CTABEND End of table definition
...
N 200 STARTPOS = CTABSSV(30.0, 1,
S tart position Y in segment 2 = 10
GRADIENT)
...
N 210 ENDPOS = CTABSEV(30.0, 1, End position Y in segment 2 = 40
GRADIENT) Segment 2 belongs to LV X = 30.0.
Deleting curve tables, CTABDEL
With CTABDEL you can delete the curve tables.
Curve tables that are active in a coupling cannot be
deleted. If at least one curve table is active out of a
multiple delete command
C TABDEL() or CTABDEL(n, m) in a coupling, none
of the addressed curve tables will be deleted.
As from SW 6.3, curve tables of a certain memory
type can be deleted by optional memory type
specification.
Siemens AG, 2002. All rights reserved
9-370 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
O verwriting curve tables
A curve table is overwritten as soon as is number is
used in another table definition. Active tables cannot
be overwritten.
Additional notes
N o warning is output when you overwrite curve
tables!
Additional notes
With the system variable $P_CTABDEF it is possible
to query from inside a parts program whether a
curve table definition is active.
The parts program section can be used as a curve
table definition after excluding the statements and
therefore as a real parts program again.
Programming example
A program section is to be used unchanged for
defining a curve table. The command for preprocess
stop STOPRE can remain and is active again
immediately as soon as the program section is not
used for table definition and CTABDEF and
CTABEND have been removed:
C TABDEF(Y,X,1,1)
…
…
I F NOT ($P_CTABDEF)
STOPRE
ENDIF
…
…
CTABEND
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-371
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
C urve tables and various operating states
During active block search, calculation of curve
tables is not possible. If the target block is within the
definition of a curve table, an alarm is output when
CTABEND is reached.
Programming example 1
Y
Definition of a curve table
6
5
4
3
2
1 X
5 20 100 150 180
N100 CTABDEF(Y,X,3,0) Beginning of the definition of a non-periodic
curve table with number 3
N 110 X0 Y0 1. Traverse statement defines starting
values and 1st intermediate point:
Leading value: 5; Following value: 0
N120 X20 Y0 2 . Intermediate point: Leading value: 0...20;
Following value:
Starting value...0
N 130 X100 Y6 3 . Intermediate point: Leading value:
20...100;
Following value: 0…6
N 140 X150 Y6 4. Intermediate point: Leading value:
100...150;
Following value: 6…6
N150 X180 Y0 5. Intermediate point: Leading value:
150...180;
Following value: 6…0
N200 CTABEND End of the definition; The curve table is
generated in its internal representation as
a polynomial up to the 3rd order;
Siemens AG, 2002. All rights reserved
9-372 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior9.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
The calculation of the curve definition
depends on the modally selected
interpolation type (circle, linear, spline
interpolation); The parts program state
before the beginning of the definition is
restored.
Programming example 2
Definition of a periodic curve table with number 2,
leading value range 0 to 360, following axis motion
from 0 to 45 and back to 0:
N 10 DEF REAL DEPPOS;
N 20 DEF REAL GRADIENT;
N 30 CTABDEF(Y,X,2,1) Beginning of definition
N40 G1 X=0 Y=0
N50 POLY
N 60 PO[X]=(45.0)
N70 PO[X]=(90.0) PO[Y]=(45.0,135.0,-
90)
N 80 PO[X]=(270.0)
N90 PO[X]=(315.0) PO[Y]=(0.0,-
135.0,90)
N 100 PO[X]=(360.0)
N110 CTABEND End of definition
T est of the curve by coupling Y to X:
N120 G1 F1000 X0
N130 LEADON(Y,X,2)
N140 X360
N150 X0
N160 LEADOF(Y,X)
R ead the table function for leading value 75.0:
N170 DEPPOS=CTAB(75.0,2,GRADIENT)
P ositioning of the leading and the following axis:
N180 G0 X75 Y=DEPPOS
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-373
9 Path Traversing Behavior 11.029.3 Curve tables, CTABDEF, CTABEND, CTABDEL, CTAB, CTABINV, 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
A fter activating the coupling no synchronization of
the following axis is required:
N190 LEADON(Y,X,2)
N200 G1 X110 F1000
N210 LEADOF(Y,X)
N220 M30
Siemens AG, 2002. All rights reserved
9-374 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.4 Axial leading value coupling, LEADON, LEADOF 9
840D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
9.4 Axial leading value coupling, LEADON, LEADOF
Programming
LEADON(FAxis,LAxis,n)
LEADOF(FAxis,LAxis,n)
Explanation
L EADON A ctivate leading value coupling
LEADOF Deactivate leading value coupling
F Axis Following axis
L Axis Leading axis
n Curve table number
Function
W ith the axial leading value coupling, a leading and
Y
a following axis are moved in synchronism. It is
possible to assign the position of the following axis
via a curve table or the resulting polynomial uniquely
to a position of the leading axis – simulated if
necessary. X
Leading axis is the axis which supplies the input
values for the curve table. Following axis is the axis
which takes the positions calculated by means of the
curve table.
T he leading value coupling can be activated and
deactivated both from the parts program and during
the movement from synchronized actions
(Chapter 10).
The leading value coupling always applies in the
basic coordinate system.
F or information about creating curve table, see
Chapter "Curve tables" in this chapter. For
information about leading value coupling, see /FB/,
M3, Coupled Motion and Leading Value Coupling.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-375
9 Path Traversing Behavior 11.02 9.4 Axial leading value coupling, LEADON, LEADOF 9
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Sequence
L eading value coupling requires synchronization of
the leading and the following axes. This
synchronization can only be achieved if the following
axis is inside the tolerance range of the curve
definition calculated from the curve table when the
leading value coupling is activated.
T he tolerance range for the position of the following
axis is defined via machine data 37200 Y
COUPLE_POS_TOL_COARSE.
If the following axis is not yet at the correct position
when the leading value coupling is activated, the
s
synchronization run is automatically initiated as soon axi ding
win
g
cco
r
as the position setpoint value calculated for the ollo a leF sitio
n ab
o rve
t
following axis is approximately the real following axis pFollowing axis position to c
u
position. During the synchronization procedure the
following axis is traversed in the direction that is
defined by the setpoint speed of the following axis
(calculated from master spindle and CTAB).
Y
Additional notes
If the following axis position calculated moves away
from the current following axis position when the
leading value coupling is activated, it is not possible
to establish synchronization.
Actual value and setpoint coupling
T he following can be used as the leading value, i.e.
as the output values for position calculation of the
following axis:
• Actual values of the leading axis position: Actual
value coupling
• Setpoints of the leading axis position: Setpoint
coupling
Siemens AG, 2002. All rights reserved
9-376 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9 .4 Axial leading value coupling, LEADON, LEADOF 9
840D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Additional notes
S etpoint coupling provides better synchronization of
the leading and following axis than actual value
coupling and is therefore set by default. NCU
Setpoint coupling is only possible if the leading and Setpoint coupling
Ax1 Ax2
following axis are interpolated by the same NCU. Actual value coupling
With an external leading axis, the following axis can
only be coupled to the leading axis via the actual
values.
NCU 1 NCU 2
Ax1 Ax2
Actual value coupling
Switchover between actual and setpoint coupling
A switchover can be programmed via setting data
$SA_LEAD_TYPE
Y ou must always switch between the actual-value
and setpoint coupling when the following axis stops.
It is only possible to resynchronize after switchover
when the axis is motionless.
Application example:
Y ou cannot read the actual values without error
during large machine vibrations. If you use leading
value coupling in press transfer, it might be
necessary to switchover from actual-value coupling
to setpoint coupling in the work steps with the
greatest vibrations.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-377
9 Path Traversing Behavior 11.02 9.4 Axial leading value coupling, LEADON, LEADOF 9
840D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Leading value simulation with setpoint simulation
V ia machine data, you can disconnect the
interpolator for the leading axis from the servo. In
this way you can generate setpoints for setpoint
coupling without actually moving the leading axis.
L eading values generated from a setpoint link can
be read from the following variables so that they can
be used, for example, in synchronized actions:
- $AA_LEAD_P Leading value position
- $AA_LEAD_V Leading value velocity
Additional notes
A s an option, leading values can be generated with
other self-programmed methods. The leading values
generated in this way are written into the variables
- $AA_LEAD_SP Leading value position
- $AA_LEAD_SV Leading value velocity
a nd read from them. Before you use these variables,
setting data $SA_LEAD_TYPE = 2 must be set.
S tatus of coupling
You can query the status of the coupling in the NC
program with the following system variable:
$AA_COUP_ACT[axis]
0 No coupling active
16 Leading value coupling active
Deactivate leading value coupling, LEADOF
W hen you deactivate the leading value coupling, the
following axis becomes a normal command axis
again!
Axial leading value coupling and different
operating states
D epending on the setting in the machine data, the
leading value couplings are deactivated with RESET.
Siemens AG, 2002. All rights reserved
9-378 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.4 Axial leading value coupling, LEADON, LEADOF 9
840D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Programming example
I n a pressing plant, an ordinary mechanical coupling
between a leading axis (stanchion shaft) and axis of
a transfer system comprising transfer axes and
auxiliary axes is to be replaced by an electronic
coupling system.
I t demonstrates how a mechanical transfer system is
replaced by an electronic transfer system. The
coupling and decoupling events are implemented as
static synchronized actions.
F rom the leading axis LW (stanchion shaft), transfer
axes and auxiliary axes are controlled as following
axes that are defined via curve tables.
F ollowing axes X Feed or longitudinal axis
YL Closing or lateral axis
ZL Stroke axis
U Roller feed, auxiliary axis
V Guiding head, auxiliary axis
W Greasing, auxiliary axis
Status management
S witching and coupling events are managed via real-
time variables:
$AC_MARKER[i]=n i Marker number
with: n Status value
Actions
T he actions that occur include, for example, the following synchronized actions:
• Activate coupling, LEADON(following axis, leading axis, curve table number)
• Deactivate coupling, LEADOF(following axis, leading axis)
• Set actual value, PRESETON(axis, value)
• Set marker, $AC_MARKER[i]=value
• Coupling type: real/virtual leading value
• Approaching axis positions, POS[axis]=value
Conditions
Fast digital inputs, real-time variables $AC_MARKER and position comparisons are linked using
the Boolean operator AND for evaluation as conditions.
N ote
I n the following example, line change, indentation and bold type are used for the sole purpose of
improving readability of the program. To the controller, everything that follows a line number
constitutes a single line.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-379
9 Path Traversing Behavior 11.02 9.4 Axial leading value coupling, LEADON, LEADOF 9
840D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
C omment
; Defines all static synchronized actions.
; **** Reset marker
N2 $AC_MARKER[0]=0 $AC_MARKER[1]=0
$AC_MARKER[2]=0 $AC_MARKER[3]=0
$AC_MARKER[4]=0 $AC_MARKER[5]=0
$AC_MARKER[6]=0 $AC_MARKER[7]=0
; **** E1 0=>1 Coupling transfer ON
N10 IDS=1 EVERY ($A_IN[1]==1) AND
($A_IN[16]==1) AND ($AC_MARKER[0]==0)
DO LEADON(X,LW,1) LEADON(YL,LW,2)
LEADON(ZL,LW,3) $AC_MARKER[0]=1
; **** E1 0=>1 Coupling roller feed ON
N20 IDS=11 EVERY ($A_IN[1]==1) AND
($A_IN[5]==0) AND ($AC_MARKER[5]==0)
DO LEADON(U,LW,4) PRESETON(U,0)
$AC_MARKER[5]=1
; **** E1 0->1 Coupling guide head ON
N21 IDS=12 EVERY ($A_IN[1]==1) AND
($A_IN[5]==0) AND ($AC_MARKER[6]==0)
DO LEADON(V,LW,4) PRESETON(V,0)
$AC_MARKER[6]=1
; **** E1 0->1 Coupling greasing ON
N22 IDS=13 EVERY ($A_IN[1]==1) AND
($A_IN[5]==0) AND ($AC_MARKER[7]==0)
DO LEADON(W,LW,4) PRESETON(W,0)
$AC_MARKER[7]=1
; **** E2 0=>1 Coupling OFF
N30 IDS=3 EVERY ($A_IN[2]==1)
DO LEADOF(X,LW) LEADOF(YL,LW)
LEADOF(ZL,LW) LEADOF(U,LW)
LEADOF(V,LW) LEADOF(W,LW) $AC_MARKER[0]=0
$AC_MARKER[1]=0 $AC_MARKER[3]=0
$AC_MARKER[4]=0 $AC_MARKER[5]=0
$AC_MARKER[6]=0 $AC_MARKER[7]=0
....
N110 G04 F01
N120 M30
Siemens AG, 2002. All rights reserved
9-380 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO 9
840D 840D 840Di
NCU 571 NCU 572
NCU 573
9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO
Programming
F … FNORM
F… FLIN
F… FCUB
F=FPO(…,…,…)
Explanation
FNORM Basic setting. The feed value is specified as a function of the traverse
path of the block and is then valid as a modal value.
FLIN Path velocity profile linear:
The feed value is approached linearly via the traverse path from the
current value at the block beginning to the block end and is then valid as
a modal value.
FCUB Path velocity profile cubic:
T he non-modally programmed F values are connected by means of a
spline referred to the block end point. The spline begins and ends
tangentially with the previous and the following feedrate specification.
If the F address is missing from a block, the last F value to be
programmed is used.
F=FPO… Polynomial path velocity profile:
The F address defines the feed characteristic via a polynomial from the
current value to the block end. The end value is valid thereafter as a
modal value.
Function
To permit flexible definition of the feed characteristic,
the feed programming according to DIN 66205 has
been extended by linear and cubic characteristics.
The cubic characteristics can be programmed either
directly or as interpolating splines.
These additional characteristics make it possible to
program continuously smooth velocity characteristics
depending on the curvature of the workpiece to be
machined.
These additional characteristics make it possible to
program continuously smooth velocity characteristics
depending on the curvature of the workpiece to be
machined.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-381
9 Path Traversing Behavior 11.02 9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO 9
840D 840D 8 40Di
NCU 571 NCU 572
NCU 573
Sequence
FNORM
The feed address F defines the path feed as a Feedrate
constant value according to DIN 66025.
Please refer to Programming Guide "Fundamentals"
for more detailed information on this subject.
Path
FLIN
Feedrate
T he feed characteristic is approached linearly from
the current feed value to the programmed F value
until the end of the block.
Example:
N30 F1400 FLIN X50
Path
Siemens AG, 2002. All rights reserved
9-382 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO 9
840D 840D 8 40Di
NCU 571 NCU 572
NCU 573
F CUB Feedrate
T he feed is approached according to a cubic
characteristic from the current feed value to the
programmed F value until the end of the block. The
control uses splines to connect all the feed values
programmed non-modally that have an active FCUB.
The feed values act here as interpolation points for
calculation of the spline interpolation.
Example:
N50 F1400 FCUB X50
N60 F2000 X47 Path
N70 F3800 X52
…
F=FPO(…,…,…)
Feedrate
T he feed characteristic is programmed directly via a
polynomial. The polynomial coefficients are specified
according to the same method used for polynomial
interpolation.
Example:
F =FPO(endfeed, quadf, cubf)
endfeed, quadf and cubf are previously
defined variables.
Path
endfeed: Feed at block end
quadf: Quadratic polynomial coefficient
c ubf: Cubic polynomial coefficient
W ith an active FCUB, the spline is linked tangentially
to the characteristic defined via FPO at the block
beginning and block end.
Supplementary conditions
The functions for programming the path traversing
characteristics apply regardless of the programmed
feed characteristic.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-383
9 Path Traversing Behavior 11.02 9.5 Feed characteristic, FNORM, FLIN, FCUB, FPO 9
840D 8 40D 840Di
NCU 571 NCU 572
NCU 573
T he programmed feed characteristic is always
absolute regardless of G90 or G91.
Additional notes
Compressor
W ith an active compressor COMPON the following
applies when several blocks are joined to form a
spline segment:
FNORM:
T he F word of the last block in the group applies to
the spline segment.
F LIN:
The F word of the last block in the group applies to
the spline segment.
The programmed F value applies until the end of the
segment and is then approached linearly.
F CUB:
T he generated feed spline deviates from the
programmed end points by an amount not exceeding
the value set in machine data
$MC_COMPESS_VELO_TOL
F=FPO(…,…,…)
These blocks are not compressed.
Feed optimization on curved path sections
F eed polynomial F-FPO and feed spline FCUB
should always be traversed at constant cutting rate
CFC, thereby allowing a jerk-free setpoint feed
profile to be generated. This enables creation of a
continuous acceleration setpoint feed profile.
Siemens AG, 2002. All rights reserved
9-384 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9 .5 Feed characteristic, FNORM, FLIN, FCUB, FPO 9
840D 840D 840Di
NCU 571 NCU 572
NCU 573
Programming example
T his example shows you the programming and Feedrate
graphic representation of various feed profiles.
5000
4000
3000
2000
1000
Path
N N N N N N N N N N N N N N N
1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
N1 F1000 FNORM G1 X8 G91 G64 C onstant feed profile, incremental dimensioning
N2 F2000 X7 S tep change in setpoint velocity
N 3 F=FPO(4000, 6000, -4000) Feed profile via polynomial with feed 4000 at
block end
N 4 X6 P olynomial feed 4000 applies as modal value
N5 F3000 FLIN X5 L inear feed profile
N6 F2000 X8 L inear feed profile
N7 X5 L inear feed applies as modal value
N 8 F1000 FNORM X5 Constant feed profile with abrupt change in
acceleration rate
N9 F1400 FCUB X8 All subsequent, non-modally programmed F
values are connected via splines
N10 F2200 X6
N11 F3900 X7
N12 F4600 X7
N13 F4900 X5 D eactivate spline profile
N14 FNORM X5
N15 X20
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-385
9 Path Traversing Behavior 11.02 9.6 Program run with preprocessing memory, STARTFIFO, STOPFIFO, 9
840D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
9.6 Program run with preprocessing memory, STARTFIFO, STOPFIFO, STOPRE
Explanation of the commands
STOPFIFO Stop high-speed processing section, fill preprocessing memory, until
STARTFIFO, "Preprocessing memory full" or "End of program" is
detected.
S TARTFIFO Start of high-speed processing section, in parallel to filling the
preprocessing memory
STOPRE P reprocessing stop
Function
Depending on its expansion level, the control system
has a certain quantity of so-called preprocessing
memory in which prepared blocks are stored prior to
program execution and then output as high-speed NC program Preprocessing
block sequences while machining is in progress. memory
These sequences allow short paths to be traversed
at a high velocity.
P rovided that there is sufficient residual control time
available, the preprocessing memory is always filled.
STARTFIFO stops the machining process until the
Machining in process
preprocessing memory is full or until STOPFIFO or (blocks output in fast succession)
STOPRE is detected.
Sequence
Mark processing section
The high-speed processing section to be buffered
in the preprocessing memory is marked at the
beginning and end with STARTFIFO and STOPFIFO
respectively.
Example:
N10 STOPFIFO
N20…
N100
N110 STARTFIFO
Execution of these blocks does not begin until the
preprocessing memory is full or command STARTFIFO
is detected.
Siemens AG, 2002. All rights reserved
9-386 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.6 Program run with preprocessing memory, STARTFIFO, STOPFIFO, 9
840D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Restrictions
T he preprocessing memory is not filled or the filling
process interrupted if the processing section
contains commands that require unbuffered
operation (reference point approach, measuring
functions, ...).
Stop preprocessing
When STOPRE is programmed, the following block is
not processed until all previously prepared and stored
blocks have been fully executed. The previous block is
halted with exact stop (as for G9).
Example:
N 10 …
N30 MEAW=1 G1 F1000 X100 Y100 Z50
N40 STOPRE
The control system initiates an internal preprocessing
stop while status data of the machine ($A...) are
accessed.
Example:
R10 = $AA_IM[X] ;Read actual value of X axis
N ote
When a tool offset or spline interpolations are active,
you should not program the STOPRE command as
this will lead to interruption in contiguous block
sequences.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-387
9 Path Traversing Behavior 11.02 9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH 9
8 40D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH
Programming
R EPOSA RMI DISPR=… or REPOSA RMB or REPOSA RME
R EPOSL RMI DISPR=… or REPOSL RMB or REPOSL RME
R EPOSQ RMI DISPR=… DISR=… or REPOSQ RMB DISR=… or REPOSQ RME DISR=… or REPOSQA
DISR=…
REPOSH RMI DISPR=… DISR=… or REPOSH RMB DISR=… or REPOSH RME DISR=… or
R EPOSHA DISR=…
Explanation of the commands
A pproach path
REPOSA A pproach along line on all axes
R EPOSL A pproach along line
REPOSQ DISR=… Approach along quadrant with radius DISR
REPOSQA DISR=… Approach on all axes along quadrant with radius DISR
REPOSH DISR=… A pproach along semi-circle with diameter DISR
R EPOSHA DISR=… Approach on all axes along semi-circle with diameter DISR
R epositioning point
RMI Approach interruption point
RMI DISPR=… Entry point at distance DISPR in mm/inch in front of interruption point
RMB Approach block start point
RME DISPR=… A pproach block end point at distance DISPR in front of end point
A0 B0 C0 Axes in which approach is to be made
Siemens AG, 2002. All rights reserved
9-388 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH 9
840D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Function
If you interrupt the program run and retract the tool
during the machining operation because, for
example, the tool has broken or you wish to check a
measurement, you can reposition at any selected
point on the contour under control by the program.
REPOS The REPOS command acts in the same way as a
subprogram return jump (e.g. via M17). Blocks
programmed after the command in the interrupt
routine are not executed.
For information about interrupting program runs, see
also Section "Interrupt routine" in Programming Guide
"Advanced".
Sequence
D efining repositioning point Y
W ith reference to the NC block in which the program Block end point
run has been interrupted, it is possible to select one
Interruption point
of three different repositioning points: RME
Block start
• RMI, interruption point RMI point
RMB, block start point or last end point
• RME, block end point RMB
R MI DISPR=… or RME DISPR=… allows you to
select a repositioning point which sits before the
interruption point or the block end point. X
D ISPR=... allows you to describe the contour
distance in mm/inch between the repositioning point
and the interruption before the end point. Even for
high values, this point cannot be further away than
the block start point.
If no DISPR=… command is programmed, then
DISPR=0 applies and with it the interruption point
(with RMI) or the block end point (with RME).
SW 5.2 and higher:
The sign before DISPR is evaluated.
In the case of a plus sign, the behavior is as
previously.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-389
9 Path Traversing Behavior 11.02 9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH 9
8 40D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
In the case of a minus sign, approach is behind the
interruption point or, with RMB, behind the block start
point.
The distance between interruption point and
approach point depends on the value of DISPR.
Even for higher values, this point can lie in the block
end point at the maximum.
Application example:
A sensor will recognize the approach to a clamp. An
ASUB is initiated to bypass the clamp. Afterwards, a
negative DISPR is repositioned on one point behind
the clamp and the program is continued.
A pproach with new tool
T he following applies if you have stopped the
Y
program run due to tool breakage:
When the new D number is programmed, the
machining program is continued with modified tool
offset values at the repositioning point.
W here tool offset values have been modified, it may
not be possible to reapproach the interruption point.
In such cases, the point closest to the interruption
point on the new contour is approached (possibly
modified by DISPR). X
Approach contour
The motion with which the tool is repositioned on the
contour can be programmed. Enter zero for the
addresses of the axes to be traversed.
Commands REPOSA, REPOSQA and REPOSHA
automatically reposition all axes. Individual axis
names need not be specified.
Siemens AG, 2002. All rights reserved
9-390 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
9 11.02 Path Traversing Behavior 9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH 9
8 40D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
W hen commands REPOSL, REPOSQ and
REPOSH are programmed, all geometry axes are
traversed automatically, i.e. they need not be named
in the command. All other axes to be repositioned
must be specified in the commands.
A pproach along a straight line, REPOSA,
REPOSL
Y Interruption point
The tool approaches the repositioning point along a
straight line.
DI
All axes are automatically traversed with command SPR
REPOSA. With REPOSL you can specify which REPOSLRepositioning
axes are to be moved. point
E xample:
REPOSL RMI DISPR=6 F400
or
REPOSA RMI DISPR=6 F400 X
Approach along quadrant, REPOSQ, REPOSQA
The tool approaches the repositioning point along a
Y IntermediateD
quadrant with a radius of DISR=.... The control IS pointR
system automatically calculates the intermediate
point between the start and repositioning points.
REPOSQ
Repositioning
Example: point
R EPOSQ RMI DISR=10 F400
Start point
X
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 9-391
9 Path Traversing Behavior 11.02 9.7 Repositioning on contour, REPOSA, REPOSL, REPOSQ, REPOSH 9
840D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Approach along semi-circle, REPOSH, REPOSHA
Intermediate
The tool approaches the repositioning point along a
Y point
semi-circle with a diameter of DISR=.... The control R
IS
system automatically calculates the intermediate D
point between the start and repositioning points.
Start point
Example:
REPOSH RMI DISR=20 F400
Repositioning
point
X
The following applies to circular motions
REPOSH and REPOSQ:
The circle is traversed in the specified working
planes G17 to G19.
I f you specify the third geometry axis (infeed
direction) in the approach block, the repositioning
point is approached along a helix in case the tool
position and programmed position in the infeed
direction do not coincide.
I n the following cases, the control automatically
switches over to linear approach REPOSL:
Y ou have not specified a value for DISR.
• No defined approach direction is available
(program interruption in a block without travel
information).
• With an approach direction that is perpendicular
to the current working plane.
Siemens AG, 2002. All rights reserved
9-392 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10
Motion-Synchronous Action
10.1 Structure, basic information ........................................................................................ 10-395
10.1.1 Programming and command elements................................................................ 10-397
10.1.2 Validity range: Identification number ID ............................................................... 10-398
10.1.3 Vocabulary word .................................................................................................. 10-399
10.1.4 Actions ................................................................................................................. 10-402
10.1.5 Overview of synchronized actions........................................................................ 10-404
10.2 Basic modules for conditions and actions ................................................................... 10-406
10.3 Special real-time variables for synchronized actions .................................................. 10-409
10.3.1 Flags/counters $AC_MARKER[n] ........................................................................ 10-409
10.3.2 Timer variable $AC_TIMER[n], SW 4 and higher ................................................ 10-409
10.3.3 Synchronized action parameters $AC_PARAM[n]............................................... 10-410
10.3.4 Access to R parameters $Rxx ............................................................................. 10-411
10.3.5 Machine and setting data read/write (SW 4 and higher)...................................... 10-412
10.3.6 FIFO variable $AC_FIFO1[n] … $AC_FIFO10[n] (SW 4 and higher).................. 10-413
10.4 Actions within synchronized actions............................................................................ 10-415
10.4.1 Auxiliary functions output ..................................................................................... 10-415
10.4.2 Set read-in disable RDISABLE ............................................................................ 10-416
10.4.3 Cancel preprocessing stop STOPREOF ............................................................. 10-417
10.4.4 Deletion of distance-to-go .................................................................................... 10-418
10.4.5 Delete distance-to-go with preparation, DELDTG, DELDTG ("Axis 1 to x") ........ 10-418
10.4.6 Polynomial definition, FCTDEF, block-synchronized ........................................... 10-420
10.4.7 Laser power control ............................................................................................. 10-422
10.4.8 Evaluation function SYNFCT ............................................................................... 10-423
10.4.9 Adaptive control (additive).................................................................................... 10-424
10.4.10 Adaptive control (multiplicative) ........................................................................... 10-425
10.4.11 Clearance control with limited compensation....................................................... 10-426
10.4.12 Online tool offset FTOC ....................................................................................... 10-428
10.4.13 Positioning movements........................................................................................ 10-430
10.4.14 Position axis POS ................................................................................................ 10-432
10.4.15 Start/stop axis MOV............................................................................................. 10-432
10.4.16 Axial feed FA........................................................................................................ 10-433
10.4.17 SW limit switch..................................................................................................... 10-434
10.4.18 Axis coordination.................................................................................................. 10-434
10.4.19 Set actual value.................................................................................................... 10-436
10.4.20 Spindle motions ................................................................................................... 10-437
10.4.21 Coupled-axis motion TRAILON, TRAILOF .......................................................... 10-438
10.4.22 Leading value coupling LEADON, LEADOF ........................................................ 10-439
10.4.23 Measurement ....................................................................................................... 10-441
10.4.24 Set/clear wait marks: SETM, CLEARM (SW 5.2 and higher) .............................. 10-441
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-393
10 Motion-Synchronous Action 11.02 10
10.4.25 Error responses....................................................................................................10-442
10.4.26 Travel to fixed stop FXS and FOCON/FOCOF....................................................10-442
10.5 Technology cycles .......................................................................................................10-445
10.5.1 Lock, unlock, reset: LOCK, UNLOCK, RESET ....................................................10-447
10.6 Cancel synchronized action: CANCEL ........................................................................10-449
10.7 Supplementary conditions ...........................................................................................10-450
Siemens AG, 2002. All rights reserved
10-394 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
10.1 Structure, basic information
Function
Synchronized actions allow you to start different
actions from the current parts program and to execute Part program
them synchronously.
Block preparation
The starting point of these actions can be defined
with conditions evaluated in real time (in interpolation
Prepared blocks
cycles). The actions are therefore responses to real- Conditions Actions
time events, execution of them is not limited by block NCK inputs NCK outputs
Setpoints Positions
boundaries. Actual values VelocitiesRealtime processing
Polynomial
A synchronized action also contains information Synchronous actionscoefficients NC functionsLogic operations
Measuring
about the effectiveness of the actions and about the Parameters Switch on link
Flags M/H function
frequency with which the programmed real-time Servo values output
Change polynom.
variables are scanned and therefore about the coefficients
frequency with which the actions are started. In this
way, an action can be triggered just once or
cyclically in interpolation cycles.
Programming
DO Action1 Action2 …
VOCABULARY_WORD condition DO action1 action2 ...
ID=n VOCABULARY_WORD condition DO action1 action2 ...
IDS=n VOCABULARY_WORD condition DO action1 action2 ...
Explanation
Identification number ID/IDS
ID=n Modal synchronized actions in automatic mode,
local to program; n = 1... 255
IDS=n Modal synchronized actions in each mode,
static; n = 1... 255
Without ID/IDS Non-modal synchronized actions in automatic mode
Vocabulary word
No vocabulary word Execution of the action is not subject to any condition. The action is
executed cyclically in any interpolation cycles.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-395
10 Motion-Synchronous Action 11.02 1 0.1 Structure, basic information 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
WHEN The condition is tested until it is fulfilled once, the associated action
is executed once.
WHENEVER The condition is tested cyclically. The associated action is executed
cyclically while the condition is fulfilled.
FROM After the condition has been fulfilled once, the action is executed
cyclically while the synchronized action is active.
EVERY The action is initiated once when the condition is fulfilled and is
executed again when the condition changes from the FALSE state to
the TRUE state. The condition is tested cyclically. Every time the
condition is fulfilled, the associated action is executed.
Condition Gating logic for real-time variables, the conditions are checked in the
interpolation cycle.
In SW 5 and higher, the G codes can be programmed in synchronized
actions for condition evaluation.
DO Triggers the action if the condition is fulfilled.
Action Action started if the condition is fulfilled, e.g. assign variable,
activate axis coupling, set NCK outputs, output M and H functions, ...
In SW 5 and higher, the G codes can be programmed in synchronized
actions for actions/technology cycles.
Coordination of synchronized actions/technology cycles
CANCEL[n] Cancel synchronized action
LOCK[n] Inhibit technology cycle
UNLOCK[n] Enable technology cycle
RESET Reset technology cycle
Programming example
WHEN $AA_IW[Q1]>5 DO M172 H510 ;If the actual value of axis Q1 exceeds 5 mm, auxiliary
functions M172 and H510 are output to the PLC interface.
If real-time variables occur in a parts program
(e.g. actual value, position of a digital input or output
etc.), preprocessing is stopped until the previous block
has been executed and the values of the real-time
variables obtained.
The real-time variables used are evaluated in
interpolation cycles.
Advantages with synchronized actions:
Preprocessing is not stopped.
Siemens AG, 2002. All rights reserved
10-396 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
Possible applications:
• Optimization of runtime-critical applications
(e.g. tool changing)
• Fast response to an external event
• Programming AC controls
• Setting up safety functions
• ....
10.1.1 Programming and command elements
Function
A synchronized action is programmed on its own in a
separate block and triggers a machine function in
the next executable block (e.g. traversing movement
with G0, G1, G2, G3; block with auxiliary function
output).
S ynchronized actions consist of up to five command
elements each with a different task:
A c tio n
ID n um b er: V o ca bu la ry w ord :
C o nd ition D O
S c op e o f va lid ity S ca n fre qu en cy
Technology
cycle
Example:
ID=1 WHENEVER $A_IN[1]==1 DO $A_OUT[1]=1
S ynchronized action no. 1: whenever input 1 is set t hen s et output 1
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-397
opt. G code
for condition
opt. G code for
action/techno. c.
10 Motion-Synchronous Action 11.02 10.1 Structure, basic information 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
10.1.2 Validity range: Identification number ID
Function
T he scope of validity of a synchronized action is
defined by the identification number (modal ID):
• No modal ID
The synchronized action is active in automatic mode
only. It applies only to the next executable block
(block with motion instructions or other machine
action), is non-modal.
Example:
WHEN $A_IN[3]==TRUE DO $A_OUTA[4]=10
G1 X20 ;Executable block
• ID=n; n=1...255
The synchronized action applies modally in the
following blocks and is deactivated by CANCEL(n) or
by programming a new synchronized action with the
same ID.
The synchronized actions that apply in the M30
block are also still active (if necessary deactivate
with the CANCEL command).
ID synchronized actions only apply in automatic
mode.
Example:
ID=2 EVERY $A_IN[1]==1 DO POS[X]=0
• IDS=n; n=1...255
These static synchronized actions apply modally in
all operating modes.
They can be defined not only for starting from a
parts program but also directly after power-on from
an asynchronous subprogram (ASUB) started by the
PLC. In this way, actions can be activated that are
executed regardless of the mode selected in the NC.
Example:
IDS=1 EVERY $A_IN[1]==1 DO POS[X]=100
Siemens AG, 2002. All rights reserved
10-398 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
A pplication:
• AC loops in JOG mode
• Logic operations for Safety Integrated
• Monitoring functions, responses to machine states in
all modes
Sequence of execution
S ynchronized actions that apply modally or statically
are executed in the order of their ID(S) numbers (in
the interpolation cycle).
Non-modal synchronized actions (without ID
number) are executed in the programmed sequence
after execution of the modal synchronized actions.
1 0.1.3 Vocabulary word
Function
T he vocabulary word determines how many times the
following condition is to be scanned and the associated
action executed.
• No vocabulary word: Example:
If no vocabulary word is programmed, the condition is DO $A_OUTA[1]=$AA_IN[X]
considered to be always fulfilled. The synchronous ;Output of actual value on analog
commands are executed cyclically. output
• WHEN
The condition is scanned in each interpolation cycle
until it is fulfilled once, whereupon the action is
executed once.
• WHENEVER
The condition is scanned in each interpolation cycle.
The action is executed in each interpolation cycle while
the condition is fulfilled.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-399
10 Motion-Synchronous Action 11.02 10.1 Structure, basic information 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
• FROM
The condition is tested in each interpolation cycle
until it is fulfilled once. The action is then executed
while the synchronous action is active, i.e. even if
the condition is no longer fulfilled.
• EVERY E xample:
The condition is scanned in each interpolation cycle. ID=1 EVERY $AA_IM[B]>75 DO
POS[U]=IC(10) FA[U]=900;
The action is executed once whenever the condition
When the actual value of axis B
is fulfilled.
overshoots the value 75 in
Pulse edge control: machine coordinates, the U axis
The action is initiated again when the condition should move forwards by 10 with
changes from FALSE to TRUE. an axial feed.
Condition
Defines whether an action is to be executed by comparing
two real-time variables or one real-time variable with an
expression calculated during preprocessing.
SW 4 and higher:
Results of comparisons can also be gated by Boolean
operators in the condition ().
The condition is tested in interpolation cycles. If it is
fulfilled, the associated action is executed.
SW 5 and higher:
Conditions can be specified with a G code. This means
that it is possible to have defined settings for condition
evaluation and the action/technology cycle irrespective
of the currently active parts program state. It is
necessary to decouple synchronized actions from the
programming environment because synchronized
actions are to execute their actions in the defined initial
state at any time when the trigger conditions are
fulfilled.
Application cases:
Defining the measurement systems for condition
assessment and action via G codes G70, G71, G700,
G710.
Siemens AG, 2002. All rights reserved
10-400 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
I n SW 5 only these G codes are allowed.
A specified G code for the condition applies for
assessment of the condition as well as for the
action if there is no separate G code specified for the
action.
Only one G code of the G code group may be
programmed for each condition part.
Programming example
WHENEVER $AA_IM[X] > 10.5*SIN(45) DO … Comparison with an expression
calculated during preprocessing
WHENEVER $AA_IM[X] > $AA_IM[X1] DO … Comparison with other real-time
variable
W HENEVER ($A_IN[1]==1) OR ($A_IN[3]==0) DO Two logic-gated comparisons
...
P ossible conditions:
• Comparison of real-time variables
(analog/digital inputs/outputs, etc.)
• Boolean gating of comparison results
• Computation of real-time expressions
• Time/distance from beginning of block
• Distance from block end
• Measured values, measured results
• Servo values
• Velocities, axis status
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-401
10 Motion-Synchronous Action 11.02 1 0.1 Structure, basic information 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
10.1.4 Actions
Function
I n each synchronized action, you can program one or
more actions. All actions programmed in a block are
started in the same interpolation cycle.
In SW 5 and higher, actions can be used with a G code
for the action/technology cycle. This G code specifies
another G code from the one set for the condition for all
actions in the block and technology cycles if necessary.
If there are technology cycles in the action part, then
after completion of the technology cycle the G code
continues to apply modally for all subsequent actions
until the next G code.
Only a G code from the G code group (G70, G71,
G700, G710) may be programmed.
Possible actions:
• Assign variables
• Write setting data
• Set control parameters
• DELDTG: Delete fast distance-to-go
• RDISABLE: Set read-in disable
• Output M, S and H auxiliary functions
• STOPREOF: Cancel preprocessing stop
• FTOC: Online tool offset
• Definition of evaluation functions (polynomials)
• SYNFCT: Activate evaluation functions: AC
control
• Switchover between several feedrates in a
programmed block depending on binary and
analog signals
• Feedrate overrides
• Start/position/stop positioning axes (POS) and
spindles (SPOS)
• PRESETON: Set actual value
Siemens AG, 2002. All rights reserved
10-402 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
• Activate or deactivate coupled-axis
motion/leading value coupling
• Measurement
• Set up additional safety functions
• Output of digital and analog signals
• ...
Programming example
Synchronized action with two actions
WHEN $AA_IM[Y] >= 35.7 DO M135 $AC_PARAM=50
If the condition is fulfilled, M135 is output to the PLC and the override is set to 50%.
A s the action, you can also specify a program
(single-axis program, technology cycle). This must
only comprise those actions that can also be
programmed individually in synchronized actions.
The individual actions of such a program are
executed sequentially in interpolation cycles.
N ote
Actions can be executed whatever mode is selected.
The following actions are only active in automatic mode
when the program is active
• STOPREOF,
• DELDTG.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-403
10 Motion-Synchronous Action 11.02 10.1 Structure, basic information 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
1 0.1.5 Overview of synchronized actions
SW 3.x and lower
• Programming of sequences in the interpolation cycle
at the user level (parts program)
• Response to events/statuses in the interpolation cycle
• Gating logic in real time
• Access to I/Os, control status and machine status
• Programming of cyclic sequences that are executed in
the interpolation cycle
• Triggering of specific NC functions (read-in disable,
axially overlaid motion, ... )
• Execution of technology functions in parallel with path
motion
• Triggering of technology functions regardless of block
boundaries
SW 4 and higher
• Diagnosis possible for synchronized actions
• Expansion of the main run variable used in
synchronized actions
• Complex conditions in synchronized actions
• Expansion of expressions in synchronized actions:
Combination of real-time variables with basic arith-
metic operations and functions in the interpolation
cycle, indirect addressing of main run variables via
index can be changed online
Setting data from synchronized actions can be
modified and evaluated online
• Configuration possibilities: Number of simultaneously ac-
tive synchronized actions can be set via machine data.
• Start positioning axis motion and spindles from
synchronized actions (command axes)
• Preset from synchronized actions
• Activation, deactivation, parameterization of axis
coupling: Leading value coupling, coupled-axis motion
• Activation/deactivation of axial measuring function
• Software cams
Siemens AG, 2002. All rights reserved
10-404 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.1 Structure, basic information 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
• Delete distance-to-go without stopping
preprocessing
• Single-axis programs, technology cycles
• Synchronized actions active in JOG mode beyond
the boundaries of the program
• Synchronized actions that can be influenced from
the PLC
• Protected synchronized actions
• Expansion for overlaid motion / clearance control
SW 5.x and higher
• Travel to fixed stop FXS:
Synchronized actions, triggered with FXS, FXST and
FXSW
• Travel with limited moment/force FOC:
Synchronized action is activated either modally or
non-modally with FOCON and deactivated with
FOCOF.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-405
10 Motion-Synchronous Action 11.02 1 0.2 Basic modules for conditions and actions 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
10.2 Basic modules for conditions and actions
R eal-time variables
Real-time variables are evaluated and written in the
interpolation cycle.
The real-time variables are
• $A… , main run variable,
• $V... , servo variable.
To identify them specially, these variables can be
programmed with $$:
$ AA_IM[X] is equivalent to $$AA_IM[X].
S etting and machine data must be identified with $$
when evaluation/assignment takes place in the
interpolation cycle.
A list of variables is given in the Appendix.
Calculations in real time
Calculations in real time are restricted to the data types
INT, REAL and BOOL.
Real-time expressions are calculations that can be
executed in interpolation cycles that can be used in
the condition and the action for assignment to NC
addresses and variables.
• Comparisons
In conditions, variables or partial expressions of
the same data type can be compared. The result
is always of data type BOOL.
All the usual comparison operators are
permissible (==, , , =).
• Boolean operators
Variables, constants and comparisons can be
gated using the usual Boolean operators (NOT,
AND, OR, XOR)
Siemens AG, 2002. All rights reserved
10-406 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.2 Basic modules for conditions and actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
• Bit operators
The bit operators B_NOT, B_AND, B_OR,
B_XOR can be used.
Operands are variables or constants of the
INTEGER type.
• Basic arithmetic operations
Real-time variables of types INTEGER and REAL
can be subjected to the basic arithmetic
operations, with each other or with a constant (+,
–, *, /, DIV, MOD).
• Mathematical functions
Mathematical functions cannot be applied to real-
time variables of data type REAL (SIN, COS,
TAN, ASIN, ACOS, ABS, TRUNC, ROUND, LN,
EXP, ATAN2, ATAN, POT, SQRT, CTAB,
CTABINV).
Example:
DO $AC_PARAM[3] = COS($AC_PARAM[1])
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-407
10 Motion-Synchronous Action 11.02 10.2 Basic modules for conditions and actions 10
840 D 840 D 810 D 840Di
NCU 571 NCU 572
NCU 573
Notes
Only variables of the same data type can be Correct: $R10=$AC_PARAM[1]
gated. I ncorrect: $R10=$AC_MARKER[1]
M ultiplication and division are performed before
addition and subtraction and bracketing of
expressions is permissible.
T he operators DIV and MOD are permissible for
the data type REAL (SW 4 and higher).
Example:
DO $AC_PARAM[3] = $A_INA[1]-$AA_IM[Z1] ; Subtraction of two real-time variables
WHENEVER $AA_IM[x2] < $AA_IM[x1]-1.9 DO $A_OUT[5] = 1
;Subtraction of a constant from real-time variable
DO $AC_PARAM[3] = $INA[1]-4*SIN(45.7 $P_EP[Y])*R4
;Constant expression, calculated during preprocessing
• Indexation
Real-time variables can be indexed with real-time
variables.
Notes
Variables that are not formed in real time must
not be indexed with real-time variables.
Example:
WHEN…DO $AC_PARAM[$AC_MARKER[1]] = 3
I llegal:
$AC_PARAM[1] = $P_EP[$AC_MARKER]
Programming example
E xample of real-time expressions
ID=1 WHENEVER ($AA_IM[Y]>30) AND ($AA_IM[Y]10) Output of the result of a comparison
Siemens AG, 2002. All rights reserved
10-408 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.3 Special real-time variables for synchronized actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573 CCU2
10.3 Special real-time variables for synchronized actions
T he real-time variables listed below can be used in
synchronized actions:
1 0.3.1 Flags/counters $AC_MARKER[n]
Function
F lag variablescan be read and written in
synchronized actions.
Channel-specific flags/counters
$AC_MARKER[n]
Data type: INTEGER
A channel-specific flag variable exists under the
same name once in each channel.
Example:
WHEN ... DO $AC_MARKER[0] = 2
WHEN ... DO $AC_MARKER[0] = 3
WHEN $AC_MARKER == 3 DO $AC_OVR=50
1 0.3.2 Timer variable $AC_TIMER[n], SW 4 and higher
Function
( not 840D NCU 571, FM-NC)
T he system variable $AC_TIMER[n] allows actions
to be started following defined waiting times.
Data type: REAL
Units: s
n: Number of the timer variable
• Set timer
A timer variable is incremented via value
assignment $AC_TIMER[n]=value
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-409
10 Motion-Synchronous Action 11.02 1 0.3 Special real-time variables for synchronized actions 10
8 40 D 810 D 840Di
NCU 572
NCU 573 CCU2
n: Number of the timer variable
value: Starting value (usually 0)
• Halt timer
Incrementation of a timer variable is halted by
assigning a negative value $AC_TIMER[n]=-1
• Read timer
The current time value can be read when the
timer is running or when it has stopped. When
the timer is stopped by assigning the value -1, the
most up-to-date timer value is retained and can
be read.
Example:
Output of an actual value via analog output
500 ms after detection of a digital input
WHEN $A_IN[1] == 1 DO $AC_TIMER[1]=0 ; Reset and start timer
WHEN $AC_TIMER[1]>=0.5 DO $A_OUTA[3]=$AA_IM[X] $AC_TIMER[1]=-1
1 0.3.3 Synchronized action parameters $AC_PARAM[n]
Function
D ata type: REAL
n : Number of parameter 0-n
Synchronized action parameters $AC_PARAM[n]
are used for calculations and as a buffer in the
synchronized actions.
The number of available AC parameter variables per
channel are defined using machine data MD 28254:
MM_NUM_AC_PARAM.
T he parameters are available once per channel
under the same name. The $AC_PARAM flags are
stored in the dynamic memory.
Siemens AG, 2002. All rights reserved
10-410 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.3 Special real-time variables for synchronized actions 10
8 40D 810D 8 40Di
NCU 572
NCU 573 CCU2
10.3.4 Access to R parameters $Rxx
Function
D ata type: REAL
T hese static variables are used for calculations in
the parts program etc. They can be addressed in the
interpolation cycle by appending $.
E xamples:
WHEN $AA_IM[X]>=40.5 DO $R10=$AA_MM[Y] Write access to the R parameter 10.
WHEN $AA_IM[X]>=6.7 DO $R[$AC_MARKER[1]]=30.6 ;Read access to the R parameter whose
number is given in flag 1
N otes
Application:
T he use of R parameters in synchronized actions
permits
• storage of values that you want to retain beyond
the end of program, NC reset, and Power On.
• display of stored value in the R parameter display
• archiving of values determined for synchronized
actions
T he R parameters must be used either as "normal"
arithmetic variables Rxx or as real-time variables $Rxx.
I f you want the R parameter to be used as a
"normal" arithmetic variable again after it has been
used in a synchronized action, make sure that the
preprocessing stop is programmed explicitly with
STOPRE for synchronization of preprocessing and
the main run:
E xample:
WHEN $AA_IM[X]>=40.5 DO $R10=$AA_MM[Y] Use of R10 in synchronized actions
G01 X500 Y70 F1000
STOPRE P reprocessing stop
IF R10>20 Evaluation of the arithmetic variable
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-411
10 Motion-Synchronous Action 11.02 10.3 Special real-time variable for synchronized actions 10
8 40 D 810 D 840Di
NCU 572
NCU 573 CCU2
10.3.5 Machine and setting data read/write (SW 4 and higher)
Function
F rom SW 4 and higher, it is possible to read and
write the machine and setting data (MD, SD) of
synchronized actions.
• Read fixed MD, SD
They are addressed from within the synchronized
action in the same manner as in normal parts
program commands and are preceded by a $
character.
Example:
ID=2 WHENEVER $AA_IM[z]=TOTAL DO POS[Y]=-30
$R1=$AC_FIFO1[0]
;As soon as the sum of all product lengths and intervals between products is greater than
or equal to the length between the placement and the removal position, remove
the product from the conveyor belt at the removal position, read the product
length out of the FIFO.
Siemens AG, 2002. All rights reserved
10-414 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
8 40 D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573 CCU2
10.4 Actions within synchronized actions
10.4.1 Auxiliary functions output
Function
I f the conditions are fulfilled, up to 10 M, H and S
functions can be output per machining block.
Auxiliary function output is activated using the action
codeword "DO".
The auxiliary functions are output immediately in
the interpolation cycle. The output timing defined in
the machine data for auxiliary functions is not active. Example:
The output timing is determined when the condition Switch on coolant at a specific axis position:
WHEN $AA_IM[X]>=15 DO M07
is fulfilled.
POS[X]=20 FA[X]=250
Sequence
Auxiliary functions must only be programmed with
the vocabulary words WHEN or EVERY in non
modal synchronized actions (without model ID).
Whether an auxiliary function is active or not is
determined by the PLC, e.g. via NC start.
Notes
Not possible from a motion synchronized action:
• M0, M1, M2, M17, M30: Program halt/end (M2,
M17, M30 possible for technology cycle)
• M70: Spindle function
• M functions for tool change set with M6 or via
machine data
• M40, M41, M42, M43, M44, M45: Gear change
Programming example
WHEN $AA_IW[Q1]>5 DO M172 H510 I f the actual value of axis Q1 exceeds 5 mm,
auxiliary functions M172 and H510 are output to
the PLC.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-415
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
840 D 8 40 D 810 D 8 40Di
NCU 571 NCU 572
NCU 573 CCU2
10.4.2 Set read-in disable RDISABLE
Function
W ith RDISABLE further block execution is stopped
in the main program if the condition is fulfilled.
Programmed synchronized motion actions are still
executed, the following blocks are still prepared.
A t the beginning of the block with RDISABLE, exact
positioning is always triggered whether RDISABLE is
active or not.
Programming example
Start the program in interpolation cycles dependent
on external inputs.
...
WHENEVER $A_INA[2]50…
Programming example
Rapid axial delete distance-to-go
Stopping a programmed positioning movement:
I D=1 WHEN $A_IN[1]==1 DO MOV[V]=3 FA[V]=700 S tart axis
WHEN $A_IN[2]==1 DO DELDTG(V) Delete distance-to-go, the axis is stopped using MOV=0
D elete distance-to-go depending on the input voltage:
W HEN $A_INA[5]>8000 DO DELDTG(X1)
;As soon as voltage on input 5 exceeds 8V, delete distance-to-go for axis X1.
Path motion continues.
POS[X1]=100 FA[X1]=10 G1 Z100 F1000
Restriction
P repared delete distance-to-go
• cannot be used with active tool radius correction.
• the action must only be programmed in non
modal synchronized actions (without ID number).
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-419
10 Motion-Synchronous Action 11.0210.4 Actions within synchronized actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
10.4.6 Polynomial definition, FCTDEF, block-synchronized
Programming
FCTDEF(Polynomial_No.,LLIMIT,ULIMIT,a0,a1,a2,a3)
Explanation
Polynomial_No. Number of the 3rd degree polynomial
LLIMIT Lower limit for function value
ULIMIT Upper limit for function value
a0,a1,a2,a3 Polynomial coefficient
Function
FCTDEF allows 3rd degree polynomials to be
defined as y=a0+a x+a x
2+a 31 2 3x . These polynomials
are used by the online tool offset FTOC and the
evaluation function SYNFCT to calculate function
values from the main run variables (real-time
variables).
The polynomials are defined either block-
synchronized with the function FCTDEF or via
system variables:
$AC_FCTLL[n] Lower limit for function value
$AC_FCTUL[n] Upper limit for function value
$AC_FCT0[n] a0
$AC_FCT1[n] a1
$AC_FCT2[n] a2
$AC_FCT3[n] a3
n Number of the polynomial
Siemens AG, 2002. All rights reserved
10-420 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action10.4 Actions within synchronized actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Notes
• The system variables can be written from the parts
program or from a synchronized action. When
writing from parts programs, program STOPRE to
ensure that writing is block synchronized.
• SW 4 and higher:
The system variables $AC_FCTLL[n],
$AC_FCTUL[n], $AC_FCT0[n] to $AC_FCTn[n] can
be modified from within synchronized actions
(not SINUMERIK FM-NC,
not SINUMERIK 840D with NCU 571).
W hen writing form synchronized actions, the
polynomial coefficients and function value limits are
active immediately.
P rogramming example
P olynomial for straight section:
W ith upper limit 1000, lower limit -1000, ordinate
section a0=$AA_IM[X] and linear gradient 1 the f (X)
polynomial is:
Upper limit
1000
a X
1
Lower limit
-1000
a0
FCTDEF(1, -1000,1000,$AA_IM[X],1)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-421
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
8 40D 840Di
NCU 572
NCU 573
1 0.4.7 Laser power control
Programming example
Polynomial definition using variables
One of the possible applications of polynomial
definition is the laser output control.
L aser output control means:
Influencing the analog output in dependence on, for $AC_FCTUL 1 [ ] 0.5
example, the path velocity. Block end
$AC_FCTUO 1[ ] 0.35 1
1.5EX-5 $AC_FCT1 1[ 1 ]
Block start
$AC_FCTLL 1 [ ] 0.2
$AC_FCTLL[1]=0.2 Definition of the polynomial coefficient
$AC_FCTUL[1]=0.5
$AC_FCT0[1]=0.35
$AC_FCT1[1]=1.5EX-5
STOPRE
ID=1 DO $AC_FCTUL[1]=$A_INA[2]*0.1 +0.35 Changing the upper limit online.
ID=2 DO SYNFCT(1,$A_OUTA[1],$AC_VACTW)
;In dependence on the path velocity (stored in $AC_VACTW) the
laser output control is controlled via analog output 1
N ote
The polynomial defined above is used with SYNFCT.
Siemens AG, 2002. All rights reserved
10-422 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 8 40Di
NCU 572
NCU 573
10.4.8 Evaluation function SYNFCT
Programming
S YNFCT(Polynomial_No., realtime variable output, real-time variable
input)
Explanation
P olynomial_No. With polynomial defined with FCTDEF
(see Subsection "Polynomial definition").
Real-time variable output Write real-time variable
Real-time variable input R ead real-time variable
Function
SYNFCT reads real-time variables in synchronism
with execution (e.g. analog input, actual value, ...)
and uses them to calculate function values up to the
3rd degree (e.g. override, velocity, axis position, ...)
using an evaluation polynomial (FCTDEF). The
result is output in to real-time variables and
subjected to upper and lower limits with FCTDEF
(see Subsection 10.4.7).
A s real-time variables, variables can be selected and
directly included in the processing operation
• with additive influencing
• with multiplicative influencing
• as position offset
• directly.
Application
The evaluation function is used
• in AC control (Adaptive Control)
• in laser output control
• with position feedforward
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-423
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
840D 840Di
NCU 572
NCU 573
10.4.9 Adaptive control (additive)
Programming example
A dditive influence on the programmed feedrate
F
[ m m / m i n ]
A programmed feedrate is to be controlled by adding
using the current of the X axis (infeed axis): Upper limit
The feedrate should only vary by +/– 100 mm/min 100
and the current fluctuates by +/–1A around the
working point of 5A.
Ι
4 5 6 [A ]
Lower limit
-100
1 . Polynomial definition
D etermination of the coefficients
y = f(x) = a0 + a1x + a2x
2 + a3x
3
a1 = -100mm/1 min A
a 0 = -(-100)*5 =500
a2 = a3 = 0 (not quadratic or cubic element)
Upper limit = 100
Lower limit = -100
T herefore:
FCTDEF(1,-100,100,500,-100,0,0)
2 . Activate AC control
I D=1 DO SYNFCT(1,$AC_VC,$AA_LOAD[x])
;Read the current axis load (% of the max. drive current) via $AA_LOAD[x],
calculate the path feedrate override with the polynomial defined above.
Siemens AG, 2002. All rights reserved
10-424 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 8 40Di
NCU 572
NCU 573
10.4.10 Adaptive control (multiplicative)
P rogramming example
Influence the programmed feedrate by
multiplication
T he aim is to influence the programmed feedrate by
multiplication. The feedrate must not exceed certain
limits – depending on the load on the drive: OVR
[ % ]
• The feedrate is to be stopped at a drive load of
80%: Override = 0. 160
• At a drive load of 30% it is possible to traverse at Upper limit 120
programmed feedrate: Override = 100%. 100
• The feedrate can be exceeded by 20%: Max.
override = 120%.
Lower limit
Load
30 80 [% ]
1 . Polynomial definition
D etermination of the coefficients
y = f(x) = a0 + a1x + a x
2
2 + a x
3
3
a1 = -100%/(80-30)% = -2
a0 = 100 + (2*30) = 160
a2 = a3 = 0 (not quadratic or cubic element)
Upper limit = 120
Lower limit = 0
Therefore:
FCTDEF(2,0,120,160,-2,0,0)
2 . Activate AC control
I D=1 DO SYNFCT(2,$AC_OVR,$AA_LOAD[x])
;Read the current axis load (% of the max. drive current) via $AA_LOAD[x],
calculate the feedrate override with the polynomial defined above.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-425
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
8 40D 810D 8 40Di
NCU 572
NCU 573
10.4.11 Clearance control with limited compensation
P rogramming example
I ntegrating calculation of the distance values with
Z Single-dimension distance control
boundary check
$AA_OFF_MODE = 1 Distance
Important: sensor e.g. Metal sheet
The loop gain of the overlying control loop depends 0.2...0.5mm
on the setting for the interpolation cycle.
X
Remedy: Read MD for interpolation cycle and take it Overlaid velocity
into account.
Upper limit
Note:
Restriction of the velocity of the overlying interpolator 0.6 m/min
-10V 1V
with MD 32020: JOG_VELO
with an interpolation cycle of 12 ms: +10V
Velocity:
0.120mm Lower limit
/mV = m0.6 /V
0.6ms min
S ubroutine: Clearance control ON
%_N_AON_SPF Subroutine for clearance control ON
PROC AON
$AA_OFF_LIMIT[Z]=1 Determine limiting value
FCTDEF(1, -10, +10, 0, 0.6, 0.12) Polynomial definition
ID=1 DO SYNFCT(1,$AA_OFF[Z],$A_INA[3]) Clearance control active
ID=2 WHENEVER $AA_OFF_LIMIT[Z]0 D isable axis X when limit value is overshot
DO $AA_OVR[X] = 0
RET
ENDPROC
S ubroutine: Clearance control OFF
%_N_AOFF_SPF
PROC AOFF Subroutine for clearance control OFF
CANCEL(1) Cancel clearance control synchronized action
CANCEL(2) Cancel off limits check
RET
ENDPROC
Siemens AG, 2002. All rights reserved
10-426 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 810D 840Di
NCU 572
NCU 573
Main program:
%_N_MAIN_MPF
AON Clearance control ON
...
G1 X100 F1000
AOFF Clearance control OFF
M30
Notes
P osition offset in the basic coordinate system
W ith the system variable $AA_OFF[axis] on overlaid
movement of each axis in the channel is possible. It acts as
a position offset in the basic coordinate system.
T he position offset programmed in this way is overlaid
immediately in the axis concerned, whether the axis is being
moved by the program or not.
F rom SW 4 upwards, it is possible to limit the absolute value
to be corrected (real-time variable output) to the variable in
setting data SD 43350: AA_OFF_LIMIT.
T he manner of overlaying the distance is defined in machine
data MD 36750: AA_OFF_MODE:
0 Proportional valuation
1 Integrating valuation
W ith system variable $AA_OFF_LIMIT[axis] a directional
scan to see whether the offset value is within the limits is
possible. These system variables can be scanned from
synchronized actions and, when a limit value is reached, it is
possible to stop the axis or set an alarm.
0 Offset value not within limits
1 Limit of offset value reached in the positive
direction
-1 Limit of the offset value reached in the negative
direction
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-427
10 Motion-Synchronous Action 11.02 1 0.4 Actions within synchronized actions 10
8 40D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
10.4.12 Online tool offset FTOC
Programming
FTOC(Polynomial_No., RV, Length1_2_3 or Radius4,
channel, spindle)
Explanation
P olynomial_No. For polynomial defined with FCTDEF, see Subsection "Polynomial
definition" in this Section.
R V Real-time variable for which a function value for the specified
polynomial is to be calculated.
L ength1_2_3 L ength compensation ($TC_DP1 to 3) or radius compensation to
Radius4 which the calculated function value is added.
C hannel Number of the channel in which the offset is active. No specification
is made here for an offset in the active channel. FTOCON must be
activated in the target channel.
S pindle Only specified if it is not the active spindle which is to be
compensated.
Function
F TOC permits overlaid movement for a geometry axis
after a polynomial programmed with FCTDEF
depending on a reference value that might, for
example, be the actual value of an axis.
T his means that you can also program modal,
Online tool compensations or clearance controls as
synchronized actions.
Application
M achining of a workpiece and dressing of a grinding
wheel in the same channel or in different channels
(machining and dressing channel).
T he supplementary conditions and specifications for
dressing grinding wheels apply to FTOC in the same
way that they apply to tool offsets using PUTFTOCF.
For further information, please refer to Chapter 5
"Tool Offsets".
Siemens AG, 2002. All rights reserved
10-428 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
Programming example
I n this example, we want to compensate for the
length of the active grinding wheel.
Dressing roll
Dressing
amount Grinding wheel
Length to be
compensated
Workpiece
%_N_DRESS_MPF
FCTDEF(1,-1000,1000,-$AA_IW[V],1) Define function
ID=1 DO FTOC(1,$AA_IW[V],3,1) Select online tool compensation:
Actual value of the V axis is the input
value for polynomial 1; the result is added
length 3 of the active grinding wheel in
channel 1 as the offset value.
WAITM(1,1,2) Synchronization with machining channel
G1 V-0.05 F0.01 G91 Infeed movement for dressing
G1 V-0.05 F0.02
...
CANCEL(1) D eselect online offset
. ..
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-429
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
8 40D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
1 0.4.13 Positioning movements
Function
A xes can be positioned completely unsynchonized with
respect to the parts program from synchronized actions.
The programming of positioning axes from
synchronized actions is advisable for cyclic sequences
or operations that are strongly dependent on events.
Axes programmed from synchronized actions are called
command axes.
I n SW 5 and higher, G codes G70/G71/G700/G710 can
be programmed in synchronized actions. They can be
used for defining the measuring system for positioning
tasks in synchronized actions.
R eferences: /PG/ Chapter 3 "Specifying paths”
/FBSY/ "Starting Command Axes"
T he measuring system is defined using G70/G71/
G700/G710.
B y programming the G functions in the synchronized
action, the INCH/METRIC evaluation for the
synchronized action can be defined independently of
the parts program context.
E xample 1 T he program environment affects the
positioning travel of the positioning axis
(no G function in the action part of the
synchronized action)
N100 R1=0
N 110 G0 X0 Z0
N120 WAITP(X)
N130 ID=1 WHENEVER $R==1 DO POS[X]=10
N 140 R1=1
N150 G71 Z10 F10 Z =10mm X=10mm
N160 G70 Z10 F10 Z =254mm X=254mm
N 170 G71 Z10 F10 Z =10mm X=10mm
N180 M30
Siemens AG, 2002. All rights reserved
10-430 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
8 40D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
E xample 2 G 71 in the action part of the
synchronized action clearly determines
the positioning travel of the positioning
axis (metric), whatever the program
environment.
N 100 R1=0
N 110 G0 X0 Z0
N120 WAITP(X)
N130 ID=1 WHENEVER $R==1 DO G71 POS[X]=10
N140 R1=1
N150 G71 Z10 F10 Z =10mm X=10mm
N 160 G70 Z10 F10 Z=254mm X=10mm (X is always
positioned to 10mm)
N170 G71 Z10 F10 Z =10mm X=10mm
N180 M30
Programming example
D isabling a programmed axis motion
I f you do not want the axis motion to start at the
beginning of the block, the override for the axis can
be held at 0 until the appropriate time
from a synchronized action.
W HENEVER $A_IN[1]==0 DO $AA_OVR[W]=0
G01 X10 Y25 F750 POS[W]=1500
FA=1000
;The positioning axis is halted as long as digital input 1 =0
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-431
10 Motion-Synchronous Action 11.02 1 0.4 Actions within synchronized actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
1 0.4.14 Position axis POS
Function
POS[axis]=value
U nlike programming from the parts program, the
positioning axis movement has no effect on
execution of the parts program.
Explanation
Axis: Name of the axis to be traversed
V alue: The value to traverse by (depending on traverse mode)
Programming example
ID=1 EVERY $AA_IM[B]>75 DO POS[U]=100
Axis U is moved incrementally from the control zero by 100 (inch/mm) or to position
100 (inch/mm) independently of the traversing mode.
ID=1 EVERY $AA_IM[B]>75 DO POS[U]=$AA_MW[V]-$AA_IM[W]+13.5
;Axis U moved by a path calculated from real-time variables.
1 0.4.15 Start/stop axis MOV
Programming
MOV [Axis]=value
Explanation
Axis: Name of the axis to be started
Value: Start command for traverse/stop motion.
The sign determines the direction of motion.
The data type for the value is INTEGER.
Value>0 (usually +1): Positive direction
Value 75 DO POS[U]=100 FA[U]=990
;Define fixed feedrate value
ID=1 EVERY $AA_IM[B]>75 DO POS[U]=100 FA[U]=$AA_VACTM[W]+100
;Calculate feedrate value from real-time variables
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-433
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
8 40D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
1 0.4.17 SW limit switch
Function
T he working area limitation programmed with G25/G26
is taken into account for the command axes depending
on the setting data SA_WORKAREA_PLUS_ENABLE.
Switching the working area limitation on and off with
G functions WALIMON/WALIMOF in the parts
program has no effect on the command axes.
1 0.4.18 Axis coordination
Function
Typically, an axis is either moved from the parts
program in the motion block or as a positioning axis
from a synchronized action.
I f the same axis is to be traversed alternately from
the parts program as a path or positioning axis and
from synchronized actions, however, a coordinated
transfer takes place between both axis movements.
If a command axis is subsequently traversed from the
parts program, preprocessing must be reorganized.
This, in turn, causes an interruption in the parts
program processing comparable to a preprocessing
stop.
Siemens AG, 2002. All rights reserved
10-434 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Programming example
Move the X axis from either the parts program or the
synchronized actions:
N 10 G01 X100 Y200 F1000 X axis programmed in the parts program
…
N20 ID=1 WHEN $A_IN[1]==1 DO Starting positioning from the synchronized
POS[X]=150 FA[X]=200 action if a digital input is set
…
C ANCEL(1) D eselect synchronized action
…
N 100 G01 X240 Y200 F1000
;X becomes the path axis; before motion, delay occurs because of axis transfer
if digital input was 1 and X was positioned from the synchronized action.
P rogramming example
Change traverse command for the same axis:
ID=1 EVERY $A_IN[1]>=1 DO POS[V]=100 FA[V]=560
;Start positioning from the synchronized action if a digital input >= 1
ID=2 EVERY $A_IN[2]>=1 DO POS[V]=$AA_IM[V] FA[V]=790
Axis follows, 2nd input is set, i.e. end position and feed
for axis V are continuously followed during a movement
when two synchronized actions are simultaneously active.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-435
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
840D 810D 8 40Di
NCU 572
NCU 573 C CU2
10.4.19 Set actual value
Function
When PRESETON (axis, value) is executed, the
current axis position is not changed but a new value
is assigned to it.
Notes
P RESETON can be executed from within a
synchronized action in the following cases:
• Modulo rotary axes that have been started from
the parts program
• All command axes that have been started from
the synchronized action
R estriction:
PRESETON is not possible for axes that participate
in a transformation.
Programming example
WHEN $AA_IM[a] >= 89.5 DO PRESETON(a4,10.5)
;Offset control zero of axis a by 10.5 length units (inch or mm) in the positive
axis direction.
Restriction
O ne and the same axis can by moved from the parts
program and from a synchronized action, only at
different times. For this reason, delays can occur in the
programming of an axis from the parts program if the
same axis has been program in a synchronized action
first.
I f the same axis is used alternately, transfer between
the two axis movements is coordinated. Parts program
execution must be interrupted for that.
Siemens AG, 2002. All rights reserved
10-436 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
8 40D 8 10D 840Di
NCU 572
NCU 573 CCU2
10.4.20 Spindle motions
Function
Spindles can be positioned completely unsynchronized
with respect to the parts program from synchronized
actions. This type of programming is advisable for
cyclic sequences or operations that are strongly
dependent on events.
Programming example
S tart/stop/position spindles
ID=1 EVERY $A_IN[1]==1 DO M3 S1000 S et direction and speed of rotation
I D=2 EVERY $A_IN[2]==1 DO SPOS=270 P osition spindle
Sequence of execution
If conflicting commands are issued for a spindle via
simultaneously active synchronized actions, the
most recent spindle command takes priority.
Programming example
Set direction and speed of rotation/position spindle
ID=1 EVERY $A_IN[1]==1 DO M3 S300 S et direction and speed of rotation
ID=2 EVERY $A_IN[2]==1 DO M4 S500 Specify new direction and new speed of
rotation
I D=3 EVERY $A_IN[3]==1 DO S1000 S pecify new speed
ID=4 EVERY ($A_IN[4]==1) AND Position spindle
($A_IN[1]==0) DO SPOS=0
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-437
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
840D 8 10D 8 40Di
NCU 572
NCU 573 C CU2
10.4.21 Coupled-axis motion TRAILON, TRAILOF
Function
DO TRAILON(following axis, leading axis, A ctivate coupled-axis motion
coupling factor)
D O TRAILOF(following axis, leading axis, Deactivate coupled-axis
leading axis 2) motion
When the coupling is activated from the
synchronized action, the leading axis can be in
motion. In this case the following axis is accelerated
up to the set velocity. The position of the leading axis
at the time of synchronization of the velocity is the
starting position for coupled-axis motion. The
functionality of coupled-axis motion is described in
the Section "Path traversing behavior".
A ctivate asynchronized coupled motion:
... DO TRAILON(FA, LA, CF) Where: FA: Following axis
LA: Leading axis
CF: Coupling factor
D eactivate asynchronized coupled motion:
... DO TRAILOF(FA, LA, LA2) Where: FA: Following axis
LA: Leading axis
LA2: Leading axis 2, optional
Programming example
$A_IN[1]==0 DO TRAILON(Y,V,1) A ctivate 1st combined axis pair when digital input is 1
$A_IN[2]==0 DO TRAILON(Z,W,-1) Activate 2nd combined axis pair
G0 Z10 I nfeed of Z and W axes in opposite axis directions
G0 Y20 Infeed of Y and V axes in same axis directions
...
G1 Y22 V25 Superimpose dependent and independent movement of
coupled-motion axis "V"
...
TRAILOF(Y,V) D eactivate 1st coupled axis
TRAILOF(Z,W) Deactivate 2nd coupled axis
Siemens AG, 2002. All rights reserved
10-438 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
8 40D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
10.4.22 Leading value coupling LEADON, LEADOF
Function
The axial leading value coupling can be
programmed in synchronized actions without
restriction.
Activate axial leading value coupling:
...DO LEADON(FA,LA,NR) Where: FA: Following axis
LA: Leading axis
NR: Number of stored
curve table
D eactivate axial leading value coupling:
...DO LEADOF(FA,LA) W here: FA: Following axis
LA: Leading axis
T he axis to be coupled is released for synchronized
action access by invoking the RELEASE function for the
axis.
Example:
RELEASE (XKAN)
ID=1 every SR1==1 to LEADON(CACH,XKAN,1)
Programming example
On-the-fly parting
A continuous material that runs continuously through the work area of parting device is to be
separated into pieces of equal length.
X axis: Axis in which the continuous material runs. WCS
X1 axis: Machine axis of the continuous material, MCS
Y axis: Axis in which the parting device "travels" with the continuous material
It is assumed that the positioning and control of the parting tool is controlled by the PLC. The
signals of the PLC interface can be evaluated for the purpose of determining the degree of
synchronism between the continuous material and the parting tool.
Actions Activate coupling, LEADON
Deactivate coupling, LEADOF
Set actual value, PRESETON
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-439
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
8 40D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
% _N_SHEARS1_MPF
;$PATH=/_N_WCS_DIR/_N_DEMOFBE_WPD
N 100 R3=1500 ; Length of a section to be parted
N200 R2=100000 R13=R2/300
N300 R4=100000
N 400 R6=30 ; Start position Y axis
N500 R1=1 ; Start condition for conveyor axis
N600 LEADOF(Y,X) ; Delete any existing coupling
N700 CTABDEF(Y,X,1,0) ; Table definition
N 800 X=30 Y=30 ; Value pair
N 900 X=R13 Y=R13
N1000 X=2*R13 Y=30
N1100 CTABEND ; End of table definition
N1200 PRESETON(X1,0) ; PRESET to begin
N1300 Y=R6 G0 ; Start pos. Y axis, axis is linear
N1400 ID=1 WHENEVER $AA_IW[X]>$R3 DO PESETON(X1,0)
;PRESET after length R3, new start following parting
N 1500 RELEASE(Y)
N1800 ID=6 EVERY $AA_IM[X]$R3-30 DO EADOF(Y,X)
;> 30 before traversed parting distance,
deactivate coupling
N2000 WAITP(X)
N2100 ID=7 WHEN $R1==1 DO MOV[X]=1 ;Place material axis in continuous motion
FA[X]=$R4
N2200 M30
Siemens AG, 2002. All rights reserved
10-440 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.4 Actions within synchronized actions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
10.4.23 Measurement
C ompared with use in traverse blocks of the parts
program, the measuring function can be activated
and deactivated as required.
• Axial measurement without deletion of distance-
to-go:
MEAWA[axis]=(mode, trigger event_1, ..._4
• Continuous measurement without deletion of
distance-to-go:
MEAC[axis]=(mode, measurement memory, trigger event_1, ..._4
For further information on measuring: See Chapter 5, "Extended Measuring Function"
10.4.24 Set/clear wait marks: SETM, CLEARM (SW 5.2 and higher)
Function
SETM(MarkerNumber) Set wait marker for channel
CLEARM(MarkerNumber) C lear wait marker for channel
In synchronized actions, wait markers can be set or
deleted for the purpose of coordinating channels, for
example.
S ETM
T he SETM command can be written in the parts
program and in the action part of a synchronized
action. It sets the marker MarkerNumber for the
channel in which the command executes.
C LEARM
T he CLEARM command can be written in the parts
program and in the action part of a synchronized
action. It resets the flag MarkerNumber for the
channel in which the command executes.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-441
10 Motion-Synchronous Action 11.02 1 0.4 Actions within synchronized actions 10
8 40D 8 40D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
10.4.25 Error responses
Function
Incorrect responses can be programmed with
synchronized actions by scanning status variables
and triggering the appropriate actions.
S ome possible responses to error conditions are:
• Stop axis: Override=0
• Set alarm: With SETAL it is possible to set cyclic
alarms from synchronized actions.
• Set output
• All actions possible in synchronized actions
Programming example
ID=67 WHENEVER ($AA_IM[X1]-$AA_IM[X2]) 17 DO FXS[X]=1 ;If X reaches a position greater than 17mm
N30 G1 F200 X100 Y110 ;FXS is activated
S tatic and block-related synchronized actions:
The same commands FXS, FXST and FXSW can be
used in static and block-related synchronized actions as
in normal parts program execution. The values that are
assigned can be generated by calculation.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-443
10 Motion-Synchronous Action 11.02 10.4 Actions within synchronized actions 10
840D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
Programming example
T ravel to fixed stop (FXS)
T riggered by a synchronized action
Y axis: ; Activate static synchronized actions:
N10 IDS=1 WHENEVER (($R1==1) AND ; By setting $R1=1, FXS is activated for
($AA_FXS[y]==0)) DO ; axis Y, the effective torque is reduced to
$R1=0 FXS[Y]=1 FXST[Y]=10 ; 10% and a traverse motion is initiated
FA[Y]=200 POS[Y]=150 ; in the direction of the fixed stop.
N 11 IDS=2 WHENEVER ($AA_FXS[Y]==4) DO ; As soon as the fixed stop is detected
FXST[Y]=30 ; ($AA_FXS[Y]==4), torque is increased
; to 30%
N12 IDS=3 WHENEVER ($AA_FXS[Y]==1) DO ; After the fixed stop is reached, torque
FXST[Y]=$R0 ; is controlled by R0
N13 IDS=4 WHENEVER (($R3==1) AND ; Deselection according to
($AA_FXS[Y]==1)) DO ; R3 and
FXS[Y]=0 ; return
FA[Y]=1000 POS[Y]=0
N20 FXS[Y]=0 G0 G90 X0 Y0 ; Normal program run: axis Y for
N30 RELEASE(Y) ; Enable motion in synchronized action
N 40 G1 F1000 X100 ; Movement of another axis
N 50 ...... ;
N60 GET(Y) ; Put axis Y back in the path group
Programming example
A ctivate torque/force limitation (FOC)
N10 FOCON[X] ; Modal activation of limitation
N 20 X100 Y200 FXST[X]=15 ; X travels with reduced torque (15%)
N30 FXST[X]=75 X20 ; Change the torque to 75%, X travels with
; this limited torque
N 40 FOCOF[X] ; Deactivation of the torque limitation
Siemens AG, 2002. All rights reserved
10-444 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.5 Technology cycles 10
840D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
10.5 Technology cycles
Function
A s an action in synchronized actions, you can invoke
programs. These must consist only of functions that
are permissible as actions in synchronized actions.
Programs structured in this way are called
technology cycles.
T echnology cycles are stored in the control as
subroutines. As far as the user is concerned, they
are called up like subroutines. Parameter transfer is
not possible.
I t is possible to process several technology cycles or
actions in parallel in one channel.
T he program end is programmed with
M02/M17/M30/RET. A maximum of one axis
movement per block can be programmed.
Application
T echnology cycles as axis programs: Each
technology cycle controls only one axis. In this way,
different axis motions can be started in the same
interpolation cycle under event control. The parts
program is now only used for the management
o f synchronized actions in extreme cases.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-445
10 Motion-Synchronous Action 11.02 10.5 Technology cycles 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
A xis programs are started by setting digital inputs. ID = 1 ID = 2 ID = 3 ID = 4
IPO cycle BCeodnideintiuonng BCeodniednituionng BCedoinedniutionng BCedoinedniutinogn
IPO cycle $AA_OVR [Y] = 0 POS [Y] = 10 $AA_OVR [Y] = 0 $AA_OVR [X] = 0
IPO cycle M100 POS [Z] = 90
IPO cycle POS [X] = 100 POS [Y] = 10
IPO cycle POS [Z] = -90
IPO cycle M17 M17
M17
M ain program:
I D=1 EVERY $A_IN[1]==1 DO AXIS_X I f input 1 is at 1, axis program X starts
ID=2 EVERY $A_IN[2]==1 DO AXIS_Y I f input 2 is at 1, axis program Y starts
I D=3 EVERY $A_IN[3]==1 DO $AA_OVR[Y]=0 I f input 3 is at 1, the override for axis Y is at 0
I D=4 EVERY $A_IN[4]==1 DO AXIS_Z I f input 4 is at 1, axis program Z starts
M30
T echnology cycle AXIS_X:
$AA_OVR[Y]=0
M 100
POS[X]=100 FA[X]=300
M 17
T echnology cycle AXIS_Y:
P OS[Y]=10 FA[Y]=200
POS[Y]=-10
M17
T echnology cycle AXIS_Z:
$AA_OVR[X]=0
POS[Z]=90 FA[Z]=250
POS[Z]=-90
M17
Siemens AG, 2002. All rights reserved
10-446 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.5 Technology cycles 10
840D 840D 8 10D 8 40Di
NCU 571 NCU 572
NCU 573
T echnology cycles are started as soon as their
conditions are fulfilled. With positioning axes, several
IPO cycles are required for execution. Other
functions (OVR) are executed in one cycle.
I n the technology cycle, blocks are executed in
sequence.
Notes
If actions are called in the same interpolation cycle
that are mutually exclusive, the action is started that
is called from the synchronized action with the higher
ID number.
1 0.5.1 Lock, unlock, reset: LOCK, UNLOCK, RESET
Programming
L OCK (n, n, ...) Lock technology cycle, the active action is interrupted
UNLOCK (n, n, ...) U nlock technology cycle
R ESET (n, n, ...) Reset technology cycle, the active action is interrupted
n Identification number of the synchronized action
Function
E xecution of a technology cycle can be locked,
unlocked or reset from within a synchronized action
or from a technology cycle.
Lock technology cycle, LOCK
T echnology cycles can be locked using LOCK from
another synchronized action or from a technology cycle.
E xample:
N100 ID=1 WHENEVER $A_IN[1]==1 DO M130
...
N200 ID=2 WHENEVER $A_IN[2]==1 DO LOCK(1)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-447
10 Motion-Synchronous Action 11.02 10.5 Technology cycles 10
840D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Unlock technology cycle, UNLOCK
L ocked technology cycles can be unlocked again from
another synchronized action/technology cycle with UNLOCK.
With UNLOCK, this is continued at the current position, this
also applies to an interrupted positioning procedure.
E xample:
N100 ID=1 WHENEVER $A_IN[1]==1 DO M130
...
N200 ID=2 WHENEVER $A_IN[2]==1 DO LOCK(1)
...
N250 ID=3 WHENEVER $A_IN[3]==1 DO UNLOCK(1)
Reset technology cycle, RESET
T echnology cycles can be reset using RESET from
another synchronized action or from a technology cycle.
Example:
N100 ID=1 WHENEVER $A_IN[1]==1 DO M130
...
N200 ID=2 WHENEVER $A_IN[2]==1 DO RESET(1)
Locking on the PLC side
M odal synchronized actions can be interlocked from the
PLC with the ID numbers n=1 ... 64. The associated
condition is no longer evaluated and execution of the
associated function is locked in the NCK.
All synchronized actions can be locked indiscriminately
with one signal in the PLC interface.
Notes
A programmed synchronized action is active as Application:
standard and can be protected against It should not be possible for end
overwriting/locking by a machine data setting. customers to modify synchronized
actions defined by the machine
manufacturer.
Siemens AG, 2002. All rights reserved
10-448 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.6 Cancel synchronized action: CANCEL 10
840D 8 40D 810D 840Di
NCU 571 NCU 572
NCU 573
10.6 Cancel synchronized action: CANCEL
Programming
CANCEL(n,n,...) Cancel synchronized action
n I dentification number of the synchronized
action
Explanation
M odal synchronized actions with the identifier
ID(S)=n can only be canceled directly from the parts
program with CANCEL.
Example:
N100 ID=2 WHENEVER $A_IN[1]==1 DO M130
...
N200 CANCEL(2) Cancel synchronized action No. 2
Notes
I ncomplete movements originating from a canceled
synchronized action are completed as programmed.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-449
10 Motion-Synchronous Action 11.02 1 0.7 Supplementary conditions 10
8 40D 840D 810D 8 40Di
NCU 571 NCU 572
NCU 573
1 0.7 Supplementary conditions
• Power ON
With power ON no synchronized actions are
active.
However, static synchronized actions can be
activated on power ON with an asynchronized
subroutine (ASUB) started by the PLC.
• Mode change
Synchronized actions activated with the
vocabulary word IDS remain active following a
changeover in operating mode.
All other synchronized actions become inactive
following operating mode changeover (e.g. axis
positioning) and become active again following
repositioning and a return to automatic mode.
• Reset
With NC reset, all actions started by
synchronized actions are stopped. Static
synchronized actions remain active. They can
start new actions.
The RESET command can be used from the
synchronized action or from a technology cycle
to reset a modally active synchronized action. If
a synchronized action is reset while the
positioning axis movement that was activated
from it is still active, the positioning axis
movement is interrupted.
Synchronized actions of the WHEN type that
have already been executed are not executed
again following RESET.
Siemens AG, 2002. All rights reserved
10-450 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.7 Supplementary conditions 10
8 40D 840D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Response following RESET
Synchronized action / Modal / non-modal Static (IDS)
technology cycle
Active actions are reset, synchronized Active action is canceled,
actions are canceled technology cycle is reset
Axis / positioning spindle Movement is reset Movement is reset
Speed-controlled spindle $MA_SPIND_ACTIVE_AFTER_RESET==1: $MA_SPIND_ACTIVE_AFTER_RES
Spindle remains active ET==1: Spindle remains active
$MA_SPIND_ACTIVE_AFTER_RESET==0: $MA_SPIND_ACTIVE_AFTER_RES
Spindle is stopped. ET==0: Spindle is stopped.
Leading value coupling $MC_RESET_MODE_MASK, Bit13 == 1: $ MC_RESET_MODE_MASK,
Leading value coupling remains active Bit13 == 1: Leading value coupling
remains active
$MC_RESET_MODE_MASK, Bit13 == 0: $MC_RESET_MODE_MASK,
Leading value coupling is disconnected Bit13 == 0: Leading value coupling
is disconnected
Measuring procedures Measurements started from synchronized M easurements started from static
actions are canceled. synchronized actions are canceled.
• NC Stop
Static synchronized actions remain active on NC
stop. Movements started from static synchronized
actions are not canceled.
Synchronized actions that are local to the
program and belong to the active block remain
active, movements started from them are stopped.
• End of program
End of program and synchronized action do not
influence one another.
Current synchronized actions are completed
even after end of program.
Synchronized actions active in the M30 block
remain active. If you do not want them to remain
active, cancel the synchronized action before
end of program by pressing CANCEL (see
preceding section).
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-451
10 Motion-Synchronous Action 11.02 10.7 Supplementary conditions 10
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
R esponse following end of program
Synchronized action / Modal and non-modal Static (IDS)
technology cycle are reset remain active
Axis / positioning spindle M30 is delayed until the axis/spindle is M ovement continues
stationary.
Speed-controlled spindle E nd of program: S pindle remains active
$MA_SPIND_ACTIVE_AFTER_RESET==1:
Spindle remains active
$MA_SPIND_ACTIVE_AFTER_RESET==0:
Spindle is stopped
Spindle remains active following a change in
operating mode
Leading value coupling $MC_RESET_MODE_MASK, Bit13 == 1: A coupling started from a static
Leading value coupling remains active synchronized action remains
$MC_RESET_MODE_MASK, Bit13 == 0:
Leading value coupling is disconnected
Measuring procedures M easurements started from synchronized M easurements started from
actions are canceled. static synchronized actions
remain active.
• Block search
Synchronized actions found during a block search
are collected and evaluated on NC Start; the
associated actions are then started if necessary.
Static synchronized actions are active during block
search.
If polynomial coefficients programmed with
FCTDEF are found during a block search, they are
written directly to the setting data.
• Program interruption by asynchronized
subroutine
ASUB start:
Modal and static motion-synchronized actions
remain active and are also active in the
asynchronized subroutine.
A SUB end:
If the asynchronized subroutine is not resumed
with Repos, modal and static motion-
synchronized actions that were modified in the
asynchronized subroutine remain active in the
main program.
Siemens AG, 2002. All rights reserved
10-452 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
10 11.02 Motion-Synchronous Action 10.7 Supplementary conditions 10
840D 8 40D 810D 8 40Di
NCU 571 NCU 572
NCU 573
• Repositioning
On repositioning REPOS, the synchronized
actions that were active in the interrupted block
are reactivated.
Modal synchronized actions changed from the
asynchronized subroutine are not active after
REPOS when the rest of the block is executed.
Polynomial coefficients programmed with
FCTDEF are not affected by asynchronized
subroutines and REPOS. No matter where they
were programmed, they can be used at any time
in the asynchronized subroutine and in the main
program after execution of REPOS.
• Deselection with CANCEL
If an active synchronized action is deselected
with CANCEL, this does not affect the active
action. Positioning movements are terminated in
accordance with programming.
The CANCEL command is used to interrupt a
modally or statically active synchronized action.
If a synchronized action is canceled while the
positioning axis movement that was activated
from it is still active, the positioning axis
movement is interrupted. If this is not required,
the axis movement can be decelerated before the
CANCEL command with axial deletion of
distance-to-go:
Example:
ID=17 EVERY $A_IN[3]==1 DO POS[X]=15 FA[X]=1500 ;Start positioning axis movement
...
WHEN ... DO DELDTG(X) ;End positioning axis movement
CANCEL(1)
▀
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 10-453
10 Motion-Synchronous Action 11.02 1 0.7 Supplementary conditions 10
840D 8 40D 8 10D 840Di
NCU 571 NCU 572
NCU 573
Siemens AG, 2002. All rights reserved
10-454 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation 11
Oscillation
11.1 Asynchronous oscillation............................................................................................. 11-456
11.2 Oscillation controlled via synchronous actions............................................................ 11-463
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-455
11 Oscillation 11.0211.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
11.1 Asynchronous oscillation
Explanation of the commands
OSP1[axis]= Position of reversal point 1
OSP2[axis]= Position of reversal point 2
OST1[axis]= Stopping time at reversal points in seconds
OST2[axis]=
FA[axis]= Feed for oscillating axis
OSCTRL[axis]= (Set, reset options)
OSNSC[axis]= Number of spark-out strokes
OSE[axis]= End position
OS[axis]= 1 = activate oscillation; 0 = deactivate oscillation
Function
An oscillating axis travels back and forth between
two reversal points 1 and 2 at a defined feedrate,
until the oscillating motion is deactivated.
Other axes can be interpolated as desired during the
oscillating motion.
A path movement or a positioning axis can be used
to achieve a constant infeed, however, there is no
relationship between the oscillating movement and
the infeed movement.
Siemens AG, 2002. All rights reserved
11-456 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
The oscillating axis
For the oscillating axis, the following applies:
• Any axis can be used as an oscillating axis.
• Several oscillating axes can be active
simultaneously (maximum: number of positioning
axes).
• Linear interpolation G1is always active for the
oscillating axis – irrespective of the G command
currently valid in the program.
The oscillating axis can
• act as an input axis for a dynamic transformation
• act as a guide axis for gantry and combined-
motion axes
• be traversed
– without jerk limitation (BRISK) or
– with jerk limitation (SOFT) or
– with acceleration curve with a knee
(as for positioning axes).
O scillation reversal points
The current offsets must be taken into account when
oscillation positions are defined:
• Absolute specification
OSP1[Z]=value
Position of reversal point = sum of offsets +
programmed value
• Relative specification
OSP1[Z]=IC(value)
Position of reversal point = reversal point 1 +
programmed value
E xample:
N 10 OSP1[Z]=100 OSP2[Z]=110
.
.
N40 OSP1[Z]=IC(3)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-457
11 Oscillation 11.0211.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Properties of asynchronized oscillation
• Asynchronized oscillation is active beyond block
limits on an axis-specific basis.
• Block-oriented activation of the oscillation
movement is ensured by the parts program.
• Combined interpolation of several axes and
superimposing of oscillation paths are not
possible.
Setting data
The setting data necessary for asynchronized oscillation
can be set in the parts program.
If the setting data are described directly in the
program, the change takes effect during
preprocessing. A synchronized response can be
achieved by means of a STOPRE.
E xample:
Oscillation with online change
of reversal position
$SA_OSCILL_REVERSE_POS1[Z]=-10
$ SA_OSCILL_REVERSE_POS2[Z]=10
G0 X0 Z0
W AITP(Z)
I D=1 WHENEVER $AA_IM[Z] < $$AA_OSCILL_REVERSE_POS1[Z] DO $AA_OVR[X]=0
I D=2 WHENEVER $AA_IM[Z] < $$AA_OSCILL_REVERSE_POS2[Z] DO $AA_OVR[X]=0
;If the actual value of the oscillation axis
; has exceeded the reversal point,
; the infeed axis is stopped.
OS[Z]=1 FA[X]=1000 POS[X]=40 ;Switch on oscillation
O S[Z]=0 ; Switch off oscillation
M30
Siemens AG, 2002. All rights reserved
11-458 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Notes on individual functions
T he following addresses allow asynchronized
oscillation to be activated and controlled from the
parts program.
T he programmed values are entered in the
corresponding setting data with block
synchronization during the main run and remain
active until changed again.
Activate, deactivate oscillation: OS
O S[axis] = 1: Activate
O S[axis] = 0: Deactivate
W AITP (axis):
• If oscillation is to be performed with a geometry
axis, you must enable this axis for oscillation with
WAITP.
• When oscillation has finished, this command is
used to enter the oscillating axis as a positioning
axis again for normal use.
Stopping times at reversal points:
OST1, OST2
Hold time Movement in exact stop area at reversal point
-2 Interpolation is continued without waiting for exact stop
-1 Wait for exact stop coarse
0 Wait for exact stop fine
>0 Wait for exact stop fine and then wait for stopping time
The unit for the stopping time is identical to the
stopping time programmed with G4.
Note
Oscillation with motion-synchronous action and
stopping times "OST1/OST2”.
When the stopping times have elapsed, the internal
block change takes place during oscillation (visible at
the new residual paths of the axes). When block
change has been completed, the deactivation function
is checked. During checking, the deactivation function
is defined according to the control setting for the
"OSCTRL" sequence of motions.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-459
11 Oscillation 11.0211.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
This timing is affected by the feedrate override.
Under certain circumstances, an oscillating stroke is
performed before the spark out strokes are started
or the end position approached.
The impression created is that the deactivation
response changes. However, this is not the case.
Setting feed FA
The feedrate is the defined feedrate of the
positioning axis.
If no feedrate is defined, the value stored in the
machine data applies.
Defining the sequence of motions: OSCTRL
The control settings for the movement are set with
enable and reset options.
Reset options
These options are deactivated (only if they have
previously been activated as setting options).
Set options
These options are switched over. When OSE (end
position) is programmed, option 4 is implicitly
activated.
Siemens AG, 2002. All rights reserved
11-460 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Option value Meaning
0 When the oscillation is deactivated, stop at the next reversal point (default)
only possible by resetting values 1 and 2
1 When the oscillation is deactivated, stop at reversal point 1
2 When the oscillation is deactivated, stop at reversal point 2
3 When the oscillation is deactivated, do not approach reversal point if no
spark-out strokes are programmed
4 Approach end position after spark-out
8 If the oscillation movement is canceled by deletion of the distance-to-go:
then execute spark-out strokes and approach end position if appropriate
16 If the oscillation movement is canceled by deletion of the distance-to-go:
reversal position is approached as with deactivation
32 New feed is only active after the next reversal point
64 FA = 0: Path overlay is active
FA 0: Speed overlay is active
128 For rotary axis DC (shortest path)
256 0=The sparking out stroke is a dual stroke.(default) 1=single stroke.
Several options are appended with plus characters.
Example:
OSCTRL[Z] = (1+4,16+32+64)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-461
11 Oscillation 11.0211.1 Asynchronous oscillation 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
Oscillating axis Z is to oscillate between 10 and 100.
Approach reversal point 1 with exact stop fine,
reversal point 2 with exact stop coarse. Machining
takes place with feedrate 250 for the oscillating axis.
At the end of the machining operation, 3 spark-out
strokes must be executed and end position 200
approached with the oscillating axis.
The feed for the infeed axis is 1, the end of the
infeed in the X direction is at 15.
WAITP(X,Y,Z) Starting position
G0 X100 Y100 Z100 Switch over in positioning axis operation
N40 WAITP(X,Z)
N50 OSP1[Z]=10 OSP2[Z]=100 -> Reversal point 1, reversal point 2
-> OSE[Z]=200 -> End position
-> OST1[Z]=0 OST2[Z]=–1 -> Stopping time at U1: exact stop fine
Stopping time at U2: exact stop coarse
-> FA[Z]=250 FA[X]=1 ->
Feed for oscillating axis, infeed axis
-> OSCTRL[Z]=(4,0) -> Setting options
-> OSNSC[Z]=3 -> Three spark-out strokes
N60 OS[Z]=1 Start oscillation
N70 WHEN $A_IN[3]==TRUE -> Deletion of distance-to-go
-> DO DELDTG(X)
N80 POS[X]=15 Starting position X axis
N90 POS[X]=50
N100 OS[Z]=0 Stop oscillation
M30
-> can be programmed in a single block.
Siemens AG, 2002. All rights reserved
11-462 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
11.2 Oscillation controlled via synchronous actions
Programming:
1. Define parameters for oscillation
2. Define motion-synchronous actions
3. Assign axes, define infeed
Parameters for oscillation
OSP1[oscillating axis]= Position of reversal point 1
OSP2[oscillating axis]= Position of reversal point 2
OST1[oscillating axis]= Stopping time at reversal point 1 in seconds
OST2[oscillating axis]= Stopping time at reversal point 2 in seconds
FA[OscillationAxis]= Feed for oscillating axis
OSCTRL[OscillationAxis]= Set or reset options
OSNSC[oscillating axis]= Number of spark-out strokes
OSE[OscillationAxis]= End position
WAITP(OscillationAxis) Enable axis for oscillation
Axis assignment, infeed
OSCILL[OscillationAxis] = (InfeedAxis1, InfeedAxis2, InfeedAxis3)
POSP[InfeedAxis] = (Endpos, Partial length, Mode)
OSCILL Assign infeed axis or axes for oscillating axis
POSP Define complete and partial infeeds (see Chapter 3)
Endpos End position for the infeed axis after all partial infeeds have
been traversed.
Partial length Length of the partial infeed at reversal point/reversal area
Mode Division of the complete infeed into partial infeeds
0 = Two residual steps of equal size (default);
1 = All partial infeeds of equal size
Motion-synchronized actions
WHEN… … DO when ... , do ...
WHENEVER … DO whenever ... , do ...
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-463
11 Oscillation 11.0211.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Control oscillation via synchronized actions
With this mode of oscillation, an infeed motion may
only be executed at the reversal points or within
defined reversal areas.
Depending on requirements, the oscillation
movement can be
• continued or
• stopped until the infeed has been finished
executing.
Sequence
1. Define oscillation parameters
The parameters for oscillation should be defined
before the movement block containing the
assignment of infeed and oscillating axes and the
infeed definition (see "Asynchronized oscillation").
2. Define motion-synchronized actions
The following synchronization conditions can be
defined:
• Suppress infeed until the oscillating axis is
within a reversal area (ii1, ii2) or at a reversal
point (U1, U2).
• Stop oscillation motion during infeed at
reversal point.
• Restart oscillation movement on completion of
partial infeed.
• Define start of next partial infeed.
3. Assign oscillating and infeed axes as well as
partial and complete infeed.
Siemens AG, 2002. All rights reserved
11-464 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Assignment of oscillating and infeed axes
OSCILL
OSCILL[oscillating axis] = (infeed axis1, infeed axis2, infeed axis3)
The axis assignments and the start of the oscillation
movement are defined with the OSCILL command.
Up to 3 infeed axes can be assigned to an oscillating
axis.
Before oscillation starts, the synchronization
conditions must be defined for the behavior of the
axes.
Define infeeds: POSP
POSP[InfeedAxis] = (EndPosition, Part, Mode)
The following are declared to the control with the POSP
command:
• Complete infeed (with reference to end position)
• The length of the partial infeed at the reversal
point or in the reversal area
• The partial infeed response when the end
position is reached (with reference to mode)
Mode = 0 The distance-to-go to the destination point for the last two partial infeeds
is divided into 2 equal steps (default setting).
Mode = 1 All partial infeeds are of equal size. They are calculated from the
complete infeed.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-465
11 Oscillation 11.0211.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
The synchronized actions
The synchronized motion actions listed below are
used for general oscillation.
You are given example solutions for individual tasks
which you can use as modules for creating user-
specific oscillation movements.
In individual cases, the synchronization conditions
can be programmed differentially.
Vocabulary words
WHEN … DO … when ... , do ...
WHENEVER … DO whenever ... , do ...
You can implement the following functions with the
language resources described in detail below:
1. Infeed at reversal point
2. Infeed at reversal area.
3. Infeed at both reversal points.
4. Stop oscillation movement at reversal point.
5. Restart oscillation movement
6. Do not start partial infeed too early.
The following assumptions are made for all
examples of synchronized actions presented here:
• Reversal point 1 < reversal point 2
• Z = oscillating axis
• X = infeed axis
You will find more information on synchronized
motion actions in Section 11.3.
Siemens AG, 2002. All rights reserved
11-466 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Infeed in reversal area
The infeed motion must start within a reversal area
before the reversal point is reached.
These synchronized actions inhibit the infeed
movement until the oscillating axis is within the
reversal area.
The following instructions are used subject to the
above assumptions:
Reversal area 1:
WHENEVER $AA_IM[Z]>$SA_OSCILL_REVERSE_POS1[Z]+ii1 DO $AA_OVR[X]=0
Whenever the current position of oscillating axis in the MCS is
greater than the start of reversal area 1
then set the axial override of the infeed axis to 0%.
Reversal area 2:
WHENEVER $AA_IM[Z]
-> $AA_OVR[Z]=100
Whenever the current position of oscillating axis Z in the MCS is
greater or less than the position of reversal point 1
then set the axial override of infeed axis X to 0%
and set the axial override of oscillating axis Z to 100%.
Reversal point 2:
For reversal point 2:
WHENEVER $AA_IM[Z]$SA_OSCILL_REVERSE_POS2[Z] DO $AA_OVR[X]=0 ->
-> $AA_OVR[Z]=100
Whenever the current position of oscillating axis Z in the MCS is
greater or less than the position of reversal point 2
then set the axial override of infeed axis X to 0%
and set the axial override of oscillating axis Z to 100%.
Siemens AG, 2002. All rights reserved
11-468 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Stop oscillation motion at reversal point
The oscillation axis is stopped at the reversal point,
the infeed motionstarts at the same time.
The oscillating motion is continued when the infeed
movement is complete.
This synchronized action can also be used to start
the infeed movement if this has been stopped by a
previous synchronized action which is still active.
The following instructions are used subject to the
above assumptions:
Reversal point 1:
WHENEVER $SA_IM[Z]==$SA_OSCILL_REVERSE_POS1[Z]DO $AA_OVR[Z]=0 ->
-> $AA_OVR[X] = 100
Whenever the current position of oscillating axis in the MCS is
equal to the position of reversal point 1
then set the axial override of the oscillating axis to 0%
and set the axial override of the infeed axis to 100%.
Reversal point 2:
WHENEVER $SA_IM[Z] ==$SA_OSCILL_REVERSE_POS2[Z]DO $AA_OVR[Z]= 0 ->
-> $AA_OVR[X]=100
Whenever the current position of oscillating axis in the MCS is
equal to the position of reversal point 2
then set the axial override of the oscillating axis to 0%
and set the axial override of the infeed axis to 100%.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-469
11 Oscillation 11.0211.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Online evaluation of reversal point
If there is a main run variable coded with $$ on the
right of the comparison, then the two variables are
evaluated and compared with one another
continuously in the IPO cycle.
Please refer to Section "Motion-synchronized
actions" for more information.
Restart oscillation movement
This synchronized action is used to continue the
oscillating movement when the partial infeed
movement is complete.
The following instructions are used subject to the
above assumptions:
WHENEVER $AA_DTEPW[X]==0 DO $AA_OVR[Z]= 100
Whenever the distance-to-go for the partial infeed on infeed axis X in the WCS is
equal to zero
then set the axial override of the oscillating axis to 100%.
Siemens AG, 2002. All rights reserved
11-470 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Next partial infeed
When infeed is complete, a premature start of the
next partial infeed must be inhibited.
A channel-specific marker ($AC_MARKER[Index])
is used for this purpose. It is enabled at the end of
the partial infeed (partial distance-to-go ≡ 0) and
deleted when the axis leaves the reversal area. A
synchronized action is then used to inhibit the next
infeed movement.
On the basis of the given assumptions, the following
instructions apply for reversal point 1:
1. Set marker
WHENEVER $AA_DTEPW[X] == 0 DO $AC_MARKER[1]=1
Whenever the distance-to-go for the partial infeed on infeed axis X in the WCS is
equal to zero
then set the marker with index 1 to 1.
2. Clear marker
WHENEVER $AA_IM[Z]$SA_OSCILL_REVERSE_POS1[Z] D0 $AC_MARKER[1]=0
Whenever the current position of oscillating axis Z in the MCS is
greater or less than the position of reversal point 1
then set marker 1 to 0.
3. Inhibit infeed
WHENEVER $AC_MARKER[1]==1 DO $AA_OVR[X]=0
Whenever marker 1 is
equal to 1,
then set the axial override of the infeed axis to 0%.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-471
11 Oscillation 11.0211.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
No infeed is to take place at reversal point 1. At 0 10 20 30 40 50 60 70
reversal point 2, the infeed is to start at a distance of Z
ii2 before reversal point 2 and the oscillating axis is 1.0
not to wait at the reversal point for the end of the
2.0
partial infeed. Axis Z is the oscillating axis and axis X
the infeed axis. 3.0
4.0
5.0
Approach reversal point 1 Approach
and 3 sparking-out strokes end position
X
Program extract
1. Define parameters for oscillation
DEF INT ii2 Define variable for reversal area 2
OSP1[Z]=10 OSP2[Z]=60 Define reversal points 1 and 2
OST1[Z]=0 OST2[Z]=0 Reversal point 1: exact stop fine
Reversal point 2: exact stop fine
FA[Z]=150 FA[X]=0.5 Oscillating axis Z feedrate, infeed axis X
feedrate
OSCTRL[Z]=(2+8+16,1) Deactivate oscillating motion at reversal
point 2; after delete DTG spark-out and
approach end position; after delete DTG
approach reversal position
OSNC[Z]=3 3 spark-out strokes
OSE[Z]=70 End position = 70
ii2=2 Set reversal area
WAITP(Z) Enable oscillation for Z axis
Siemens AG, 2002. All rights reserved
11-472 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
11 11.02 Oscillation11.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
2. Motion-synchronized actions
WHENEVER $AA_IM[Z]
-> $AA_OVR[X]=0 $AC_MARKER[0]=0
Whenever the current position of oscillating axis Z in the MCS is
less than the start of reversal area 2
then set the axial override of infeed axis X to 0%
and set the marker with index 0 to value 0.
WHENEVER $AA_IM[Z]>=$SA_OSCILL_REVERSE_POS2[Z] DO $AA_OVR[Z]=0
Whenever the current position of oscillating axis Z in the MCS is
greater or equal to the position of reversal point 2
then set the axial override of oscillating axis Z to 0%.
WHENEVER $AA_DTEPW[X]==0 DO $AC_MARKER[0]=1
Whenever the distance-to-go of the partial infeed is
equal to 0,
then set the marker with index 0 to value 1.
WHENEVER $AC_MARKER[0]==1 DO $AA_OVR[X]=0 $AA_OVR[Z]=100
Whenever the marker with index 0 is
equal to 1,
then set the axial override of infeed axis X to 0% in order to inhibit premature
infeed (oscillating axis Z has not yet left reversal area 2 but infeed axis X is
ready for a new infeed)
set the axial override of oscillating axis Z to 100% (this cancels the 2nd
synchronized action).
-> must be programmed in a separate block
3. Start oscillation
OSCILL[Z]=(X) POSP[X]=(5,1,1) Start axes
Assign axis X as the infeed axis for
oscillating axis Z.
Axis X is to travel to end position 5 in
steps of 1.
M30 End of program
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 11-473
11 Oscillation 11.0211.2 Oscillation controlled via synchronous actions 11
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Notes
Siemens AG, 2002. All rights reserved
11-474 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
12 11.02 Punching and Nibbling 12
Punching and Nibbling
12.1 Activation, deactivation................................................................................................ 12-476
12.1.1 Language commands .......................................................................................... 12-476
12.1.2 Use of M commands............................................................................................ 12-479
12.2 Automatic path segmentation...................................................................................... 12-480
12.2.1 Path segmentation for path axes ......................................................................... 12-481
12.2.2 Path segmentation for single axes....................................................................... 12-482
12.2.3 Programming examples....................................................................................... 12-484
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 12-475
12 Punching and Nibbling 11.0212.1 Activation, deactivation 12
840 D 840Di
NCU 572
NCU 573
12.1 Activation, deactivation
12.1.1 Language commands
Programming
PDELAYON
PON G... X... Y... Z...
PONS G... X... Y... Z...
PDELAYOF
SON G... X... Y... Z...
SONS G... X... Y... Z...
SPOF
PUNCHACC(Smin, Amin, Smax, Amax)
Explanation of the parameters
PON Punching on
PONS Punching with leader on
SON Nibbling on
SONS Nibbling with leader on
SPOF Punching, nibbling Off
PDELAYON Punching with delay On
PDELAYOF Punching with delay Off
PUNCHACC Travel dependent acceleration PUNCHACC (Smin, Amin, Smax, Amax)
• "Smin" Minimum hole spacing
• "Smax" Maximum hole spacing
• "Amin" The initial acceleration Amin can be greater than Amax
• "Amax" The end acceleration Amin can be less than Amax
Function
Punching and Nibbling, activate/deactivate,
PON/SON
The punching and nibbling functions are activated
with PON and SON respectively. SPOF terminates
all functions specific to punching and nibbling
operations.
Modal commands PON and SON are mutually
exclusive, i.e. PON deactivates SON and vice versa.
Siemens AG, 2002. All rights reserved
12-476 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
12 11.02 Punching and Nibbling12.1 Activation, deactivation 12
840 D 840Di
NCU 572
NCU 573
Punching and nibbling with leader, PONS/SONS
The SONS and PONS commands also activate the
punching or nibbling functions.
In contrast to SON/PON - stroke control on
interpolation level - PONS and SONS control stroke
initiation on the basis of signals on servo level.
This means that you can work with higher stroke
frequencies and thus with an increased punching
capacity.
While signals are evaluated in the leader, all
functions that cause the nibbling or punching axes to
change position are inhibited.
Example: Handwheel mode, changes to frames via
PLC, measuring functions.
Otherwise PONS and SONS work in exactly the
same way as PON and SON.
Punching with delay
PDELAYON effects a delay in the output of the
punching stroke. The command is modal and has a
preparatory function. It is thus generally
programmed before PON.
Punching continues normally after PDELAYOF.
Travel-dependent acceleration PUNCHACC
The NC command PUNCHACC(Smin, Amin, Smax, Amax)
specifies an acceleration characteristic that defines
different accelerations (A), depending on the hole
spacing (S). Example for PUNCHACC(2, 50, 10, 100)
Hole spacing less than 2mm:
Traversal acceleration is 50% of maximum
acceleration.
Hole spacing from 2mm to 10mm:
Acceleration is increased to 100%, proportional to
the spacing.
Hole spacing greater than 10mm:
Traverse at an acceleration of 100%.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 12-477
12 Punching and Nibbling 11.0212.1 Activation, deactivation 12
840 D 840Di
NCU 572
NCU 573
Initiation of stroke
Initiation of the first stroke
The instant at which the first stroke is initiated after
Y
activation of the function differs depending on
whether nibbling or punching is selected:
PON
PON/PONS:
• All strokes – even the one in the first block after
activation – are executed at the block end.
SON
S ON/SONS:
• The first stroke after activation of the nibbling
function is executed at the start of the block. X
Positioning
• Each of the following strokes is initiated at the Positioning and stroke initiation
block end.
Punching and nibbling on the spot
A stroke is initiated only if the block contains
traversing information for the punching or nibbling
axes (axes in active plane).
However, if you wish to initiate a stroke at the same
position, you can program one of the punching/nibbling
axes with a traversing path of 0.
Additional notes
Machining with rotatable tools
Use the tangential control function if you wish to
position rotatable tools at a tangent to the
programmed path.
Siemens AG, 2002. All rights reserved
12-478 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
12 11.02 Punching and Nibbling12.1 Activation, deactivation 12
840 D 840Di
NCU 572
NCU 573
12.1.2 Use of M commands
By using macro technology, you can also use M
commands instead of language commands:
DEFINE M22 AS SON Nibbling on
DEFINE M122 AS SONS Nibbling with leader on
DEFINE M25 AS PON Punching on
DEFINE M125 AS PONS Punching with leader on
DEFINE M26 AS PDELAYON Punching on with delay
DEFINE M20 AS SPOF Punching, nibbling off
DEFINE M23 AS SPOF Punching, nibbling off
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 12-479
12 Punching and Nibbling 11.0212.2 Automatic path segmentation 12
840 D 840Di
NCU 572
NCU 573
12.2 Automatic path segmentation
Programming
SPP=
SPN=
Explanation
SPP Size of path section (maximum distance between strokes); modal
SPN Number of path sections per block; non-modal
Function
Path segmentation
When punching or nibbling is active, SPP and SPN
cause the total traversing distance programmed for
the path axes to be divided into a number of path
sections of equal length (equidistant path
segmentation). Each path segment corresponds
internally to a block.
Number of strokes
When punching is active, the first stroke is executed
at the end of the first path segment. In contrast, the
first nibbling stroke is executed at the start of the first
path segment.
The number of punching/nibbling strokes over the
total traversing path is thus as follows:
Punching:
Number of strokes = number of path segments
Nibbling:
Number of strokes = number of path segments
+ 1
Auxiliary functions
Auxiliary functions are executed in the first of the
generated blocks.
Siemens AG, 2002. All rights reserved
12-480 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
12 11.02 Punching and Nibbling12.2 Automatic path segmentation 12
840 D 840Di
NCU 572
NCU 573
12.2.1 Path segmentation for path axes
Sequence
Length of SPP path segment
With the SPP command, you specify the maximum
distance between strokes and thus the maximum
length of the path segments into which the total
traversing distance is to be divided.
The command is deactivated with SPOF or SPP=0.
Example:
N10 G1 SON X0 Y0
N20 SPP=2 X10
In this example, the total traversing distance of
10mm is divided into 5 path segments of 2mm
(SPP=2) each.
The path segments effected by SPP are always
Y
equidistant, i.e. all segments are equal in length.
In other words, the programmed path segment size
(SPP setting) is valid only if the quotient of the total
traversing distance and the SPP value is an integer.
If this is not the case, the size of the path segment is Y2
reduced internally such as to produce an integer E1
quotient.
E1
Example:
N10 G1 G91 SON X10 Y10 X2 X
N20 SPP=3.5 X15 Y15 X2/Y2 Programmed path
(nibbling or punching block)
E1 Programmed path segment
E1' Automatically rounded path segment length
When the total traversing distance is 15mm and the
path segment length 3.5mm, the quotient is not an
integer value (4.28).
In this case, the SPP value is reduced down to the
next possible integer quotient. The result in this
example would be a path segment length of 3mm.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 12-481
12 Punching and Nibbling 11.0212.2 Automatic path segmentation 12
840 D 840Di
NCU 572
NCU 573
Number of SPN path segments
Y
SPN defines the number of path segments to be
generated from the total traversing distance. The
length of the segments is calculated automatically.
Since SPN is non-modal, punching or nibbling must Y2
be activated beforehand with PON or SON
respectively.
Y1
SPP and SPN in the same block X1 X
X2
If you program both the path segment length (SPP)
X2/Y2 Programmed traversing distance
and the number of path segments (SPN) in the X1 Automatically calculated segment in X
same block, then SPN applies to this block and SPP Y1 Automatically calculated segment in Y
to all the following blocks.
If SPP was activated before SPN, then it takes effect
again after the block with SPN.
Additional notes
Provided that punching/nibbling functions are
available in the control, then it is possible to program
the automatic path segmentation function with SPN
or SPP even when the punching/nibbling functions
are not in use.
12.2.2 Path segmentation for single axes
If single axes are defined as punching/nibbling axes
in addition to path axes, then the automatic path
segmentation function can be activated for them.
Response of single axis to SPP
The programmed path segment length (SPP)
basically refers to the path axes.
For this reason, the SPP value is ignored in blocks
which contain a single axis motion and an SPP
value, but not a programmed path axis.
Siemens AG, 2002. All rights reserved
12-482 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
12 11.02 Punching and Nibbling12.2 Automatic path segmentation 12
840 D 840Di
NCU 572
NCU 573
If both a single axis and a path axis are programmed
in the block, then the single axis responds according
to the setting of the appropriate machine data.
1. Default setting
The path traversed by the single axis is distributed
evenly among the intermediate blocks generated by
SPP.
100 80 100
60
Example: 40
N10 G1 SON X10 A0 20
N20 SPP=3 X25 A100
As a result of the programmed distance between
strokes of 3mm, five blocks are generated for the
total traversing distance of the X axis (path axis) of
15mm. 1 2
The A axis thus rotates through 20° in every block.
2. Single axis without path segmentation
The single axis traverses the total distance in the
first of the generated blocks.
3. With/without path segmentation
The response of the single axis depends on the
interpolation of the path axes:
• Circular interpolation: With path segmentation
• Linear interpolation: Without path segmentation
Response to SPN
The programmed number of path segments is
applicable even if a path axis is not programmed in
the same block.
Precondition: The single axis is defined as a
punching/nibbling axis.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 12-483
12 Punching and Nibbling 11.0212.2 Automatic path segmentation 12
840 D 840Di
NCU 572
NCU 573
12.2.3 Programming examples
Programming example 1
The programmed nibbling paths must be divided
4 1 X
automatically into equidistant path segments.
62.5 75 75
Y
0
DO $AN_ESR_TRIGGER=1
• and also dependent on EU synchronized operation (if, for
example, Y is defined as EU following axis and if the max.
allowed deviation of synchronized operation shall be
100 µml):
IDS=03 WHENEVER ABS($VA_EG_SYNCDIFF[Y])>0.1
DO $AN_ESR_TRIGGER=1
13.7 Link communication (SW 5.2 and higher)
Function
The NCU link, which connects several NCU units
from an installation, is used in configurations with a
distributed system design. When there is a high
demand for axes and channels, e.g. with revolving
machines and multi-spindle machines, computing
capacity, configuration options and memory areas
can reach their limits when only one NCU is used.
Siemens AG, 2002. All rights reserved
13-522 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.7 Link communication (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Several networked NCUs connected by means of an
NCU link module represent an open, scalable
solution that meets all the requirements of this type
of machine tool. The NCU link module (hardware)
provides high-speed NCU-to-NCU communication.
Options providing this functionality can be ordered
separately.
Function
Several NCUs linked via link modules can have read
and write access to a global NCU memory area via
the system variables described in the following.
• Each NCU linked via a link module can use
global link variables. These link variables are
addressed in the same way by all connected
NCUs.
• Link variables can be programmed as system
variables.
As a rule, the machine manufacturer defines and
documents the meaning of these variables.
• Applications for link variables:
- Global machine states
- Workpiece clamping open/closed
- Etc.
• Relatively small data volume
• Very high transfer speed,
therefore: Use is intended for time-critical
information.
• These system variables can be accessed from
the parts program and from synchronized
actions. The size of the memory area for global
NCU system variables configurable.
When a value is written in a global system variable, it
can be read by all the NCUs connected after one
interpolation cycle.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-523
13 Additional Functions 11.0213.7 Link communication (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Link variables are global system data that can be
addressed by the connected NCUs as system
variables. The
- contents of these variables,
- their data type,
- use, and
- position (access index) in the link memory
are defined by the user (in this case generally the
machine manufacturer).
Link variables are stored in the link memory.
After power-up, the link memory is initialized with 0.
The following link variables can be addressed within
the link memory:
• INT $A_DLB[i] ; data byte (8 bits)
• INT $A_DLW[i] ; data word (16 bits)
• INT $A_DLD[i] ; double data word (32 bits)
• REAL $A_DLR[i] ; real data (64 bits)
According to the type in question, 1, 2, 4 or 8 bytes
are addressed when the link variables are
written/read.
Index i defines the start of the respective variable in
relation to the start of the configured link memory.
The index is counted from 0 up.
Value ranges
The different data types have the following value
ranges:
BYTE: 0 to 255
WORD: –32768 to 32767
DWORD: –2147483648 to 2147483647
REAL: –4.19e-308 to 4.19e-307
The various NCU applications sharing access to the
link memory at the same time must use the link
memory in a uniform manner. When the process is
completely separate in time, the link memory can be
occupied differently.
Siemens AG, 2002. All rights reserved
13-524 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.7 Link communication (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Warning
A link variable write process is only then completed
when the written information is also available to all
the other NCUs. Approximately two interpolation
cycles are necessary for this process. Local writing
to the link memory is delayed by the same time for
purposes of consistency.
For more information, please refer to the Description
of Functions B3 (SW 5)
Programming example
$A_DLB[5]=21 The 5th byte in the shared link memory is
assigned value 21.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-525
13 Additional Functions 11.0213.8 Axis container (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
13.8 Axis container (SW 5.2 and higher)
Function
With revolving machines/multi-spindle machines the
axes holding the workpiece move from one
machining station to the next.
As the machining stations are controlled by different
NCU channels, atstation/position change the axes
holding the workpiece must be dynamically
reassigned to the appropriate NCU channel. The
axis container is provided for this purpose.
Only one workpiece clamping axis/spindle can be
active at any one time at the local machining station.
The axis container compiles the possible
connections with all clamping axes/spindles, of
which only exactly one is always activated for the
machining station.
The following can be assigned via axis containers:
• Local axes and/or
• Link axes (see Fundamentals)
The available axes that are defined in the axis
container can be changed by switching the entries in
the axis container.
This switching function can be triggered from the
parts program.
The axis containers with link axes are a tool that is
valid across NCUs (NCU global) and is coordinated
by the control.
It is also possible to have axis containers in which
only local axes are managed.
Detailed information on configuring axis containers
can be found in /FB/, B3 (SW 5.2)
The entries in the axis container can be switched by
increment n via the commands:
Programming
AXCTSWE (CT )
i AXIS CONTAINER SWITCH ENABLE
AXCTSWED(CT )
i AXIS CONTAINER SWITCH ENABLE
DIRECT
Siemens AG, 2002. All rights reserved
13-526 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.8 Axis container (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Explanation
CT or Number of the axis container whose contents
i
are to be switched or
e.g. A_CONT1 individual name of axis container set via MD.
Function
AXCTSWE ()
Each channel whose axes are contained in the
specified container issues an enable for a
container rotation, if it has finished machining
the position/station. Once the control receives
the enables from all channels for the axes in
the container, the container is rotated with the
increment specified in the SD.
Channel axis Logical machine axis image
name
X 1 AX2 1 Local machine axis 2
Y 2 AX3 2 Local machine axis 3
Z 6
S1 7
CT1_SL1 Axis container 1 entry 1 (slot 1)
No. in the logical
machine axis image
Axis container 1 Axis container 1
NC1_AX1 NC1_AX5
NC2_AX2
NC1_AX1
NC2_AX1 AXCTSWE(CT1) NC2_AX2
...
NC2_AX1
... ...
... ...
NC1_AX5
...
Axis container entries displaced by increments of 1
In the preceding example, after axis container
rotation by 1, axis AX5 on NCU1 is assigned to
channel axis Z instead of axis AX1 on NCU1.
The command variant AXCTSWED(CTi) can be
used to simplify startup. Under the sole effect of the
active channel, the axis container rotates around the
increment stored in the SD.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-527
13 Additional Functions 11.0213.9 Program execution time/Workpiece counter (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
This call may only be used if the other channels,
which have axes in the container are in the RESET
state.
After an axis container rotation, all NCUs whose
channels refer to the rotated axis container via the
logical machine axis image are affected by the new
axis assignment.
13.9 Program execution time/Workpiece counter (SW 5.2 and higher)
Function
Information on the program execution time and on
the workpiece count are provided to support the
person working at the machine tool.
This information is specified in the respective
machine data and can be edited as a system
variable in the NC and/or PLC program. This
information is also available to the MMC at the
operator panel front interface.
13.9.1 Program runtime
Function
Under this function, timers are provided as system
variables, which can be used to monitor
technological processes.
These timers can only be read. They can be
accessed at any time by the MMC in read mode.
Explanation
The following two timers are defined as NCK-
specific system variables and always active.
$AN_SETUP_TIME Time in minutes since the last setup;
is reset with SETUP
Siemens AG, 2002. All rights reserved
13-528 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.9 Program execution time/Workpiece counter (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
$AN_POWERON_TIME Time in minutes since the last PowerOn;
is reset with POWERON
The following three timers are defined as
channel-specific system variables and can be
activated via machine data.
$AC_OPERATING_TIME Total execution time in seconds of NC
programs in the automatic mode
$AC_CYCLE_TIME Execution time in seconds of the selected NC
program
$AC_CUTTING_TIME Tool operation time in seconds
$MC_RUNTIMER_MODE Tool operation time in seconds
All timers are reset with default values when the
control is powered up, and can be read independent
of their activation.
Programming example
1. Activate runtime measurement for the active NC
program; no measurement with active dry run
feedrate and program testing:
$MC_PROCESSTIMER_MODE = 'H2'
2. Activate measurement for the tool operating time;
measurement also with active dry run feedrate and
program testing:
$MC_PROCESSTIMER_MODE= 'H34'
3. Activate measurement for the total runtime and
tool operating time; measurement also during
program testing:
$MC_PROCESSTIMER_MODE= 'H25'
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-529
13 Additional Functions 11.0213.9 Program execution time/Workpiece counter (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
13.9.2 Workpiece counter
Function
The "Workpiece counter" function can be used to
prepare counters, e.g. for internal counting of
workpieces on the control. These counters exist as
channel-specific system variables with read and
write access within a value range from 0 to
999 999 999.
Machine data can be used to control counter
activation, counter reset timing and the counting
algorithm.
Explanation
The following counters are provided:
$AC_REQUIRED_PARTS Number of workpieces required
In this counter you can define the number of workpieces at which the
actual workpiece counter $AC_ACTUAL_PARTS is reset to zero.
Machine data can be used to configure the generation of the display
alarm "Required number of workpieces reached" and the channel
VDI signal "Required number of workpieces reached".
$AC_TOTAL_PARTS Total number of workpieces actually produced (total actual)
The counter indicates the total number of workpieces produced
since the starting time. The counter is automatically reset with
default values only when the control is powered up.
$AC_ACTUAL_PARTS Number of actual workpieces. This counter records the number of all
workpieces produced since the starting time. The counter is
automatically reset to zero (on condition that $AC_REQUIRED_PARTS
is not equal to 0) when the required number of workpieces
($AC_REQUIRED_PARTS) has been reached.
$AC_SPECIAL_PARTS Number of workpieces specified by the user
This counter allows user-defined workpiece counting. Alarm output can
be defined for the case of identity with $AC_REQUIRED_PARTS
(workpiece target). The user must reset the counter
The "Workpiece counter" function operates
independently of the tool management functions.
All counters can be read and written from the MMC.
All counters are reset with default values when the
control is powered up, and can be read/written
independent of their activation.
Siemens AG, 2002. All rights reserved
13-530 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.9 Program execution time/Workpiece counter (SW 5.2 and higher) 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
1. Activate workpiece counter $AC_REQUIRED_PARTS:
$MC_PART_COUNTER='H3' $AC_REQUIRED_PARTS is active, display
alarm on $AC_REQUIRED_PARTS ==
$AC_SPECIAL_PARTS
2. Activate workpiece counter $AC_TOTAL_PARTS:
$MC_PART_COUNTER='H10' $AC_TOTAL_PARTS is active, the counter is
$MC_PART_COUNTER_MCODE[0]=80 incremented by 1 on each M02,
$MC_PART_COUNTER_MCODE[0] is
irrelevant
3. Activate workpiece counter $AC_ACTUAL_PARTS:
$MC_PART_COUNTER='H300' $AC_TOTAL_PARTS is active, the counter is
$MC_PART_COUNTER_MCODE[1]=17 incremented by 1 on each M17
4. Activate workpiece counter $AC_SPECIAL_PARTS:
$MC_PART_COUNTER='H3000' $AC_SPECIAL_PARTS is active, the counter
$MC_PART_COUNTER_MCODE[2]=77 is incremented by 1 on each M77
5. Deactivate workpiece counter $AC_ACTUAL_PARTS:
$MC_PART_COUNTER='H200' $AC_TOTAL_PARTS is not active, rest
$MC_PART_COUNTER_MCODE[1]=50 irrelevant
6. Activate all counters, examples 1-4:
$MC_PART_COUNTER ='H3313' $AC_REQUIRED_PARTS is active
$MC_PART_COUNTER_MCODE[0] =80 Display alarm on $AC_REQUIRED_PARTS
$MC_PART_COUNTER_MCODE[1] =17 == $AC_SPECIAL_PARTS
$MC_PART_COUNTER_MCODE[2] =77 $AC_TOTAL_PARTS is active, the counter is
incremented by 1 on each M02
$MC_PART_COUNTER_MCODE[0] is
irrelevant
$AC_ACTUAL_PARTS is active, the counter
is incremented by 1 on each M17
$AC_SPECIAL_PARTS is active, the counter
is incremented by 1 on each M77
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-531
13 Additional Functions 11.0213.10 Interactive window call from parts program, command MMC 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
13.10 Interactive window call from parts program, command MMC
(SW 4.4 and higher)
Programming
MMC ("CYCLES, PICTURE_ON, T_SK.COM, PICTURE, MGUD.DEF, PICTURE_3.AWB,
TEST_1, A1","S")
Explanation
CYCLES Operating area in which the configured
user dialog boxes are implemented.
PICTURE_ON or PICTURE_OFF Command: display selection or display
deselection
T_SK.COM Com file: Name of the dialog display file
(user cycles). The dialog display design
is defined here. The dialog displays can
show user variables and/or
comments.
DISPLAY Name of dialog display: The individual
displays are selected via the names of
the dialog displays.
MGUD.DEF User data definition file, which is
addressed while reading/writing
variables.
PICTURE_3.AWB Graphics file
TEST_1 Display time or acknowledgement
variable
A1 Text variables...",
"S" Acknowledgement mode: synchronous,
acknowledgement via "OK" soft key
Function
With the MMC command, user-defined dialog
windows (dialog displays) can be displayed on the
MMC/HMI from the parts program.
The dialog window design is defined in pure text
configuration (COM file in cycles directory), while the
MMC/HMI system software remains unchanged.
User-defined dialog windows cannot be called
simultaneously in different channels.
Siemens AG, 2002. All rights reserved
13-532 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.10 Interactive window call from parts program, command MMC 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Please see the detailed notes on how to program the
MMC command (incl. programming examples) in
/IAM/ in the manuals IM1 through IM4 depending on
the MMC/HMI software used.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-533
13 Additional Functions 11.0213.11 Influencing the motion control 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
13.11 Influencing the motion control
13.11.1 Percentage jerk correction: JERKLIM
Programming
JERKLIM[axis]= ...
Explanation of the command
Percentage change for the greatest permissible jerk relative to
JERKLIM the value set in the machine data for the axis
Machine axis whose jerk limit has to adapted
Axis
Function
In critical program sections, it may be necessary to
limit the jerk to below maximum value, for example,
to reduce mechanical stress. The acceleration mode
SOFT must be active.
The function only effects path axes.
Sequence
In the AUTOMATIC modes, the jerk limit is limited to
the percentage of the jerk limit stored in the machine
data.
Example: N60 JERKLIM[X]=75
Meaning: The axis carriage in the X direction must
be accelerated/decelerated with only 75% of the jerk
permissible for the axis.
Value range: 1 ... 200
100 corresponds to: no effect on jerk.
100 is applied after RESET and parts program start.
Siemens AG, 2002. All rights reserved
13-534 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.11 Influencing the motion control 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
A further example will follow at the end of the next
subsection.
13.11.2 Percentage velocity correction: VELOLIM
Programming
VELOLIM[axis]= ...
Explanation of the command
Percentage change for the greatest permissible velocity relative
VELOLIM to the value set in the machine data for the axis
Machine axis whose velocity limit has to adapted
Axis
Function
In critical program sections, it may be necessary to
limit the velocity to below maximum values, for
example, to reduce mechanical stress or enhance
finish. The function only effects path and positioning
axes.
Sequence
In the AUTOMATIC modes, the velocity limit is
limited to the percentage of the velocity limit stored
in the machine data.
Example: N70 VELOLIM[X]=80
Meaning: The axis carriage in the X direction must
travel at only 80% of the velocity permissible for the
axis.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-535
13 Additional Functions 11.0213.12 Master/slave grouping 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Value range: 1 ... 100
100 corresponds to: no effect on velocity.
100 is applied after RESET and parts program start.
Programming example
N1000 G0 X0 Y0 F10000 SOFT G64
N1100 G1 X20 RNDM=5 ACC[X]=20
ACC[Y]=30
N1200 G1 Y20 VELOLIM[X]=5
JERKLIM[Y]=200
N1300 G1 X0 JERKLIM[X]=2
N1400 G1 Y0
M30
13.12 Master/slave grouping
Programming:
MASLDEF(Slv1, Slv2, ..., master axis) For dynamic configuration
(SW 6.4 and higher)
MASLDEL(Slv1, Slv2, ..., ) For dynamic configuration
(SW 6.4 and higher)
MASLON(Slv1, Slv2, ..., )
MASLOF(Slv1, Slv2, ..., )
MASLOFS(Slv1, Slv2, ..., ) (SW 6.4 and higher)
Explanation of the parameters
Slv1, Slv2, ... Slave axes led by a master axis
Master axis Axis leading slave axes defined in a
master/slave grouping
Siemens AG, 2002. All rights reserved
13-536 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.12 Master/slave grouping 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Function
The master/slave coupling in SW 6.4 and lower
permitted coupling of the slave axes to their master
axis only while the axes involved are stopped.
Extension of SW 6.4 permits coupling and
uncoupling of rotating, speed-controlled spindles
and dynamic configuration.
Dynamic configuration
MASLDEF (SW 6.4 and higher)
Definition of a master/slave grouping
from the parts program. In SW 6.4 and
lower, definition as in the machine data
only.
MASLDEL (SW 6.4 and higher)
The instruction cancels assignment of the
slave axes to the master axis and
simultaneously uncouples the current
coupling, like MASLOF.
The master/slave definitions declared in
the machine data are retained.
General
MASLON Enable a temporary coupling
MASLOF This instruction uncouples an active
coupling.
(SW 6.4 and higher)
For spindles in speed control mode, this
instruction is executed immediately. The
slave spindles rotating at this time retain
their speeds until next speed
programming.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-537
13 Additional Functions 11.0213.12 Master/slave grouping 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
MASLOFS (SW 6.4 and higher)
The MASLOFS instruction can be used
to decelerate slave spindles automatically
on uncoupling. For axes and spindles in
positioning mode, uncoupling is only
possible while stopped.
More information (SW 6.4 and higher)
For MASLOF/MASLOFS, the implicit preprocessing
stop is not required. Because of the missing
preprocessing stop, the $P system variables for the
slave axes do not provide updated values until next
programming.
Programming example
Dynamic configuration of a master/slave coupling
from the parts program:
The axis relevant after axis container rotation must
become the master axis.
MASLDEF(AUX,S3) ; S3 master for AUX
MASLON(AUX) ; Coupling ON for AUX
M3=3 S3=4000 ; Clockwise rotation
MASLDEL(AUX) ; Clear configuration and
; uncoupling
AXCTSWE(CT1) ; Container rotation
Siemens AG, 2002. All rights reserved
13-538 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
13 11.02 Additional Functions13.12 Master/slave grouping 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
To enable coupling with another spindle after
container rotation, the previous coupling must be
uncoupled, the configuration cleared, and a new
coupling configured.
Example of a coupling sequence Position 3 /
Container CT1
Original situation
See /FB/, B3 Section 2.6 Axis container
After rotation by one slot
▀
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 13-539
13 Additional Functions 11.0213.12 Master/slave grouping 13
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Siemens AG, 2002. All rights reserved
13-540 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs 14
User Stock Removal Programs
14.1 Supporting functions for stock removal ...................................................................... 14-542
14.2 Contour preparation: CONTPRON............................................................................. 14-543
14.3 Contour decoding: CONTDCON (SW 5.2 and higher)............................................... 14-550
14.4 Intersection of two contour elements: INTERSEC ..................................................... 14-554
14.5 Traversing a contour element from the table: EXECTAB .......................................... 14-556
14.6 Calculate circle data: CALCDAT ................................................................................ 14-557
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-541
14 User Stock Removal Programs 11.0214.1 Supporting functions for stock removal 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
14.1 Supporting functions for stock removal
User stock removal programs
Preprogrammed stock removal programs are
provided for stock removal. You can also use the
following functions to develop your own stock
removal programs.
CONTPRON Activate tabular contour preparation (11 columns)
CONTDCON Activate tabular contour decoding (6 columns)
INTERSEC Calculate intersection of two contour elements.
(Only for tables created by CONTPRON).
EXECTAB Block-by-block execution of contour elements of a table
(Only for tables created by CONTPRON).
CALCDAT Calculate radii and center points
You can use these functions universally, not just for
stock removal.
Siemens AG, 2002. All rights reserved
14-542 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
14.2 Contour preparation: CONTPRON
Programming
CONTPRON (TABNAME, MACH, NN, MODE)
EXECUTE (ERROR)
Explanation of the parameters
CONTPRON Activate contour preparation
TABNAME Name of contour table
MACH Parameters for type of machining:
"G": Longitudinal turning: Inside machining
"L": Longitudinal turning: External machining
"N": Face turning: Inside machining
"P": Face turning: External machining
NN Number of relief cuts in result variable of type INT
MODE (SW 4.4 and Direction of machining, type INT
higher) 0 = Contour preparation forward (SW 4.3 and lower, default value)
1 = Contour preparation in both directions
EXECUTE Terminate contour preparation
ERROR Variable for error checkback, type INT
1 = error; 0 = no error
Function
The blocks executed after CONTPRON describe the
contour to be prepared.
The blocks are not processed but are filed in the
contour table.
Each contour element corresponds to one row in the
two-dimensional array of the contour table.
The number of relief cuts is returned.
EXECUTE deactivates the contour preparation and
switches back to the normal execution mode.
Example:
N30 CONTPRON(…)
N40 G1 X… Z…
N50…
N100 EXECUTE(…)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-543
14 User Stock Removal Programs 11.0214.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
Preconditions for the call
Before CONTPRON is called
• a starting point must be approached which
permits collision-free machining,
• tool edge radius compensation with G40 must be
deactivated.
Permitted traversing commands, coordinate
system
Only G commands G0 to G3 are permitted for
contour programming in addition to rounding and
chamfer.
SW 4.4 and higher supports circular-path
programming via CIP and CT.
The functions Spline, Polynomial, thread produce
errors.
It is not permitted to change the coordinate system by
activating a frame between CONTPRON and
EXECUTE. The same applies to a change between
G70 and G71/ G700 and G710.
Changing the geometry axes with GEOAX while
preparing the contour table produced an alarm.
Terminate contour preparation
When you call the predefined subroutine EXECUTE
(variable), contour preparation is terminated and the
system switches back to normal execution when the
contour has been described. The variable then
indicates:
1 = error
0 = no error (the contour is error free).
Relief cut elements
The contour description for the individual relief cut
elements can be performed either in a subroutine or
in individual blocks.
Stock removal irrespective of the programmed
contour direction (SW 4.4 and higher)
In SW 4.4 and higher, contour preparation has been
expanded. Now when CONTPRON is called, the
contour table is available irrespective of the
programmed direction.
Siemens AG, 2002. All rights reserved
14-544 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example 1 X
Create a contour table with (20,150)150
• name KTAB,
• up to 30 contour elements (circles, straight lines),
(30,110)
• a variable for the number of relief cut elements,
100
• a variable for error messages
(30,65)
(70,50)
50 (45,50) (85,40)
(90,30)
(90,0)
Z
50 100 150
NC parts program
N10 DEF REAL KTAB[30,11] Contour table named KTAB and, for
example, a maximum of 30 contour
elements
Parameter value 11 is a fixed size
N20 DEF INT ANZHINT Variable for number of relief cut elements
with name ANZHINT
N30 DEF INT ERROR Variable for acknowledgment
0 = no error, 1 = error
N40 G18
N50 CONTPRON (KTAB,"G",ANZHINT) Contour preparation call
N60 G1 X150 Z20 N60 to N120 contour description
N70 X110 Z30
N80 X50 RND=15
N90 Z70
N100 X40 Z85
N110 X30 Z90
N120 X0
N130 EXECUTE(ERROR) Terminate filling of contour table, switch to
normal program execution
N140 … Continue processing table
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-545
14 User Stock Removal Programs 11.0214.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Table KTAB
(0) (1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
7 7 11 0 0 20 150 0 82.40535663 0 0
0 2 11 20 150 30 110 - 104.0362435 0 0
1111
1 3 11 30 110 30 65 0 90 0 0
2 4 13 30 65 45 50 0 180 45 65
3 5 11 45 50 70 50 0 0 0 0
4 6 11 70 50 85 40 0 146.3099325 0 0
5 7 11 85 40 90 30 0 116.5650512 0 0
6 0 11 90 30 90 0 0 90 0 0
0 0 0 0 0 0 0 0 0 0 0
0 0 0 0 0 0 0 0 0 0 0
Explanation of column contents
(0) Pointer to next contour element (to the row number of that column)
(1) Pointer to previous contour element
(2) Coding of contour mode for the movement
Possible values for X = abc
a = 102 G90 = 0 G91 = 1
b = 101 G70 = 0 G71 = 1
c = 100 G0 = 0 G1 = 1 G2 = 2 G3 = 3
(3), (4) Starting point of contour elements
(3) = abscissa, (4) = ordinate in current plane
(5), (6) Starting point of contour elements
(5) = abscissa, (6) = ordinate in current plane
(7) Max/min indicator: Identifies local maximum and minimum values on the contour
(8) Maximum value between contour element and abscissa (for longitudinal machining) or
ordinate (for transverse machining).
The angle depends on the type of machining programmed.
(9), (10) Center point coordinates of contour element, if it is a circle block.
(9) = abscissa, (10) = ordinate
Siemens AG, 2002. All rights reserved
14-546 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example 2 X
Create a contour table with
150
• name KTAB,
• up to 92 contour elements (circles, straight lines),
• mode: Longitudinal turning, external machining (100,100)
100
• preparation forwards and backwards. (-30,80)
(-40,80)
50
(0,45) (20,45)
(-30,30)
(-15,30)
(20,20)
Z
-50 50 100
NC parts program
N10 DEF REAL KTAB[92,11] Contour table named KTAB and, for
example, a maximum of 92 contour
elements
Parameter value 11 is a fixed size
N20 CHAR BT="L" Mode for CONTPRON:
Longitudinal turning, external machining
N30 DEF INT HE=0 Number of relief cut elements=0
N40 DEF INT MODE=1 Preparation forwards and backwards
N50 DEF INT ERR=0 Error checkback message
...
N100 G18 X100 Z100 F1000
N105 CONTPRON (KTAB, BT, HE, MODE) Contour preparation call
N110 G1 G90 Z20 X20
N120 X45
N130 Z0
N140 G2 Z-15 X30 K=AC(-15) I=AC(45)
N150 G1 Z-30
N160 X80
N170 Z-40
N180 EXECUTE(ERR) Terminate filling of contour table, switch to
normal program execution
...
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-547
14 User Stock Removal Programs 11.0214.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Table KTAB
After contour preparation is finished, the contour is
available in both directions.
Row Column
(0) (1) (2) (3) (4) (5) (6) (7) (8) (9) (10)
0 61) 72) 11 100 100 20 20 0 45 0 0
1 03) 2 11 20 20 20 45 –3 90 0 0
2 1 3 11 20 45 0 45 0 0 0 0
3 2 4 12 0 45 –15 30 5 90 –15 45
4 3 5 11 –15 30 –30 30 0 0 0 0
5 4 7 11 –30 30 –30 45 –1111 90 0 0
6 7 04) 11 –30 80 –40 80 0 0 0 0
7 5 6 11 –30 45 –30 80 0 90 0 0
8 15) 26) 0 0 0 0 0 0 0 0 0
...
83 84 07) 11 20 45 20 80 0 90 0 0
84 90 83 11 20 20 20 45 –1111 90 0 0
85 08) 86 11 –40 80 –30 80 0 0 0 0
86 85 87 11 –30 80 –30 30 88 90 0 0
87 86 88 11 –30 30 –15 30 0 0 0 0
88 87 89 13 –15 30 0 45 –90 90 –15 45
89 88 90 11 0 45 20 45 0 0 0 0
90 89 84 11 20 45 20 20 84 90 0 0
91 839) 8510) 11 20 20 100 100 0 45 0 0
Explanation of column contents
(0) Pointer to next contour element (to the row number of that column)
(1) Pointer to previous contour element
(2) Coding of contour mode for the movement
Possible values for X = abc
a = 102 G90 = 0 G91 = 1
b = 101 G70 = 0 G71 = 1
c = 100 G0 = 0 G1 = 1 G2 = 2 G3 = 3
(3), (4) Starting point of contour elements
(3) = abscissa, (4) = ordinate in current plane
(5), (6) Starting point of contour elements
(5) = abscissa, (6) = ordinate in current plane
(7) Max/min indicator: Identifies local maximum and minimum values on the contour
(8) Maximum value between contour element and abscissa (for longitudinal machining) or
ordinate (for transverse machining)
The angle depends on the type of machining programmed.
Siemens AG, 2002. All rights reserved
14-548 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.2 Contour preparation: CONTPRON 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
(9), (10) Center point coordinates of contour element, if it is a circle block.
(9) = abscissa, (10) = ordinate
Explanation of comment in columns
Always in table line 0: 1) Previous: Line n contains the contour end forwards
2) Following: Line n is the contour table end forwards
Once each within the contour elements forwards:
3) Previous: Contour start (forwards)
4) Following: Contour end (forwards)
Always in line contour table end (forwards) +1:
5) Previous: Number of relief cuts forwards
6) Following: Number of relief cuts backwards
Once each within the contour elements backwards:
7) Following: Contour end (backwards)
8) Previous: Contour start (backwards)
Always in last line of table:
9) Previous: Line n is the contour table start (backwards)
10) Following: Line n contains the contour start (backwards)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-549
14 User Stock Removal Programs 11.0214.3 Contour decoding: CONTDCON (SW 5.2 and higher) 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
14.3 Contour decoding: CONTDCON (SW 5.2 and higher)
Programming
CONTDCON (TABNAME,MODE)
EXECUTE (ERROR)
Explanation of the parameters
CONTDCON Activate contour preparation
TABNAME Name of contour table
MODE Direction of machining, type INT
0 = Contour preparation (default) according to the contour block sequence
EXECUTE Terminate contour preparation
ERROR Variable for error checkback, type INT
1 = error; 0 = no error
Function
The blocks executed after CONTPRON describe the
contour to be decoded.
The blocks are not processed but stored, memory-
optimized, in a 6-column contour table.
Each contour element corresponds to one row in the
contour table. When familiar with the coding rules
specified below, you can combine DIN code
programs from the tables to produce applications
(e.g. cycles). The data for the starting point are
stored in the table cell with the number 0. The G
codes permitted for CONTDCON in the program
section to be included in the table are more
comprehensive than for the CONTPRON function. In
addition, feedrates and feed type are also stored for
each contour section.
EXECUTE deactivates the contour preparation and
switches back to the normal execution mode.
Example:
N30 CONTDCON(…)
N40 G1 X… Z…
N50…
N100 EXECUTE(…)
Siemens AG, 2002. All rights reserved
14-550 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.3 Contour decoding: CONTDCON (SW 5.2 and higher) 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Additional notes
Preconditions for the call
Before CONTDCON is called
• a starting point must be approached which
permits collision-free machining,
• tool edge radius compensation with G40 must be
deactivated.
Permitted traversing commands, coordinate
system
The following G groups and specified commands are
permissible for contour programming:
G group 1: G0, G1, G2, G3
G group 10: G9
G group 11: G60, G44, G641, G642
G group 13: G70, G71, G700, G710
G group 14: G90, G91
G group 15: G93, G94, G95, G96
also corner and chamfer.
Circular-path programming is possible via CIP and
CT. The functions Spline, Polynomial, thread
produce errors.
It is not permitted to change the coordinate system by
activating a frame between CONDCRON and
EXECUTE. The same applies to a change between
G70 and G71/ G700 and G710.
Changing the geometry axes with GEOAX while
preparing the contour table produced an alarm.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-551
14 User Stock Removal Programs 11.0214.3 Contour decoding: CONTDCON (SW 5.2 and higher) 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Terminate contour preparation
When you call the predefined subroutine EXECUTE
(ERROR), contour preparation is terminated and the
system switches back to normal execution when the
contour has been described. The associated variable
ERROR gives the return value:
0 = no error (contour produced no errors)
1 = error
Impermissible commands, incorrect initial conditions,
CONTDCON call repeated without EXECUTE( ), too
few contour blocks or table definitions too small
produce additional alarms.
Stock removal in the programmed contour
direction
The contour table produced using CONTDCON is
used for stock removal in the programmed direction
of the contour.
Programming example X
Create a contour table with
150
• name KTAB,
• contour elements (circles, straight lines),
• mode: Turning (100,100)
100
• preparation forward (-30,80)
(-40,80)
50
(0,45) (20,45)
(-30,30)
(-15,30)
(20,20)
Z
-50 50 100
Siemens AG, 2002. All rights reserved
14-552 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.3 Contour decoding: CONTDCON (SW 5.2 and higher) 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
NC parts program
N10 DEF REAL KTAB[9,6] Contour table with name KTAB and 9 table
cells. These allow 8 contour sets.
Parameter value 6 (column number in table)
is fixed.
N20 DEF INT MODE = 0 Default value 0: Only in programmed
contour direction. Value 1 is not permitted.
N30 DEF INT ERROR = 0 Error checkback message
...
N100 G18 G64 G90 G94 G710
N101 G1 Z100 X100 F1000
N105 CONTDCON (KTAB, MODE) Call contour decoding
MODE may be omitted (see above)
N110 G1 Z20 X20 F200 Contour description
N120 G9 X45 F300
N130 Z0 F400
N140 G2 Z-15 X30 K=AC(-15) I=AC(45)F100
N150 G64 Z-30 F600
N160 X80 F700
N170 Z-40 F800
N180 EXECUTE(ERROR) Terminate filling of contour table, switch to
normal program execution
...
Column index 0 1 2 3 4 5
Line index Contour End point End point Center point Center point Feed
mode abscissa ordinate Abscissa ordinate
0 30 100 100 0 0 7
1 11031 20 20 0 0 200
2 111031 20 45 0 0 300
3 11031 0 45 0 0 400
4 11032 –15 30 –15 45 100
5 11031 –30 30 0 0 600
6 11031 –30 80 0 0 700
7 11031 –40 80 0 0 800
8 0 0 0 0 0 0
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-553
14 User Stock Removal Programs 11.0214.4 Intersection of two contour elements: INTERSEC 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Explanation of column contents
Line 0: Coding for starting point:
Column 0:
100 (ones): G0 = 0
101 (tens): G70 = 0, G71 = 1, G700 = 2, G710 = 3
Column 1: starting point of abscissa
Column 2: starting point of ordinate
Column 3-4: 0
Column 5 Line index of last contour piece in the table
Lines 1-n: Entries for contour pieces:
Column 0:
100 (ones): G0 = 0, G1 = 1, G2 = 2, G3 = 3
101 (tens): G70 = 0, G71 = 1, G700 = 2, G710 = 3
102 (hundreds): G90 = 0, G91 = 1
103 (thousands): G93 = 0, G94 = 1, G95 = 2, G96 = 3
104 (ten thousands): G60 = 0, G44 = 1, G641 = 2, G642 = 3
105 (hundred thousands): G9 = 1
Column 1: End point abscissa
Column 2: End point ordinate
Column 3: Center point Abscissa for circular interpolation
Column 4: Center point ordinate for circular interpolation
Column 5: Feedrate
14.4 Intersection of two contour elements: INTERSEC
Programming
VARIB=INTERSEC (TABNAME1[n1], TABNAME2[n2], TABNAME3)
Explanation of the parameters
VARIB Variable for status TRUE: Intersection found
FALSE: No intersection found
TABNAME1[n1] Table name and n1st contour element of the first table
TABNAME2[n2] Table name and n2nd contour element of the second table
TABNAME3 Table name for the intersection coordinates in the active plane G17–G19
Siemens AG, 2002. All rights reserved
14-554 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.4 Intersection of two contour elements: INTERSEC 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Function
INTERSEC calculates the intersection of two
normalized contour elements from the contour table
generated with CONTPRON. The indicated status
specifies whether or not an intersection exists (TRUE =
intersection, FALSE = no intersection).
Additional notes
Please note that variables must be defined before
they are used.
Programming example
Calculate the intersection of contour element 3 in
table KTAB1 and contour element 7 in table KTAB2.
The intersection coordinates in the active plane are
stored in CUT (1st element = abscissa, 2nd element
= ordinate).
If no intersection exists, the program jumps to
NOCUT (no intersection found).
DEF REAL KTAB1 [12, 11] Contour table 1
DEF REAL KTAB2 [10, 11] Contour table 2
DEF REAL CUT [2] Intersection table
DEF BOOL ISPOINT Variable for status
…
N10 ISPOINT=INTERSEC (KTAB1[3],KTAB2[7],CUT)
Call intersection of contour elements
N20 IF ISPOINT==FALSE GOTOF NOCUT Jump to NOCUT
…
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-555
14 User Stock Removal Programs 11.0214.5 Traversing a contour element from the table: EXECTAB 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
14.5 Traversing a contour element from the table: EXECTAB
Programming
EXECTAB (TABNAME[n])
Explanation of the parameter
TABNAME[n] Name of table with number n of the element
Function
You can use command EXECTAB to traverse
contour elements block by block in a table
generated, for example, with the CONTPRON
command.
Programming example
The contour elements stored in Table KTAB are
traversed non-modally by means of subroutine
EXECTAB. Elements 0 to 2 are passed in
consecutive calls.
N10 EXECTAB (KTAB[0]) Traverse element 0 of table KTAB
N20 EXECTAB (KTAB[1]) Traverse element 1 of table KTAB
N30 EXECTAB (KTAB[2]) Traverse element 2 of table KTAB
Siemens AG, 2002. All rights reserved
14-556 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
14 11.02 User Stock Removal Programs14.6 Calculate circle data: CALCDAT 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
14.6 Calculate circle data: CALCDAT
Programming
VARIB = CALCDAT(PT[n,2],NO,RES)
Explanation of the parameters
VARIB Variable for status
TRUE = circle, FALSE = no circle
PT[n,2] Points for calculation
n = number of points (3 or 4); 2 = point coordinates
NO. Number of points used for calculation: 3 or 4
RES[3] Variable for result: specification of circle center point coordinates and
radius;
0 = abscissa, 1 = ordinate of circle center point; 2 = radius
Function
Calculation of radius and circle center point coordinates
from three or four known circle points.
The specified points must be different.
Where 4 points do not lie directly on the circle an
average value is taken for the circle center point and
the radius.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 14-557
14 User Stock Removal Programs 11.0214.6 Calculate circle data: CALCDAT 14
840D 840D 810D 840Di
NCU 571 NCU 572
NCU 573
Programming example
Y
The program determines whether the three points lie
along the arc of a circle. 60
(20,50)
50
(50,40)
40
30
(65,20)
20
ERG [1]
10
X
10 20 30 40 50 60 70
ERG [0]
N10 DEF REAL Point definition
PT[3,2]=(20,50,50,40,65,20)
N20 DEF REAL RES[3] Result
N30 DEF BOOL STATUS Variable for status
N40 STATUS = CALCDAT(PT,3,RES) Call calculated circle data
N50 IF STATUS == FALSE GOTOF ERROR Jump to error
■
Siemens AG, 2002. All rights reserved
14-558 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
ERG[2]
15 11.02 Tables 15
Tables
15.1 List of instructions ....................................................................................................... 15-561
15.2 List of system variables ............................................................................................... 15-591
15.2.1 R parameters ....................................................................................................... 15-591
15.2.2 Channel-specific synchronized action variables .................................................. 15-591
15.2.3 Frames 1.............................................................................................................. 15-592
15.2.4 Toolholder data .................................................................................................... 15-593
15.2.5 Channel-specific protection zones ....................................................................... 15-601
15.2.6 Tool parameters................................................................................................... 15-603
15.2.7 Cutting edge data OEM user ............................................................................... 15-609
15.2.8 Monitoring data for tool management .................................................................. 15-617
15.2.9 Monitoring data for OEM users ............................................................................ 15-618
15.2.10 Tool-related data.................................................................................................. 15-619
15.2.11 Tool-related grinding data .................................................................................... 15-621
15.2.12 Magazine location data ........................................................................................ 15-622
15.2.13 Magazine location data for OEM users................................................................ 15-623
15.2.14 Magazine description data for tool management ................................................. 15-624
15.2.15 Tool management magazine description data for OEM users ............................ 15-625
15.2.16 Magazine module parameter ............................................................................... 15-626
15.2.17 Adapter data ........................................................................................................ 15-626
15.2.18 Measuring system compensation values............................................................. 15-626
15.2.19 Quadrant error compensation.............................................................................. 15-627
15.2.20 Interpolatory compensation.................................................................................. 15-629
15.2.21 NCK-specific protection zones............................................................................. 15-630
15.2.22 Cycle parameterization ........................................................................................ 15-631
15.2.23 System data ......................................................................................................... 15-636
15.2.24 Frames 2.............................................................................................................. 15-636
15.2.25 Tool data .............................................................................................................. 15-638
15.2.26 Magazines............................................................................................................ 15-643
15.2.27 Programmed geometry axis values ..................................................................... 15-646
15.2.28 G groups .............................................................................................................. 15-647
15.2.29 Programmed values............................................................................................. 15-647
15.2.30 Channel states ..................................................................................................... 15-651
15.2.31 Synchronized actions ........................................................................................... 15-656
15.2.32 I/Os ...................................................................................................................... 15-657
15.2.33 Reading and writing PLC variables ...................................................................... 15-657
15.2.34 NCU link............................................................................................................... 15-658
15.2.35 Direct PLC I/O...................................................................................................... 15-658
15.2.36 Tool management................................................................................................ 15-659
15.2.37 Timers .................................................................................................................. 15-662
15.2.38 Path movement.................................................................................................... 15-663
15.2.39 Speeds/accelerations........................................................................................... 15-665
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-559
15 Tables 11.02 15
15.2.40 Spindles................................................................................................................15-667
15.2.41 Polynomial values for synchronized actions.........................................................15-670
15.2.42 Channel states .....................................................................................................15-672
15.2.43 Measurement .......................................................................................................15-673
15.2.44 Positions...............................................................................................................15-677
15.2.45 Indexing axes .......................................................................................................15-679
15.2.46 Encoder values.....................................................................................................15-679
15.2.47 Axial measurement ..............................................................................................15-680
15.2.48 Offsets..................................................................................................................15-681
15.2.49 Axial paths............................................................................................................15-684
15.2.50 Oscillation.............................................................................................................15-685
15.2.51 Axial velocities......................................................................................................15-685
15.2.52 Drive data .............................................................................................................15-687
15.2.53 Axis statuses ........................................................................................................15-688
15.2.54 Master/slave links.................................................................................................15-689
15.2.55 Travel to fixed stop...............................................................................................15-690
15.2.56 Electronic gear .....................................................................................................15-691
15.2.57 Leading value coupling.........................................................................................15-692
15.2.58 Synchronized spindle ...........................................................................................15-693
15.2.59 Safety Integrated ..................................................................................................15-696
Siemens AG, 2002. All rights reserved
15-560 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.1 List of instructions 15
15.1 List of instructions
Legend:
1 Default setting at start of program (in delivery state of control system provided that another setting is not programmed).
2 The group numbers correspond to the table ”List of G functions/Preparatory functions” in /PG/, Programming Guide
Fundamentals, Section 12.3
3 Absolute end points: Modal; incremental end points: Non-modal; otherwise modal/non-modal depending
on syntax of G function
4 IPO parameters act incrementally as arc centers. They can be programmed in absolute mode with AC. When they have other
meanings (e.g. pitch), the address modification is ignored.
5 Vocabulary word does not apply to SINUMERIK FM-NC/810D
6 Vocabulary word does not apply to SINUMERIK FM-NC/810D/NCU571
7 Vocabulary word does not apply to SINUMERIK 810D
8 The OEM user can incorporate two extra interpolation types and modify their names.
9 Vocabulary word applies only to SINUMERIK FM-NC
10 The extended address block format may not be used for these functions.
2
Name Meaning Value Description, Syntax Modal/ Group
assignment comment non-
modal
: Block number - main block (see N) 0 ... Special code for e.g. :20
9999 9999 blocks - instead of
integer N... ; this block
values only, should contain all
no sign instructions for a
following complete
machining section
A Axis Real m,s3
A2 5 Tool orientation: Euler angle Real s
A3 5 Tool orientation: Direction vector Real s
component
A4 5 Tool orientation for block beginning Real s
A5 5 Tool orientation for block end; Real s
Normal vector component
ABS Absolute value Real
AC Dimension input, absolute 0, ..., X=AC(100) s
359.9999°
ACC 5 Axial acceleration Real, m
without sign
ACN Absolute dimension setting for rotary axes, A=ACN(...) B=ACN(...) s
approach position in negative direction C=ACN(...)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-561
15 Tables 11.0215.1 List of instructions 15
ACP Absolute dimension setting for rotary axes, A=ACP(...) B=ACP(...) s
approach position in positive direction C=ACP(...)
ACOS Arc cosine (trigon. function) Real
ADIS Resurfacing distance for path functions G1, Real, without m
G2, G3, ... sign
ADISPOS Resurfacing distance for rapid traverse G0 Real, without m
sign
ADISPOSA Size of the tolerance window for IPOBRKA Integer, real, ADISPOSA=.. or m
ADISPOSA([,REAL])
ALF Angle lift fast Integer, m
without sign
AMIRROR Programmable mirroring (additive mirror) AMIRROR X0 Y0 Z0 s 3
; separate block
AND Logical AND
ANG Contour definition angle Real
AP Polar angle (Angle Polar) 30, ..., ± 360° m,s
APR Read/display access protection Integer,
(access protection read) without sign
APW Write access protection Integer,
(access protection write) without sign
AR Aperture angle (angle circular) 30, ..., 360° m,s
AROT Programmable rotation Rotation AROT X... Y... Z... s 3
(additive rotation) around 1st ;separate
geom. axis: AROT RPL= block
-180o .. 180°
2nd geom.
axis:
-89.999°
.. 90°
3rd geo. axis:
-180° .. 180°
AROTS programmable frame rotations with solid angles (additive AROT X... Y... s 3
rotation) AROT Z... X...
AROT Y... Z... ;own
AROT RPL= block
AS Macro definition String
ASCALE Programmable scaling (additive scale) ASCALE X... Y... Z... s 3
; separate block
ASIN Arc sine (trigon. function) Real
ASPLINE Akima spline m 1
ATAN2 Arc tangent 2 Real
ATRANS Additive programmable offset ATRANS X... Y... Z... s 3
(additive translation) ; separate block
AX Integer without sign Real m,s3
Siemens AG, 2002. All rights reserved
15-562 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.1 List of instructions 15
AXCSWAP Switch container axis AXCSWAP(CTn,CTn+1,...) 25
AXIS Data type: Axis name Name of file can be
added
AXNAME Converts the input string to an axis name String An alarm is
(get axname) generated if the
input string does
not contain a valid
axis name
AXSTRING Up to SW 5, axis identifier is converted to Up to SW 5 Name of file can AXSTRING( SPI(n) )
string (get axis as string) AXIS be added
With SW 6 and higher, the spindle number From SW 6
from SW 6
converts the string (get string) AXSTRING[ SPI(n) ]
string
B Axis Real m,s3
B_AND Bit AND
B_NOT Bit negation
B_OR Bit OR
B_XOR Bit exclusive OR
B2 5 Tool orientation: Real s
Euler angle
B3 5 Tool orientation: Real s
Direction vector component
B4 5 Tool orientation for block beginning Real s
B5 5 Tool orientation for block end; Real s
Normal vector component
BAUTO Definition of first spline segment by means of following 3 m 19
points (begin not a knot)
BLSYNC Processing of interrupt routine is only to start with the
next block change
BNAT 1 Natural transition to first spline block m 19
(begin natural)
BOOL Data type: Boolean value TRUE / FALSE or 0 / 1
BRISK 1 Brisk path acceleration m 21
BRISKA Activate brisk axis acceleration for the programmed axes
BSPLINE B spline m 1
BTAN Tangential transition to first spline block m 19
(begin tangential)
C Axis Real m,s3
C2 5 Tool orientation: Euler angle Real s
C3 5 Tool orientation: Real s
Direction vector component
C4 5 Tool orientation for block beginning Real s
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-563
15 Tables 11.0215.1 List of instructions 15
C5 5 Tool orientation for block end; Real s
Normal vector component
CAC Absolute approach of position Coded value is
(coded position: absolute coordinate) table index; table
value is
approached
CACN Absolute approach in negative direction of value stored in Permissible for
table. programming rotary
(coded position absolute negative) axes as positioning
axes
CACP Absolute approach in positive direction of value stored in
table.
(coded position absolute positive)
CALCDAT Calculate radius and center point or circle VAR Real The points must be
from 3 or 4 points [3] different.
(calculate circle data)
CALL Indirect subroutine call CALL PROGVAR
CALLPATH Programmable search path for subprogram calls A path can be CALLPATH(/_N_WKS
programmed to the _DIR/
existing NCK file _N_MYWPD/subprogram
system with _ID_SPF)
CALLPATH.
CANCEL Cancel modal synchronized action INT Cancel with
specified ID.
Without parameter:
All modal
synchronized
actions are
deselected.
CASE Conditional program branch
CDC Direct approach of position See CAC
(coded position: direct coordinate)
CDOF 1 Collision detection OFF m 23
CDON Collision detection ON m 23
CDOF2 Collision detection OFF For CUT3DC only m 23
CFC 1 Constant feed on contour m 16
CFIN Constant feed at internal radius only, m 16
not at external radius
CFTCP Constant feed at tool center point (center-point path) m 16
(constant feed in tool-center-point)
CHAN Specify validity range for data once per channel
Siemens AG, 2002. All rights reserved
15-564 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.1 List of instructions 15
CHANDATA Set channel number for channel data INT Only permissible in
access the initialization
module
CHAR Data type: ASCII character 0, ..., 255
CHF Chamfer; value = length of chamfer in Real, s
SW 3.5 direction of movement (chamfer) without sign
and higher Chamfer; value = length of chamfer
CHR
CHKDNO D number check
CIC Incremental approach of position See CAC
(coded position: incremental coordinate)
CIP Circular interpolation through intermediate points CIP X... Y... Z... m 1
I1=... J1=... K1=...
CLEARM Reset one/several markers for channel INT, Does not influence
coordination 1 - n machining in own
channel
CLGOF Const. workpiece speed for centerless grinding OFF
CLGON Const. workpiece speed for centerless grinding ON
CLRINT Deselect interrupt: INT Parameter:
Interrupt number
CMIRROR Mirror on a coordinate axis FRAME
COARSEA Motion end when "Exact stop coarse" reached COARSEA=.. or m
COARSEA[n]=..
1,6
COMPOF Compressor OFF m 30
6
COMPON Compressor ON m 30
COMPCURV Compressor ON constant curve polynomials m 30
COMPCAD Compressor ON optimized surface finish m 30
CONTPRON Activate contour preparation (contour preparation ON) m 49
COS Cosine (trigon. function) Real
COUPDEF Definition ELG group / synchronous spindle String Block change (soft-
group ware) response:
(couple definition) NOC: no software
control,
FINE/COARSE:
software on ”Syn-
chronization fine /
coarse”,
IPOSTOP: software
on setpoint-depen-
dent termination of
overlaid movement
COUPDEL Delete ELG group (couple delete)
COUPOF ELG group / synchronous spindle pair OFF (couple OFF)
COUPON ELG group / synchronous spindle pair ON (couple ON)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-565
15 Tables 11.0215.1 List of instructions 15
COUPRE Reset ELG group Programmed
S (couple reset) values invalid;
machine data
values valid
CP Path movement (continuous path) m 49
CPRECOF Programmable contour precision OFF m 39
1,6
6
CPRECON Programmable contour precision ON m 39
CPROT Channel-specific protection zone ON/OFF
CPROTDEF Channel specific protection area definition
CR Circle radius Real, s
without sign
CROT Rotation of the current coordinate system. FRAME Maximum number
of parameters: 6
CROTS programmable frame rotations with solid angles (rotations CROT X... Y... s
in the indicated axes) CROT Z... X...
CROT Y... Z... ;own
CROT RPL= block
CSCALE Scale factor for multiple axes. FRAME Maximum number
of parameters: 2 *
axis numbermax
CSPLINE Cubic spline m 1
CTAB Define following axis position according to Real If parameter 4/5
leading axis position from curve table not programmed:
Standard scaling
CTABDEF Table definition ON
CTABDEL Clear curve table
CTABEND Table definition OFF
CTABINV Define leading axis position according to Real See CTAB
following axis position from curve table
CT Circle with tangential transition CT X... Y.... Z... m 1
CTRANS Zero offset for multiple axes FRAME Max. of 8 axes
CUT2D 1 2 ½D tool offset (cutter compensation type m 22
2-dimensional)
CUT2DF 2 ½D tool offset (cutter compensation type 2-dimensional m 22
frame); The tool offset acts in relation to the current frame
(inclined plane)
CUT3DC 5 3D cutter compensation type 3-dimensional m 22
circumference milling
5
CUT3DCC Cutter compensation type 3-dimensional circumference m 22
milling with limit surfaces
Siemens AG, 2002. All rights reserved
15-566 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.1 List of instructions 15
CUT3DCCD Cutter compensation type 3-dimensional circumference m 22
5
milling with limit surfaces with differential tool
CUT3DF 5 3D tool offset face milling (cutter compensation type m 22
3-dimensional face)
5
CUT3DFF 3D tool offset face milling with constant tool orientation as m 22
a function of active frame (cutter compensation type
3-dimensional face frame)
5
CUT3DFS 3D tool offset face milling with constant tool orientation m 22
irrespective of active frame (cutter compensation type
3-dimensional face frame)
CUTCONO1 Constant radius compensation OFF m 40
CUTCONON Constant radius compensation ON m 40
D Tool offset number 1, ..., 9 includes D...
compensation data
SW 3.5 and for a certain tool
higher T... ; D0 →
1, ... 32 000 compensation
values for a tool
DC Absolute dimension setting for rotary axes, A=DC(...) B=DC(...) s
approach position directly C=DC(...)
SPOS=DC(...)
DEF Variable definition Integer,
without sign
DEFAULT Branch in CASE branch Jump to if
expression does
not fulfill any of the
specified values
DEFINE Define macro
DELDTG Delete distance-to-go
DELT Delete tool Duplo number can
be omitted
DIAMCYOF Radius programming for G90/91: ON. The G-code of this Radius pro- m 29
group that was last active remains active for display gramming last
active G-code
DIAMOF1 Diametral programming: OFF Radius pro- m 29
gramming for
G90/G91
DIAMON Diametral programming: ON Diameter progr. for m 29
G90/G91
DIAM90 Diameter program for G90, radius progr. for G91 m 29
DILF Rapid lift length m
DISABLE Interrupt OFF
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-567
15 Tables 11.0215.1 List of instructions 15
DISC Transition circle overshoot in tool radius 0, ..., 100 m
compensation
DISPLOF Suppress current block display
(display OFF)
DISPR Distance path for repositioning Real, s
without sign
DISR Distance for repositioning Real, s
without sign
DITE Thread run-out path Real m
DITS Thread run-in path Real m
DIV Integer division
DL Tool sum compensation INT m
DRFOF Deactivate the handwheel offsets (DRF) m
DRIVE 9 Velocity-dependent path acceleration m 21
DRIVEA Switch on bent acceleration characteristic curve for the
programmed axes
DZERO Set D number of all tools of the TO unit assigned to the
channel invalid
EAUTO Definition of last spline segment by last 3 points (end not m 20
a knot)
EGDEF Definition of an electronic gear for 1 following axis
(Electronic gear define) with up to 5
leading axes
EGDEL Delete coupling definition for the following axis Triggers
(Electronic gear delete) preprocessing stop
EGOFC Switch off electronic gear continuous
(Electronic gear OFF continuous)
EGOFS Switch off electronic gear selectively
(Electronic gear OFF selective)
EGON Switch on electronic gear without
(electronic gear ON) synchronization
EGONSYN Switch on electronic gear with
(electronic gear ON synchronized) synchronization
EGONSYN Switch on electronic gearing, stating approach mode with
E (electronic gear ON synchronized) synchronization
ELSE Program branch, if IF condition not fulfilled
ENABLE Interrupt ON
ENAT 1,7 Natural curve transition to next traversing block m 20
(end natural)
ENDFOR End line of FOR counter loop
ENDIF End line of IF branch
ENDLOOP End line of endless program loop LOOP
Siemens AG, 2002. All rights reserved
15-568 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.1 List of instructions 15
ENDPROC End line of program with start line PROC
ENDWHILE End line of WHILE loop
ETAN Tangential curve transition to next traversing block at m 20
beginning of spline (end tangential)
EVERY Execute synchronized action if condition changes from
FALSE to TRUE
EXECSTR Transfer of a string variable with the parts program line to Indirect parts EXECSTRING(MFCT1
ING run program line address programmed as incremental
bit = 0 -> address programmed as absolute
$C_TYP_PROG INT $C_TYP_PROG R W 6
Bit pattern of all the programmed addresses with the value INT .
or REAL 4
bit0 = address "A" .... bit25 = address "Z"
Bit = 1 -> address programmed with real value
Bit = 0 -> address programmed with int value
$C_I_NUM INT $C_I_NUM R W 6
$C_I_NUM contains the number of I addresses programmed in .
the block. 1
For cycle programming, this value is always 1 whenever bit 0 in
$C_I_PROG is set.
In the case of macro programming with G65/G66, this contains
the number of "I" addresses programmed in the block, (max.
10).
$C_J_NUM INT $C_J_NUM R W 6
$C_J_NUM contains the number of "J" addresses programmed .
in the block. 1
For cycle programming, this value is always 1 whenever bit 0 in
$C_J_PROG is set.
In the case of macro programming with G65/G66, this contains
the number of "J" addresses programmed in the block, (max.
10).
$C_K_NUM INT $C_K_NUM R W 6
$C_K_NUM contains the number of I addresses programmed in .
the block. 1
For cycle programming, this value is always 1 whenever bit 0 in
$C_K_PROG is set.
In the case of macro programming with G65/G66, this contains
the number of "K" addresses programmed in the block, (max.
10).
Siemens AG, 2002. All rights reserved
15-634 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$C_I_ORDER INT $C_I_ORDER[] R W 6
Number of the IJK block, in which I has been programmed .
For macro programming with G65/G66, up to 10 entries are 4
possible in the block with address I. These can be used to
evaluate the IJK sequence. A note is always made of which IJK
go together.
$C_J_ORDER INT $C_J_ORDER[] R W 6
Number of the IJK block, in which J has been programmed .
For macro programming with G65/G66, up to 10 entries are 4
possible in the block with address J. These can be used to
evaluate the IJK sequence.
from the parts program. A note is always made of which IJK go
together.
$C_K_ORDER INT $C_K_ORDER[] R W 6
Number of the IJK block, in which K has been programmed .
For macro programming with G65/G66, up to 10 entries are 4
possible in the block with address K. These can be used to
evaluate the IJK sequence from the parts program. A note is
always made of which IJK go together.
$C_ME INT $C_ME R W 6
Address extension for address M in the case of a subroutine .
call by M function 1
$C_TE INT $C_TE R W 6
Address extension for address T in the case of a subroutine call .
by T function 1
$C_MACPAR REAL $MAC_PAR[n] R W 6
Macro variable in ISO2/3 mode programmed in the original .
program with 3
#
The max. number of ISO macro parameters is 33
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-635
15 Tables 11.0215.2 List of system variables 15
15.2.23 System data
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AN_SETUP_ REAL IF $AN_SETUP_TIME > 60000 GOTOF MARK01 RS WS R W 6
TIME Time since last power up of control with default values .
(in minutes) 1
$AN_POWERON_ REAL IF $AN_POWERON_TIME == 480 GOTOF MARK02 RS WS R W 6
TIME Time since last power-on of control .
(in minutes) 1
$AN_NCK_VER REAL NCK version: RS R 6
SION NCK version: only the part of the floating-point number prior .
to the decimal point is evaluated, the part after the decimal 1
point can contain identification for intermediate states within
development. The part prior to the decimal point contains
the official software version identifier of the NCK: For
example, if 20.00.00 is for the NCK version,
the value of the variable is 200000.0
compare OPI N/Y nckVersion
15.2.24 Frames 2
$P_UBFR FRAME $P_UBFR R W 4
1st base frame in channel activated after G500, G54..G599.
Corresponds to $P_CHBFR[0].
Axes: (geometry axis, channel axis, machine axis)
$P_SETFRAME FRAME $P_SETFRAME R W 6
Current system frame for preset actual value memory and .
scratching. 1
Axes: (geometry axis, channel axis, machine axis)
$P_EXTFRAME FRAME $P_EXTFRAME R W 6
Current system frame for zero offset external. .
Axes: (geometry axis, channel axis, machine axis) 1
$P_PARTFRAME FRAME $P_PARTFRAME R 6
Current system frame for TCARR and PAROT. .
Axes: (geometry axis, channel axis, machine axis) 1
$P_TOOLFRAME FRAME $P_TOOLFRAME R 6
Current system frame for TOROT and TOFRAME. .
Axes: (geometry axis, channel axis, machine axis) 1
$P_WPFRAME FRAME $P_WPFRAME R W 6
Current system frame for part reference points. .
Axes: (geometry axis, channel axis, machine axis) 3
$P_CYCFRAME FRAME $P_CYCFRAME R W 6
Current system frame for cycles. .
Axes: (geometry axis, channel axis, machine axis) 3
Siemens AG, 2002. All rights reserved
15-636 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_CHBFRAME FRAME $P_CHBFRAME[n] R W 5
Current base frames in the channel.
Configurable via MD $MC_MM_NUM_BASE_FRAMES. The
dimension is checked on variable access.
Axes: (geometry axis, channel axis, machine axis)
$P_NCBFRAME FRAME $P_NCBFRAME[n] R W 5
Current NCU base frames.
Configurable via MD
$MN_MM_NUM_GLOBAL_BASE_FRAMES.
The dimension is checked on variable access.
Axes: (geometry axis, channel axis, machine axis)
$P_ACTBFRAME FRAME $P_ACTBFRAME R 5
Current chained total basic frame
Axes: (geometry axis, channel axis, machine axis)
$P_BFRAME FRAME $P_BFRAME R W 4
Current 1st base frame in the channel. Corresponds to
$P_CHBFRAME[0].
Axes: (geometry axis, channel axis, machine axis)
$P_IFRAME FRAME $P_IFRAME R W 2
Current settable frame
Axes: (geometry axis, channel axis, machine axis)
$P_PFRAME FRAME $P_PFRAME R W 2
Current programmable frame
Axes: (geometry axis, channel axis, machine axis)
$P_ACTFRAME FRAME $P_ACTFRAME R 2
Current total frame
Axes: (geometry axis, channel axis, machine axis)
$P_UIFRNUM INT $P_UIFRNUM R 2
Number of the active $P_UIFR
$P_NCBFRMASK INT $P_NCBFRMASK R W 5
Bit screenform is used for definition of the NCU global base
frames that are included in the calculation of the total base
frame.
$P_CHBFRMASK INT $P_CHBFRMASK R W 5
Bit screenform is used for definition of channel-specific base
frames that are included in the calculation of the total base
frame.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-637
15 Tables 11.0215.2 List of system variables 15
15.2.25 Tool data
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_AD REAL $P_AD[n] R W 2
Active tool offsets
n: Parameter number 1–31
n = 1-25 $TC_DP1 to $TC_DP25
n = 26 $TC_DPCE
n = 27 $TC_DPH
n = 28 $TC_DPV
n = 29 $TC_DPV3
n = 30 $TC_DPV4
n = 31 $TC_DPV5
$P_ADT REAL $P_ADT[n] R W 6
With an active tool adapter, the transformed compensation .
values of the tool adapter transformation are returned when 1
reading the values tool compensations are transformed
n: Parameter number 1–31
n = 1-25 $TC_DP1 to $TC_DP25
n = 26 $TC_DPCE
n = 27 $TC_DPH
n = 28 $TC_DPV
n = 29 $TC_DPV3
n = 30 $TC_DPV4
n = 31 $TC_DPV5
$P_DLNO INT $P_DLNO R 6
Active cumulative compensation number DL=0 - DL='max.'; .
'max'= value of 1
$MN_MM_MAX_SUMCORR_PER_CUTTEDGE
$P_TOOL INT $P_TOOL R 2
Active tool cutting edge D0 - D'max.'; 'max'= value of
$MN_MM_MAX_CUTTING_EDGE_NO
Siemens AG, 2002. All rights reserved
15-638 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_TOOLNO INT $P_TOOLNO R 2
Active tool number T0 - T32000; with active function 'flat D
number' T can have 8 digits
The command should generally not be used when magazine
management is active.
When magazine management is active, GETEXET should be
used instead.
(The programming is only ever reliable in a situation where
$MC_CUTTING_EDGE_DEFAULT=-1, > 0 applies.
The wrong tool number can be determined for
$MC_CUTTING_EDGE_DEFAULT=0, or =-2.
If programming takes place after programming D > 0, it is also
always reliable.
NOTICE: Especially for $MC_CUTTING_EDGE_DEFAULT=-
2, $P_TOOLNO
(the tool no. of the active tool with which the currently
effective D offset was being calculated) and GETEXET (the
changed tool) can return different tool numbers.
->also see $P_MTHSDC and documentation on the topic of
more than one tool holder/spindle.
$P_TOOLP INT $P_TOOLP R 6
Last programmed tool number T0 - T32000 (for operation .
without magazine management). 1
The command cannot be used when magazine management
is active.
When magazine management is active, GETSELT must be
used instead.
$P_TOOLL REAL $P_TOOLL[n] R 2
Active total tool length
n: Length 1–3
$P_TOOLO REAL $P_TOOLO[n] R 6
Active tool orientation. .
n: Component 1–3 1
$AC_TOOLO_A REAL $AC_TOOLO_ACT[n] RS R 6
CT Active setpoint orientation. .
n: Component 1–3 4
$AC_TOOLO_E REAL $AC_TOOLO_END[n] RS R 6
ND End orientation of the active block .
n: Component 1–3 4
$AC_TOOLO_DI REAL $AC_TOOLO_DIFF RS R 6
FF Residual angle of tool orientation in the active block .
4
$VC_TOOLO REAL $VC_TOOLO[n] RS R 6
Actual orientation .
n: Component 1–3 4
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-639
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$VC_TOOLO_DI REAL $VC_TOOLO_DIFF RS R 6
FF Angle between setpoint orientation and actual orientation .
4
$VC_TOOLO_S INT $VC_TOOLO_STAT RS R 6
TAT Status of the calculation of actual orientation .
4
$P_TC INT $P_TC R 6
Active tool carrier .
1
$AC_TC INT $AC_TC RS R 6
Active tool carrier .
4
$P_TCANG REAL $P_TCANG[n] R 5
Active angle of toolholder axis
n: Angle 1–2
$P_TCDIFF REAL $P_TCDIFF[n] R 6
The difference between the calculated and the used angle of .
a toolholder axis when incrementing (Hirth tooth system) the 1
angle
n: Angle 1–2
$P_TCSOL INT $P_TCSOL R 6
Number of solutions when specifying the axis of rotation angle .
of an orientable toolholder from a frame 1
With 0 to 2 solutions, the corresponding value
is returned.
With an infinite number of solutions, the return value is 3.
If the angles are specified (TCOABS), the number of solutions
is always 1.
$P_TCSTAT INT $P_TCSTAT R 6
Specifies the status of an orientable toolholder. .
The variable is bit-coded with the following significance: 4
0x1 The first rotary axis is available
0x2 The second rotary axis is available
0x4 The angles used for the calculation
come from an orientation in the frame direction
0x8 The angles used for the calculation
have been specified as absolute
0x10 The pole axis angle is indeterminate for
orientation in the frame direction
0x1000 Only the tool can be rotated (kinematics type T)
0x2000 Only the workpiece can be rotated (kinematics type
P)
0x4000 Tool and workpiece can be rotated
(kinematics type M)
Bits not designated here are currently unassigned.
$P_TOOLR REAL $P_TOOLR R 2
Active tool radius (total)
Siemens AG, 2002. All rights reserved
15-640 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_TOOLND INT $P_TOOLND[t] R 4
Number of cutting edges of tool t
t: Tool number 1–32000
$P_TOOLEXIST BOOL $P_TOOLEXIST[t] R 4
Tool with T No. t exists
t: Tool number 1–32000
$P_D INT $P_D R 6
Current D number in ISO_2-language mode .
1
$P_H INT $P_H R 6
Current H number in ISO_2-language mode .
1
$A_TOOLMN INT $A_TOOLMN[t] R 4
Magazine number of tool t
t: Tool number 1–32000
$A_TOOLMLN INT $A_TOOLMLN[t] R 4
Magazine location number of tool t
t: Tool number 1–32000
$A_MYMN INT $A_MYMN[t] R 6
Owner magazine number of the tool with T number t. .
Result value = 0 = tool is not loaded (if $A_TOOLMN 1
> 0, then
manual tool).
Result value = -1 = tool management is not active
Result value = -2 = tool with T number t does not exist.
t: Tool number 1–32000
$A_MYMLN INT $A_MYMLN[t] R 6
Owner magazine location number of the tool with T number t. .
Result value = 0 = tool is not loaded (if $A_TOOLMLN > 0, 1
then
manual tool).
Result value = -1 = tool management is not active
Result value = -2 = tool with T number t does not exist.
t: Tool number 1–32000
$A_MONIFACT REAL $A_MONIFACT R WS R W 4
Factor for tool length monitoring
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-641
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_TOOLNG INT $P_TOOLNG R 6
Number of defined tool groups assigned to the channel .
OPI module type = TM 1
$P_TOOLNT INT $P_TOOLNT R 6
Number of defined tools assigned to the channel .
OPI module type = TV 1
$P_TOOLT INT $P_TOOLT[i] R 6
i-th tool number T .
OPI module type = TV 1
i= 1,..., $P_TOOLNT
$P_TOOLD INT $P_TOOLD[t,i] R 6
i-th D-no of the tool with T number t; i=1,2... .
if t is the value of a non-defined tool, -2 is returned 1
If i is a value outside the permitted range, 0 is returned.
OPI module type = TO
t = 1, ...., 32000
i = 1,......., $P_TOOLND
$P_USEKT INT $P_USEKT (= USE Kind of Tool) R W 6
Is a bit-coded value .
All the tools whose parameter $TC_TP11 has set one of the bits 1
of $P_USEKT,
are available to the following tool changes. The value zero
has the same content
as 'all bits set'
OPI module = C/S
$P_TOOLNDL INT $P_TOOLNDL[t,d] R 6
Number of DL offsets of the D offset given by T number t and .
D number d 1
>0 Number of DL offsets
0 no DL offset for this D offset
-1 sum offset function not active
-2 t is the value of a non-defined tool
-3 d is the value of a non-defined D offset
OPI module type = TO memory; TO unit
t = 1, ...., 32000
d = 1,......., 32000
Siemens AG, 2002. All rights reserved
15-642 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
15.2.26 Magazines
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_MAGN INT $P_MAGN R 6
Number of defined magazines assigned to the channel .
> 0 successful read access 1
0 no magazines defined
-1 TMMG not active
OPI module = TM
$P_MAG INT $P_MAG[ i ] R 6
i-th magazine number .
> 0 successful read access 1
0 i is outside the permitted range
-1 TMMG not active
OPI module = TM
i= 1,..., $P_MAGN
$P_MAGNDIS INT P_MAGNDIS[ n, m ] R 6
Number of magazines interconnected with location m of the .
internal magazine n. 1
> 0 successful read access
0 no magazine interconnected with the buffer location
-1 TMMG not active
-2 n is not the number of an internal magazine
-3 m is not the number of an internal magazine location
OPI module = TPM
n= must be the number of the buffer magazine or of the
loading magazine
m= 1,..., max. number of a location in the internal magazine
mentioned
$P_MAGDISS INT P_MAGDISS[ l, i ] R 6
Number of the i-th magazine interconnected with location l .
of the buffer magazine. 1
> 0 successful read access
0 i is outside the permitted range
-1 TMMG not active
-2 m is not the number of a buffer location
-3 no buffer magazine defined
OPI module = TPM
l= 1,..., max. number of a location in the buffer magazine
i= 1,..., $P_MAGNDIS[ no. of the buffer magazine, refLoc ]
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-643
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_MAGDISL INT P_MAGDISL[ l, i ] R 6
Number of the i-th magazine interconnected with location l of .
the loading magazine. 1
> 0 successful read access
0 i is outside the permitted range
-1 TMMG not active
-2 m is not the number of a loading magazine location
-3 no loading magazine defined
OPI module = TPM
l= 1,..., max. number of a location in the loading magazine
i= 1,..., $P_MAGNDIS[ no. of the loading magazine, refLoc ]
$P_MAGNS INT $P_MAGNS R 6
Number of spindle locations / toolholder locations in the buffer .
assigned to the channel. 1
> 0 successful read access
0 no spindle locations defined
-1 TMMG not active
-3 no buffer magazine defined
$P_MAGS INT $P_MAGS[ n ] R 6
nth number of the spindle / of the toolholder in the buffer .
> 0 successful read access 1
0 n is outside the permitted range
-1 TMMG not active
-3 no buffer magazine defined
n= 1,..., max. toolholder number
$P_MAGNREL INT $P_MAGNREL[ n ] R 6
Number of the buffer assigned to the spindle number / .
toolholder number n 1
> 0 successful read access
0 spindle location has no buffer location assigned
-1 TMMG not active
-2 n is not the number of a spindle location
-3 no buffer magazine defined
n= 1,..., max. toolholder number
$P_MAGREL INT P_MAGREL[ n, m ] R 6
m-th buffer number of the n-th spindle number / toolholder .
number 1
> 0 successful read access
0 m is outside the permitted range
-1 TMMG not active
-2 n is not the number of a spindle location
-3 no buffer magazine defined
n= 1,..., max. toolholder number
m= 1,..., $P_MAGNREL
Siemens AG, 2002. All rights reserved
15-644 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_MAGNH INT $P_MAGNH R 6
Number of defined magazine location type hierarchies assigned .
to the channel. 1
> 0 successful read access
0 no location type hierarchies are defined
-1 TMMG not active
OPI module = TT
$P_MAGNHLT INT $P_MAGNHLT[ n ] R 6
Number of defined location types in the nth defined hierarchy .
> 0 successful read access 1
0 n is outside the defined range
-1 TMMG not active
OPI module = TT
n= 1,..., $P_MAGNH
$P_MAGHLT INT P_MAGHLT[ n, m ] R 6
m-th location type of hierarchy n; n= 1,..., $P_MAGNH; m= 1,..., .
$P_MAGNHLT 1
> 0 successful read access
0 m is outside the defined range
-1 TMMG not active
-2 hierarchy n has no defined location types
OPI module = TT
n= 1,..., $P_MAGNH
m= 1,..., $P_MAGNHLT
$P_MAGNA INT $P_MAGNA R 6
Number of defined adapters assigned to the channel .
> 0 successful read access 1
0 no adapters defined
-1 TMMG or 'Adapter' function not active
OPI module = AD
$P_MAGA INT $P_MAGA[ i ] R 6
i-th adapter number .
> 0 successful read access 1
0 i is outside the permitted range
-1 TMMG or 'Adapter' function not active
OPI module = AD
i= 1,..., $P_MAGNA
$P_MTHSDC INT $P_MTHSDC R 6
Master toolholder no. or master spindle no. relative to that of the .
active tool 4
for
which the next D offset selection is specified.
> 0 successful read access
0 No master toolholder or master spindle available.
The next D offset works with T0.
-1 TMMG not available
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-645
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_MONMIN REAL $AC_MONMIN R WS R W 6
Ratio between tool monitoring actual value and setpoint. .
Threshold for tool search strategy "load only tools 1
with actual value greater than threshold"
$P_VDITCP INT $P_VDITCP[n] R W 2
Available parameters for magazine management on VDI
interface
n: Index 1–3
$A_DNO INT $A_DNO[i] R 4
Read a D number defined by the PLC via VDI interface
i: Index 1–9 for table location in D number table
$P_ATPG REAL $P_ATPG[n] R W 2
Current tool-related grinding data
n: Parameter number 1–9
$P_TOOLENV STRING $P_TOOLENV[i] R 6
Returns the name of the tool environment stored under .
(internal) 3
index i. If i refers to a non-defined data block, the zero string
is returned.
If index i is invalid, in other words, if i is less than 1 or more
than the maximum number of data blocks for tool
environments
($MN_MM_NUM_TOOLENV), an alarm is output.
A maximum number of tool environments is configurable via
MD $MN_MM_NUM_TOOLENV.
2nd dimension for TYPE_STRING is automatically
MAXSTRINGLEN
$P_TOOLENVN INT $P_TOOLENVN R 6
Indicates the number of defined data blocks for describing .
tool environments. 3
$P_AP REAL $P_AP R 6
Programmed angle for polar coordinates .
1
15.2.27 Programmed geometry axis values
$P_AXN1 AXIS $P_AXN1 R 3
Current address of the geometry axis - abscissa
$P_AXN2 AXIS $P_AXN2 R 3
Current address of the geometry axis - ordinate
Siemens AG, 2002. All rights reserved
15-646 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_AXN3 AXIS $P_AXN3 R 3
Current address of the geometry axis - applicate
$P_ACTGEOAX AXIS $P_ACTGEOAX[1] R 4
Current geometry axis assignment, dependent on plane
Returns the current geometry axis assignment programmed
with
geometry axis(1,X,2,Y,3,Z)
Array index 1–3 for 1st to 3rd geometry axis
n: Number of input 1 - ...
15.2.28 G groups
$P_GG INT $P_GG[n] R 2
Current G function of a G group (index as PLC interface)
n: Number of the G group
$P_EXTGG INT $P_EXTGG[n] R 5
Can only be used in Siemens mode:
Current G function of a G group with external NC languages
(index as PLC interface)
n: Number of the G group
$A_GG INT $A_GG[n] R 5
Read current G function of a G group from SA (index like PLC
interface)
n: Number of the G group
15.2.29 Programmed values
$P_SEARCH BOOL $P_SEARCH R 2
Block search is active if TRUE (1)
$P_SEARCH1 BOOL $P_SEARCH1 R 2
Block search with calculation is active if TRUE (1)
$P_SEARCH2 BOOL $P_SEARCH2 R 2
The last selected search type was block search without
calculation, if
TRUE (1)
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-647
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_SEARCHL INT R1 = $P_SEARCHL R 5
Returns the last selected search type:
(coding analogous to PI service _N_FINDBL)
0 : No block search
1 : Block search without calculation
2 : Block search with calculation on contour
3 : Reserved
4 : Block search with calculation at end of block position
5 : Block search in extended program test
$P_SUBPAR BOOL $P_SUBPAR[n] R 5
Query whether during subroutine call with parameter transfer
parameter n
was actually programmed (TRUE) or whether the system has
set a default parameter (FALSE).
n: Parameter number 1 to n corresponding to the definition in
the PROC instruction
$P_CTABDEF BOOL $P_CTABDEF R 4
Definition of curve tables is active if TRUE (1)
$P_MC INT $P_MC R 2
Status of modal subprogram call
FALSE (0) -> Subprogram call not modal
TRUE (1) -> Subprogram call modal
$P_REPINF INT $P_REPINF R 4
Status info for repositioning with REPOS command
(0) -> Repositioning with REPOS not possible for following
reasons
- Call is not executed in an ASUB
- Call is executed in an ASUB, which was started in the reset
state JOG mode
- Call is executed in an ASUB, which was started in
JOG mode
(1) -> Repositioning with REPOS possible
$P_SIM BOOL $P_SIM R 2
Simulation runs if TRUE (1)
Siemens AG, 2002. All rights reserved
15-648 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_DRYRUN BOOL $P_DRYRUN R 2
Dry run on if TRUE, else FALSE
$P_OFFN REAL $P_OFFN R 5
Programmed offset contour normal .
1
$PI REAL $PI R 2
Circle constant PI = 3.1415927
$P_PROG_EVE INT The system variable $P_PROG_EVENT can be used to query R 6
NT whether the program was implicitly activated by an event .
configured by $MC_PROG_EVENT_MASK or by 1
$MN_SEARCH_RUN_MODE. $P_PROG_EVENT returns an
integer value between 0 and 5 with the following significance:
0 : explicit activation via NC Start or ASUB Start over the
VDI or ASUB interface
1 : Implicit activation via event "Parts program start”
2 : Implicit activation via event "Parts program end"
3 : Implicit activation via event "Operator panel front reset"
4 : Implicit activation via event "Booting"
5 : Implicit activation subsequent to last action block display
after block search
$P_PROGPATH STRING PCALL ($P_PROGPATH deflected
n: Number of probe
$AC_MEA INT $AC_MEA[n] R 2
Probe has been triggered if TRUE (1)
n: Number of probe
1 - MAXNUM_PROBE
$AC_TRAFO INT $AC_TRAFO RS R 3
Code number of the active transformation
corresponding to machine data $MC_TRAFO_TYPE_n
$P_TRAFO INT $P_TRAFO R 6
Code number of the programmed transformation .
corresponding to machine data $MC_TRAFO_TYPE_n 1
$AC_TRAFO_P REAL $AC_TRAFO_PAR[n] RS R 6
AR Parameter of the active transformation .
n: Number of the parameter 1
$P_TRAFO_PAR REAL $P_TRAFO_PAR[n] R 6
Parameter of the programmed transformation .
n: Number of the parameter 1
$AC_TRAFO_P INT $AC_TRAFO_PARSET RS R 6
ARSET Number of the active transformation record .
Variable is '0' if no transformer active 3
$P_TRAFO_PA INT $P_TRAFO_PARSET R 6
RSET Number of the programmed transformation record .
Variable is '0' if no transformer active 3
$AC_LIFTFAST INT $AC_LIFTFAST RS WS R W 4
Information about execution of liftfast.
0: Initial state.
1: Liftfast has been executed.
At the start of the liftfast operation, the NC sets the value
of the variable internally to "1".
The evaluating program (if available) must reset the variable
to its initial setting ($AC_LIFTFAST=0) to enable a
subsequent liftfast to be detected.
Siemens AG, 2002. All rights reserved
15-652 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$P_LIFTFAST INT $P_LIFTFAST R 6
Information about execution of liftfast. .
0: Initial state. 3
1: Liftfast has been executed.
At the start of the liftfast operation, the NC sets the value
of the variable internally to "1".
The evaluating program (if available) must reset the variable
to its initial setting to enable a subsequent liftfast to be
detected.
The reset is initiated by writing $AC_LIFTFAST!
$AC_ASUB INT $AC_ASUB RS R 4
Code number for the cause of the ASUB activation. The
reasons are bit-coded and have the following significance:
BIT0:
Activation due to: User interrupt "ASUB with Blsync"
Activation by: VDI signal, digital/analog interface
Continuation by: user-selectable Reorg or Ret
BIT1:
Activation due to: User interrupt "ASUB"
For program continuation with Repos, the position, after
which the stop occurred is stored.
Activation by: VDI signal, digital/analog interface
Continuation by: user-selectable
BIT2:
Activation due to: User interrupt "ASUB from Ready channel
status"
Activation by: VDI signal, digital/analog interface
Continuation by: user-selectable
BIT3:
Activation due to: User interrupt "ASUB not READY
in a manual mode and channel status"
Activation by: VDI signal, digital/analog interface
Continuation by: user-selectable
BIT4:
Activation due to: Activation due to: User interrupt "ASUB"
For program continuation with Repos, the actual position
when the interrupt occurred is stored.
Activation by: VDI signal, digital/analog interface
Continuation by: user-selectable
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-653
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_ASUB INT BIT5: RS R 4
(continuation) Activation due to: Cancelation of subprogram repetition
Activation by: VDI signal
Continuation by: using system ASUB REPOS
BIT6:
Activation due to: Activation of decoding single block
Activation by: VDI signal (+OPI)
Continuation by: using system ASUB REPOS
BIT7:
Activation due to: Activation of delete distance to go
Activation by: VDI signal
Continuation by: using system ASUB Ret
BIT8:
Activation due to: Activation of axis synchronization
Activation by: VDI signal
Continuation by: using system ASUB REPOS
BIT9:
Activation due to: Mode change
Activation by: VDI signal
Continuation by: using system ASUB REPOS or RET
(see MD.)
BIT10:
Activation due to: Program continuation with teach-in or
after teach-in deactivation
Activation by: VDI signal
Continuation by: using system ASUB Ret
BIT11:
Activation due to: Overstore selection
Activation by: Pi selection
Continuation by: using system ASUB REPOS
BIT12:
Activation due to: Alarm with reaction of compensation
block with Repos (COMPBLOCKWITHREORG)
Activation by: Internal
Continuation by: using system ASUB REPOS
BIT13:
Activation due to: Retraction movement on G33 and Stop
Activation by: Internal
Continuation by: using system ASUB Ret
BIT14:
Activation due to: Activation of dry run feedrate
Activation by: VDI
Continuation by: using system ASUB REPOS
BIT15:
Activation due to: Deactivation of dry run feedrate
Activation by: VDI
Continuation by: using system ASUB REPOS
Siemens AG, 2002. All rights reserved
15-654 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
ASUB BIT16: RS R 4
(continuation) Activation due to: Activation of block suppression
Activation by: VDI
Continuation by: using system ASUB REPOS
BIT17:
Activation due to: Deactivation of block suppression
Activation by: VDI
Continuation by: using system ASUB REPOS
BIT18:
Activation due to: Set machine data active
Activation by: Pi
Continuation by: using system ASUB REPOS
BIT19:
Activation due to: Set tool offset active
Activation by: Pi "_N_SETUDT"
Continuation by: using system ASUB REPOS
BIT20:
Activation due to: System ASUB after search type
SERUPRO has reached the search target.
Activation by: Pi "_N_FINDBL" Parameter == 5
Continuation by: using system ASUB REPOS
$P_ISTEST BOOL $P_ISTEST R 4
Check test mode in parts program
TRUE = Program test active
FALSE = Program test not active
$P_MMCA STRING $P_MMCA R W 2
MMC task acknowledgment
2nd dimension for TYPE_STRING is automatically
MAXSTRINGLEN
$A_PROTO BOOL $A_PROTO RS WS R W 4
Activate / disable Logging function for the first user
$A_PROTOC BOOL $A_PROTOC RS WS R W 6
Activate / disable Logging function for a user .
0–9, USER 1
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-655
15 Tables 11.0215.2 List of system variables 15
15.2.31 Synchronized actions
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_FIFO1 REAL $AC_FIFO1[n] RS W R W + 4
FIFO for motion-synchronized actions and cyclic
measurements
n: Parameter number 0 - max. FIFO element
Special meaning:
n=0: On write accesses with index 0, a new value is stored
in the FIFO,
On read accesses with index 0, the oldest element is
read and deleted from the FIFO
n=1: Read access to oldest element
n=2: Read access to latest element
n=3: Sum of all the elements located in the FIFO when in MD
$MC_MM_MODE_FIFO, bit0 is set
n=4: Read access to current number of FIFO elements
n=5-m: Read access to individual FIFO elements
5 is the oldest element
6 is the second-oldest, etc.
$AC_FIFO2 REAL $AC_FIFO2[n] RS W R W + 4
FIFO for motion-synchronized actions and cyclic
measurements
n: Parameter number 0 - max. FIFO element
Special meaning:
n=0: On write accesses with index 0, a new value is stored
in the FIFO,
On read accesses with index 0, the oldest element is
read and deleted from the FIFO
n=1: Read access to oldest element
n=2: Read access to latest element
n=3: Sum of all the elements located in the FIFO when in MD
$MC_MM_MODE_FIFO, bit0 is set
n=4: Read access to current number of FIFO elements
n=5-m: Read access to individual FIFO elements
5 is the oldest element
6 is the second-oldest, etc.
...
$AC_FIFO10 REAL $AC_FIFO10[n] RS W R W + 4
as $AC_FIFO01 ...
Siemens AG, 2002. All rights reserved
15-656 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
15.2.32 I/Os
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$A_IN BOOL $A_IN[n] RS R 2
Digital input NC
n: Number of input 1 - ...
The max. input number results from MD
$MN_FASTIO_DIG_NUM_INPUTS
$A_OUT BOOL $A_OUT[n] RS W R W 2
Digital output NC
n: Number of output 1 - ...
The max. input number results from MD
$MN_FASTIO_DIG_NUM_OUTPUTS
$A_INA REAL $A_INA[n] RS R 2
Analog input NC
n: Number of input 1 - ...
The max. input number results from MD
$MN_FASTIO_ANA_NUM_INPUTS
$A_OUTA REAL $A_OUTA[n] RS W R W 2
Analog output NC When writing, the value does not become
active until the next IPO cycle at which point it is read back.
n: Number of output 1 - ...
The max. input number results from MD
$MN_FASTIO_ANA_NUM_OUTPUTS
$A_INCO BOOL $A_INCO[n] RS R 2
Comparator input
n: Number of output 1 - ...
The max. input number results from the MD
15.2.33 Reading and writing PLC variables
$A_DBB INT $A_DBB[n] RS W R W + 4
Read/write data byte (8 bits) from/to PLC
n: Position offset within I/O area 0 - ...
$A_DBW INT $A_DBW[n] RS W R W + 4
Read/write data word (16 bits) from/to PLC
n: Position offset within I/O area 0 - ...
$A_DBD INT $A_DBD[n] RS W R W + 4
Read/write double data word (32 bits) from/to PLC
n: Position offset within I/O area 0 - ...
$A_DBR REAL $A_DBR[n] RS W R W + 4
Read/write Real data (32 bits) from/to PLC
n: Position offset within I/O area 0 - ...
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-657
15 Tables 11.0215.2 List of system variables 15
15.2.34 NCU link
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$A_DLB INT $A_DLB[n] RS W R W + 5
Read/write data byte (8 bits) from/to NCU link
n: Position offset within the link memory area 0 - ...
$A_DLW INT $A_DLW[n] RS W R W + 5
Read/write data word (16 bits) from/to NCU link
n: Position offset within the link memory area 0 - ...
synchronized with main run
$A_DLD INT $A_DLD[n] RS W R W + 5
Read/write data double word (32 bits) from/to NCU link
n: Position offset within the link memory area 0 - ...
synchronized with main run
$A_DLR REAL $A_DLR[n] RS W R W + 5
Read/write Real data (32 bits) from/to NCU link
n: Position offset within the link memory area 0 - ...
synchronized with main run
$A_LINK_TRAN INT $A_LINK_TRANS_RATE R 5
S_RATE Number of bytes that can still be transferred via NCU link
Communication in the current IPO cycle.
15.2.35 Direct PLC I/O
$A_PBB_IN INT $A_PBB_IN[n] RS R 5
Read data byte (8 bits) directly from PLC I/O
n: Position offset within PLC input area 0 - ...
$A_PBW_IN INT $A_PBW_IN[n] RS R 5
Read data word (16 bits) directly from PLC I/O
n: Position offset within PLC input area 0 - ...
$A_PBD_IN INT $A_PBD_IN[n] RS R 5
Read data double word (32 bits) directly from PLC I/O
n: Position offset within PLC input area 0 - ...
$A_PBR_IN REAL $A_PBR_IN[n] RS R 6
Read Real data (32 bits) directly from PLC I/O .
n: Position offset within PLC input area 0 - ... 1
Siemens AG, 2002. All rights reserved
15-658 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$A_PBB_OUT INT $A_PBB_OUT[n] RS W R W 5
Write data byte (8 bits) directly to PLC I/O
n: Position offset within PLC output area 0 - ...
synchronized with main run
$A_PBW_OUT INT $A_PBW_OUT[n] RS W R W 5
Write data word (16 bits) directly to PLC I/O
n: Position offset within PLC output area 0 - ...
synchronized with main run
$A_PBD_OUT INT $A_PBD_OUT[n] RS W R W 5
Write data double word (32 bits) directly to PLC I/O
n: Position offset within PLC output area 0 - ...
synchronized with main run
$A_PBR_OUT REAL $A_PBR_OUT[n] RS W R W 5
Write Real data (32 bits) directly to PLC I/O
n: Position offset within PLC output area 0 - ...
synchronized with main run
$C_IN BOOL $C_IN[n] RS R 6
Signal from PLC to Cycle .
reserved for SIEMENS applications 1
n: Number of input 1 - ...
$C_OUT BOOL $C_OUT[n] RS W R W 6
Signal from Cycle to PLC .
reserved for SIEMENS applications 1
n: Number of output 1 - ...
15.2.36 Tool management
These system variables have value –1 if no tool management command is active at time of reading.
$AC_TC_CMDT INT $AC_TC_CMDT RS R 6
Trigger variable: $AC_TC_CMDT (CoMmandTrigger) then .
always takes on the value 1 for an interpolation cycle when a 1
new magazine management command is output to the PLC.
$AC_TC_ACKT INT $AC_TC_ACKT RS R 6
Trigger variable: $AC_TC_ACKT (ACKnowledgeTrigger) then .
always takes on a value of 1 for an interpolation cycle 1
when the PLC acknowledges a tool management command.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-659
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_TC_CMDC INT $AC_TC_CMDC RS WS R W 6
Counter variable: $AC_TC_CMDC (CoMmandCounter) is .
incremented by 1 for each tool management command 1
output to the PLC.
synchronized with main run
$AC_TC_ACKC INT $AC_TC_ACKC RS WS R W 6
Counter variable: $AC_TC_CMDC (ACKnowledgeCounter) .
on acknowledging a tool management command is 1
incremented by 1 via the PLC.
synchronized with main run
$AC_TC_FCT INT $AC_TC_FCT RS R 5
Command number. Specifies which action is desired.
-1: No tool management command is active at the time of
reading.
$AC_TC_STATUS INT $AC_TC_STATUS RS R 5
Status enjoyed by the command to read via $AC_TC_FCT.
-1: No tool management command is active at the time of
reading.
$AC_TC_THNO INT $AC_TC_THNO RS R 5
Number of the toolholder (spec. the spindle no.) where the
new tool is to be changed.
-1: No tool management command is active at the time of
reading.
$AC_TC_TNO INT $AC_TC_TNO RS R 5
NCK-internal T number of new tool (to be changed).
0: There is no new tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_MMYN INT $AC_TC_MMYN RS R 6
Owner magazine number of old tool (to be changed). .
0: There is no new tool, or the new tool (if $AC_TC_TNO > 4
0) is not loaded (manual tool).
-1: No tool management command is active at the time of
reading.
$AC_TC_LMYN INT $AC_TC_LMYN RS R 6
Owner location number of old tool (to be changed). .
0: There is no new tool, or the new tool (if $AC_TC_TNO > 4
0) is not loaded (manual tool).
-1: No tool management command is active at the time of
reading.
$AC_TC_MFN INT $AC_TC_MFN RS R 5
Source magazine number of new tool.
0: There is no new tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_LFN INT $AC_TC_LFN RS R 5
Source location number of new tool.
0: There is no new tool.
-1: No tool management command is active at the time of
reading.
Siemens AG, 2002. All rights reserved
15-660 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_TC_MTN INT $AC_TC_MTN RS R 5
Target magazine number of new tool.
0: There is no new tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_LTN INT $AC_TC_LTN RS R 5
Target location number of new tool.
0: There is no new tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_MFO INT $AC_TC_MFO RS R 5
Source magazine number of old tool (to be changed).
0: There is no old tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_LFO INT $AC_TC_LFO RS R 5
Source location number of old tool (to be changed).
0: There is no old tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_MTO INT $AC_TC_MTO RS R 5
Target magazine number of old tool (to be changed).
0: There is no old tool.
-1: No tool management command is active at the time of
reading.
$AC_TC_LTO INT $AC_TC_LTO RS R 5
Target location number of old tool (to be changed).
0: There is no old tool.
-1: No tool management command is active at the time of
reading.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-661
15 Tables 11.0215.2 List of system variables 15
15.2.37 Timers
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$A_YEAR INT $A_YEAR RS R 3
System time, year
$A_MONTH INT $A_MONTH RS R 3
System time, month
$A_DAY INT $A_DAY RS R 3
System time, day
$A_HOUR INT $A_HOUR RS R 3
System time, hour
$A_MINUTE INT $A_MINUTE RS R 3
System time, minute
$A_SECOND INT $A_SECOND RS R 3
System time, second
$A_MSECOND INT $A_MSECOND RS R 3
System time, millisecond
$AC_TIME REAL $AC_TIME RS R 2
Time from the beginning of block in seconds
This variable can only be accessed from synchronized
actions
$AC_TIMEC REAL $AC_TIMEC RS R 3
Time from the beginning of block in IPO clock cycles
This variable can only be accessed from synchronized
actions
$AC_TIMER REAL $AC_TIMER[n] RS WS R W + 4
Timer - unit in seconds
Time is counted internally in multiples of the interpolation
cycle;
Counting for the time variable is started by assigning the
value
$AC_TIMER[n]=
To stop the counter variable, assign a negative value:
$AC_TIMER[n]=-1
The current time can be read while the counter is active or
stopped. Stopping the time variable, by assigning - 1
stops the last current time value which can then be read
The dimension is defined in MD $MC_MM_NUM_AC_TIMER.
Siemens AG, 2002. All rights reserved
15-662 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Syn O S
$AC_PRTIME_M REAL $AC_PRTIME_M "ProgramRunTIME-Main" W 4
Set (initialize) the accumulated program runtime (main time)
$AC_PRTIME_A REAL $AC_PRTIME_A "ProgramRunTIME-Auxiliary" W 4
Set (initialize) the accumulated program runtime (auxiliary
time)
$AC_PRTIME_M REAL $AC_PRTIME_M_INC "ProgramRunTIME-Main- W 4
_INC INCrement"
Increment the accumulated program runtime (main time)
$AC_PRTIME_A REAL $AC_PRTIME_A_INC "ProgramRunTIME-Auxiliary- W 4
_INC INCrement"
Increment the accumulated program runtime (auxiliary time)
15.2.38 Path movement
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_PATHN REAL $AC_PATHN RS R 2
Normalized path parameter
value between 0=start of block and 1=end of block
This variable can only be accessed from synchronized
actions
$AC_DTBW REAL $AC_DTBW RS R 2
Geometric distance from start of block in workpiece
coordinate system
The programmed position is decisive for computing the
distance; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-663
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_REPOS_P INT $AC_REPOS_PATH_MODE RS R 6
ATH_MODE REPOS mode type .
0 not defined. 4
1 == RMB
Repositioning approach to start of interrupted block
2 == RMI
Repositioning approach to interruption point of interrupted
block
3 == RME
Repositioning approach to end of interrupted block
4 == RMN
Repositioning approach to geometrically nearest point of
interrupted block
The variable is defined just as REPOS is being executed,
or if a a new REPOS mode has been specified via VDI.
$AC_DTBB REAL $AC_DTBB RS R 2
Geometric distance from start of block in basic coordinate
system
The programmed position is decisive for computing the
distance; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
$AC_DTEW REAL $AC_DTEW RS R 2
Geometric distance from end of block in workpiece
coordinate system
The programmed position is decisive for computing the
distance; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
$AC_DTEB REAL $AC_DTEB RS R 2
Geometric distance from end of block in basic coordinate
system
The programmed position is decisive for computing the
distance; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
$AC_PLTBB REAL $AC_PLTBB RS R 3
Path distance from start of block in basic coordinate system
This variable can only be accessed from synchronized
actions
$AC_PLTEB REAL $AC_PLTEB RS R 3
Path distance from end of block in basic coordinate system
This variable can only be accessed from synchronized
actions
Siemens AG, 2002. All rights reserved
15-664 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_DELT REAL $AC_DELT R 3
Stored distance-to-go path in the workpiece coordinate
system subsequent to deletion of the residual distance
during synchronized motion actions
$P_APDV BOOL $P_APDV R 4
Returns True if the position values readable with
$P_APR[X] and $P_AEP[X] (approach and depart starting
point and contour point when smoothing) are valid.
15.2.39 Speeds/accelerations
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_F REAL $P_F R 2
Path feed F last programmed
$AC_F REAL $AC_F R 6
Programmed path feed F .
3
$AC_OVR REAL $AC_OVR: R W 2
Path override for synchronized actions
Multiplicative override component, works in addition to
operation OV, programmed OV and transformation OV.
However, the overall factor remains limited to the maximum
value defined by machine data
$MN_OVR_FACTOR_LIMIT_BIN and
$MN_OVR_FACTOR_FEEDRATE[31].
If a value of < 0.0 is entered, 0 is assumed and alarm
14756 reported.
Must be rewritten in every interpolator cycle, otherwise the
value is 100%.
This variable can only be accessed from synchronized
actions
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-665
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_VC REAL $AC_VC R W 2
Additive path feed compensation for synchronized actions
The compensation value does not work with G0, G33,
G331, G332 and G63.
It must be rewritten in every interpolator cycle, otherwise the
value is 0.
With an override of 0, the compensation value has no
effect, otherwise the override has no impact on the
compensation value.
The compensation value cannot make the total feedrate
negative.
The upper value is limited such that the maximum axis
velocities and accelerations are not exceeded.
The computation with different feedrate components is not
affected by $AC_VC.
The override defined by machine data
$MN_OVR_FACTOR_LIMIT_BIN,
$MN_OVR_FACTOR_FEEDRATE[30],
$MN_OVR_FACTOR_AX_SPEED[30] and
$MN_OVR_FACTOR_SPIND_SPEED
Override values cannot be exceeded. The additive feedrate
override is limited such that the resulting feedrate does not
exceed the maximum override value of the programmed
feedrate.
This variable can only be accessed from synchronized
actions
$AC_PATHACC REAL $AC_PATHACC RS WS R W 6
Specification of an increased path acceleration for override .
changes and Stop/Start events. 3
$AC_PATHACC is only considered when the value is
greater than the prepared acceleration limitation.
The value 0 deselects the function.
Values that lead to machine axis accelerations that are
twice as high as that parameterized in
$MA_MAX_AX_ACCEL[..], are accordingly restricted
internally.
$AC_PATHJERK REAL $AC_PATHJERK RS WS R W 6
Specification of an increased path jerk for override changes .
and Stop/Start events. 3
$AC_PATHJERK is only considered when the value is
greater than the prepared jerk limitation.
The value 0 deselects the function.
$AC_VACTB REAL $AC_VACTB RS R 2
Path velocity in the base coordinate system
This variable can only be accessed from synchronized
actions
$AC_VACTW REAL $AC_VACTW RS R 2
Path velocity in workpiece coordinate system
This variable can only be accessed from synchronized
actions
Siemens AG, 2002. All rights reserved
15-666 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
15.2.40 Spindles
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_S REAL $P_S[n] R 2
Last programmed spindle speed
n: Spindle number
0 ... max. spindle number
$AA_S REAL $AA_S[n] RS R 4
Spindle actual speed. The sign corresponds to the direction
of rotation.
n: Spindle number
0 ... max. spindle number
$P_CONSTCUT REAL $P_CONSTCUT_S[n] R 6
_S Last programmed constant cutting speed. .
n: Spindle number 1
0 ... max. spindle number
$AC_CONSTCU REAL $AC_CONSTCUT_S[n] RS R 6
T_S Current constant cutting speed. .
n: Spindle number 1
0 ... max. spindle number
$P_SEARCH_S REAL $P_SEARCH_S[n] R 6
The last programmed spindle speed or cutting rate picked .
up during search mode 1
n: Spindle number
0 ... max. spindle number
$P_SDIR INT $P_SDIR[n] R 3
Last direction of spindle rotation to be programmed.
3: Clockwise spindle rotation,
4: Counterclockwise spindle rotation,
5: Spindle stop
n: Spindle number
0 ... max. spindle number
$AC_SDIR INT $AC_SDIR[n] RS R 3
Current direction of spindle rotation
3: Clockwise spindle rotation,
4: Counterclockwise spindle rotation,
5: Spindle stop
n: Spindle number
0 ... max. spindle number
$P_SEARCH_S INT $P_SEARCH_SDIR[n] R 6
DIR The last programmed spindle programming picked up .
during search mode: 1
3: M3 Clockwise spindle rotation
4: M4 Counterclockwise spindle rotation
5: M5 Spindle stop
-19: M19, SPOS, SPOSA spindle positioning, position and
approach mode are read from SEARCH variables
70: M70 Switch over to axis mode
-5: No direction of spindle rotation programmed, no output.
n: Spindle number
0 ... max. spindle number
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-667
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_SMODE INT $P_SMODE[n] R 3
Last programmed spindle mode:
0: No spindle in the channel or spindle is active in another
channel or
is being used by the PLC (FC18) or by synchronized
actions.
1: Speed control mode
2: Positioning mode
3: synchronized mode
4: Axis mode
n: Spindle number
0 ... max. spindle number
$AC_SMODE INT $AC_SMODE[n] RS R 3
Spindle mode currently active
0: No spindle in the channel
1: Speed control mode
2: Positioning mode
3: synchronized mode
4: Axis mode
n: Spindle number
0 ... max. spindle number
$P_SGEAR INT $P_SGEAR[n] R 6
Spindle gear stage last programmed or requested during .
M40 by S programming 1
1: 1st gear stage requested
....
5: 5th gear stage requested
n: Spindle number
0 ... max. spindle number
$AC_SGEAR INT $AC_SGEAR[n] RS R 6
Active spindle gear stage .
1: 1st gear stage is active 1
....
5: 5th gear stage is active
n: Spindle number
0 ... max. spindle number
$P_SAUTOGEAR INT $P_SAUTOGEAR[n] R 6
Automatic gear stage change (M40) is programmed. .
0: Gear stages are requested by M41..M45 1
1: The gear stage is calculated and requested (M40
Automatic gear stage change is active) to fit the
programmed speed (S)
n: Spindle number
0 ... max. spindle number
Siemens AG, 2002. All rights reserved
15-668 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_SEARCH_S INT $P_SEARCH_SGEAR[n] R 6
GEAR The last programmed gear stages M function picked up .
during search mode. 1
40: M40 Automatic gear stage change
41: M41 1st gear stage requested
...
45: M45 5th gear stage requested
n: Spindle number
0 ... max. spindle number
$P_SEARCH_S REAL $P_SEARCH_SPOS[n] R W 6
POS The last spindle position or travel path programmed by M19, .
SPOS or SPOSA 1
picked up during search mode.
Position: 0...359.999, when the value in MD 30330
MODULO_RANGE is 360.0 degrees
Path: -100000000 ... 100000000 degrees. The sign
indicates the traversing direction.
n: Spindle number
0 ... max. spindle number
$P_SEARCH_S INT $P_SEARCH_SPOSMODE[n] R W 6
POSMODE The last position approach mode programmed by M19, .
SPOS or SPOSA picked up during search mode. 1
0: DC
1: AC
2: IC
3: DC
4: ACP
5: ACN
n: Spindle number
0 ... max. spindle number
$P_NUM_SPIND INT $P_NUM_SPINDLES R 6
LES Calculates the maximum number of spindles in the channel .
0: No spindle in the channel. 1
1..n: Number of spindles in the channel
$P_MSNUM INT $P_MSNUM R 6
Returns the number of the master spindle. .
0: No spindle in the channel 1
1..n: Number of the master spindle
$AC_MSNUM INT $AC_MSNUM RS R 3
Returns the number of the current master spindle.
0: No spindle exists
1..n: Number of the master spindle
$P_MTHNUM INT $P_MTHNUM - only useful with active magazine R 6
management .
Returns the number of the master tool carrier: 1
0: No master tool carrier
1..n: Number of master tool carrier
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-669
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MTHNUM INT $AC_MTHNUM - only useful with active magazine RS R 6
management .
Returns the number of the current master tool carrier: 1
0: No master tool carrier
1..n: Number of master tool carrier
$P_GWPS BOOL $P_GWPS[n] R 2
Constant grinding wheel surface speed on if TRUE
n: Spindle number
15.2.41 Polynomial values for synchronized actions
$AC_FCT1LL REAL $AC_FCT1LL RS WS R W + 2
Lower limit value for evaluation function FCTDEF 1
$AC_FCT2LL REAL $AC_FCT2LL RS WS R W + 2
Lower limit value for evaluation function FCTDEF 2
$AC_FCT3LL REAL $AC_FCT3LL RS WS R W + 2
Lower limit value for evaluation function FCTDEF 3
$AC_FCT1UL REAL $AC_FCT1UL RS WS R W + 2
Upper limit value for evaluation function FCTDEF 1
$AC_FCT2UL REAL $AC_FCT2UL RS WS R W + 2
Upper limit value for evaluation function FCTDEF 2
$AC_FCT3UL REAL $AC_FCT3UL RS WS R W + 2
Upper limit value for evaluation function FCTDEF 3
$AC_FCT1C REAL $AC_FCT1C[n] RS WS R W + 2
Polynomial coefficient a0–a3 for evaluation function
FCTDEF 1
n: Degree of coefficient 0–3
$AC_FCT2C REAL $AC_FCT2C[n] RS WS R W + 2
Polynomial coefficient a0–a3 for evaluation function
FCTDEF 2
n: Degree of coefficient 0–3
$AC_FCT3C REAL $AC_FCT3C[n] RS WS R W + 2
Polynomial coefficient a0–a3 for evaluation function
FCTDEF 3
n: Degree of coefficient 0–3
$AC_FCTLL REAL $AC_FCTLL[n] RS WS R W + 4
Lower limit of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
$AC_FCTUL REAL $AC_FCTUL[n] RS WS R W + 4
Upper limit of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
Siemens AG, 2002. All rights reserved
15-670 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_FCT0 REAL $AC_FCT0[n] RS WS R W + 4
a0 coefficient of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
$AC_FCT1 REAL $AC_FCT1[n] RS WS R W + 4
a1 coefficient of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
$AC_FCT2 REAL $AC_FCT2[n] RS WS R W + 4
a2 coefficient of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
$AC_FCT3 REAL $AC_FCT3[n] RS WS R W + 4
a3 coefficient of polynomial for synchronized actions
(SYNFCT)
n: Number of polynomial, limited by machine data
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-671
15 Tables 11.0215.2 List of system variables 15
15.2.42 Channel states
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_ALARM_S INT $AC_ALARM_STAT RS R 5
TAT (Selected) alarm reactions for synchronized actions
(SYNFCT)
$AN_ESR_TRIG BOOL $AN_ESR_TRIGGER = 1 R W 5
GER Trigger "Extended stop and retract"
$AN_BUS_FAIL BOOL $AN_BUS_FAIL_TRIGGER = 1 R W 6
_TRIGGER Simulation of a drive bus failure for test purposes .
4
$AC_ESR_TRIG BOOL $AC_ESR_TRIGGER = 1 R W 6
GER Triggering "NC controlled ESR" .
1
$AC_OPERATIN REAL IF $AC_OPERATING_TIME < 12000 GOTOB RS WS R W 6
G_TIME STARTMARK .
Total execution time ( in seconds ) of NC programs in 1
automatic mode
$AC_CYCLE_TI REAL IF $AC_CYCLE_TIME > 2400 GOTOF ALARM01 RS WS R W 6
ME Execution time of the selected NC program .
( in seconds ) 1
$AC_CUTTING_ REAL IF $AC_CUTTING_TIME > 6000 GOTOF ACT_M06 RS WS R W 6
TIME Tool operation time .
( in seconds ) 1
$AC_REQUIRE REAL $AC_REQUIRED_PARTS = ACTUAL_LOS RS WS R W 6
D_PARTS Definition of number of parts required, .
e.g. for definition of a batch size, daily production target, 1
etc.
$AC_TOTAL_PA REAL IF $AC_TOTAL_PARTS > SERVICE_COUNT GOTOF RS WS R W 6
RTS MARK_END .
Total number of all parts produced 1
$AC_ACTUAL_ REAL IF $AC_ACTUAL_PARTS == 0 GOTOF NEW_RUN RS WS R W 6
PARTS Actual number of parts produced .
For $AC_ACTUAL_PARTS == $AC_REQUIRED_PARTS, 1
$AC_ACTUAL_PARTS = 0
automatically.
$AC_SPECIAL_ REAL $AC_SPECIAL_PARTS = R20 RS WS R W 6
PARTS Number of parts counted according to a user strategy. .
without internal impact. 1
Siemens AG, 2002. All rights reserved
15-672 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_G0MODE INT $AC_G0MODE R 6
0: G0 not active .
1: G0 and linear interpolation active 1
2: G0 and nonlinear interpolation active
The response of the path axes at G0 is dependent on
machine data $MC_G0_LINEAR_MODE (Siemens mode)
or $MC_EXTERN_G0_LINEAR_MODE (ISO mode):
with linearer interpolation, the path axes traverse together,
with non-linear interpolation, the path axes traverse as
positioning axes.
15.2.43 Measurement
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MEAS_SE INT $AC_MEAS_SEMA = 1 R W 6
MA Assigning the measuring interface. .
1
$AC_MEAS_LA INT $AC_MEAS_LATCH[0] = 1 R WS R W 6
TCH Writing the actual axis values to the 1st measuring point. .
0: 1st measuring point, 1
.. ,
3: 4th measuring point
$AC_MEAS_P1_ INT $AC_MEAS_P1_COORD = R W 6
COORD 0: WCS .
1: BCS 4
2: MCS
Coordinate system of the 1st measuring point.
$AC_MEAS_P2_ INT $AC_MEAS_P2_COORD = R W 6
COORD 0: WCS .
1: BCS 4
2: MCS
Coordinate system of the 2nd measuring point.
$AC_MEAS_P3_ INT $AC_MEAS_P3_COORD = R W 6
COORD 0: WCS .
1: BCS 4
2: MCS
Coordinate system of the 3rd measuring point.
$AC_MEAS_P4_ INT $AC_MEAS_P4_COORD = R W 6
COORD 0: WCS .
1: BCS 4
2: MCS
Coordinate system of the 4th measuring point.
$AC_MEAS_SE INT $AC_MEAS_SET_COORD = R W 6
T_COORD 0: WCS .
1: BCS 4
2: MCS
Coordinate system of the setpoint.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-673
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MEAS_WP REAL $AC_MEAS_WP_SETANGLE = 0.0 R W 6
_SETANGLE Setpoint angle of the part position for part gauging. .
1
$AC_MEAS_CO REAL $AC_MEAS_CORNER_SETANGLE = 90.0 R W 6
RNER_SETANG Setpoint cutting angle of the corner for part gauging. .
LE 1
$AC_MEAS_DIR INT $AC_MEAS_DIR_APPROACH = R W 6
_APPROACH 0: +x .
1: -x 1
2: +y
3: -y
4: +z
5: -z
Direction of approach to the part.
$AC_MEAS_AC INT $AC_MEAS_ACT_PLANE = R W 6
T_PLANE 0: G17 .
1: G18 1
2: G19
Setting the plane for calculation and measuring.
$AC_MEAS_FIN INT $AC_MEAS_FINE_TRANS = R W 6
E_TRANS 0: Offset in Trans .
1: Offset in Fine Trans 3
Setting the fine offset for calculation and measuring.
$AC_MEAS_FR INT $AC_MEAS_FRAME_SELECT = R W 6
AME_SELECT 0: $P_SETFRAME .
10..25: $P_CHBFRAME[0..15] 1
50..65: $P_NCBFRAME[0..15]
100..199: $P_IFRAME
1010..1025: $P_CHBFRAME[0..15], with active G500
1050..1065: $P_NCBFRAME[0..15], with active G500
2000: $P_SETFR
2010..2025: $P_CHBFR[0..15]
2050..2065: $P_NCBFR[0..15]
2100..2199: $P_UIFR[0..99]
3010..3025: $P_CHBFR[0..15], with active G500
3050..3065: $P_NCBFR[0..15], with active G500
Selecting the frames for part gauging.
$AC_MEAS_CH INT $AC_MEAS_CHSFR = 'B1001' R W 6
SFR System frame bit mask in accordance with .
$MC_MM_SYSTEM_FRAME_MASK 4
$AC_MEAS_NC INT $AC_MEAS_NCBFR = 'B1' R W 6
BFR Global basic frame mask to set up the new frame. .
4
$AC_MEAS_CH INT $AC_MEAS_CHBFR = 'B1' R W 6
BFR Channel basic frame mask to set up the new frame. .
4
$AC_MEAS_UIFR INT $AC_MEAS_UIFR = 1 R W 6
Adjustable data management frame to set up the new .
frame. 4
Siemens AG, 2002. All rights reserved
15-674 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MEAS_PF INT $AC_MEAS_PFRAME = 1 R W 6
RAME Programmable frame not included. .
4
$AC_MEAS_T_ INT $AC_MEAS_T_NUMBER = 1 R W 6
NUMBER Selecting the tool for calculation and measuring. .
1
$AC_MEAS_TO INT $AC_MEAS_TOOL_MASK = 'B1' R W 6
OL_MASK Setting the tool for calculation and measuring. .
4
$AC_MEAS_D_ INT $AC_MEAS_D_NUMBER = 1 R W 6
NUMBER Selecting the cutting edge for calculation and measuring. .
1
$AC_MEAS_TY INT $AC_MEAS_TYPE = R W 6
PE 0: default .
1: x edge 1
2: y edge
3: z edge
4: corner 1
5: corner 2
6: corner 3
7: corner 4
8: bore hole
9: shaft
10: tool length
11: tool diameter
12: groove
13: bar
14: preset actual value memory for geometry and special
axes
15: preset actual value memory for special axes only
16: oblique edge
17: Plane_Angles (2 solid angles of a plane)
18: Plane_Normal (3 solid angles of a plane with
setpoint input)
19: Dimension_1 (1-dimensional setpoint input)
20: Dimension_2 (2-dimensional setpoint input)
21: Dimension_3 (3-dimensional setpoint input)
22: ToolMagnifier (ShopTurn: Measuring
tool lengths with a zoom-in function)
23: ToolMarkedPos (ShopTurn: Measuring a
tool length with a marked position)
24: coordinate transformation of a position
25: rectangle
Specification of the measuring type.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-675
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MEAS_VA INT $AC_MEAS_VALID = 0 R W 6
LID Validity bits of the measuring variables. The value should .
be set to 0 prior to all measuring processes. The individual 1
bits are set implicitly when writing to the corresponding
variables.
Bit 0: $AA_MEAS_POINT1[axis]
Bit 1: $AA_MEAS_POINT2[axis]
Bit 2: $AA_MEAS_POINT3[axis]
Bit 3: $AA_MEAS_POINT4[axis]
Bit 4: $AA_MEAS_SETPOINT[axis]
Bit 5: $AC_MEAS_WP_SETANGLE
Bit 6: $AC_MEAS_CORNER_SETANGLE
Bit 7: $AC_MEAS_T_NUMBER
Bit 8: $AC_MEAS_D_NUMBER
Bit 9: $AC_MEAS_DIR_APPROACH
Bit 10 :$AC_MEAS_ACT_PLANE
Bit 11: $AC_MEAS_FRAME_SELECT
Bit 12: $AC_MEAS_TYPE
Bit 13: $AC_MEAS_FINE_TRANS
Bit 14: $AA_MEAS_SETANGLE[axis]
Bit 15: $AC_MEAS_SCALEUNIT
Bit 16: $AC_MEAS_TOOL_MASK
Bit 17: $AC_MEAS_P1_COORD
Bit 18: $AC_MEAS_P2_COORD
Bit 19: $AC_MEAS_P3_COORD
Bit 20: $AC_MEAS_P4_COORD
Bit 21: $AC_MEAS_SET_COORD
Bit 22: $AC_MEAS_CHSFR
Bit 23: $AC_MEAS_NCBFR
Bit 24: $AC_MEAS_CHBFR
Bit 25: $AC_MEAS_UIFR
Bit 26: $AC_MEAS_PFRAME
$AC_MEAS_FR FRAME $AC_MEAS_FRAME R W 6
AME Result frame for part gauging. .
1
$AC_MEAS_WP REAL $AC_MEAS_WP_ANGLE R 6
_ANGLE Calculated part position angle for part gauging. .
1
$AC_MEAS_CO REAL $AC_MEAS_CORNER_ANGLE R 6
RNER_ANGLE Calculated cutting angle of the corner for part gauging. .
1
$AC_MEAS_DIA REAL $AC_MEAS_DIAMETER R 6
METER Calculated diameter for part and tool gauging. .
1
$AC_MEAS_TO REAL $AC_MEAS_TOOL_LENGTH R 6
OL_LENGTH Calculated tool length for tool gauging. .
1
Siemens AG, 2002. All rights reserved
15-676 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_MEAS_RE REAL R0 = $AC_MEAS_RESULTS[0] R 6
SULTS Measured results .
3
$AC_MEAS_SC INT Unit of measurement in accordance with the configuration R W 6
ALEUNIT $AC_MEAS_SCALEUNIT = 0 .
Unit of measurement relative to the active G code 4
G70/G700/G71/G710
$P_CHANNO INT Query the current channel number. R 6
.
4
$AC_SERUPRO INT $AC_SERUPRO R 6
Query whether search run type SERUPRO is active. .
(SERUPRO: "Search run via program testing") 4
Possible to use in SYNACTs and in the parts program
$AC_SERUPRO == 0 SERUPRO search run type not
active
$AC_SERUPRO == 1 SERUPRO search run type is
active
15.2.44 Positions
$P_EP REAL $P_EP[X] R 2
The system variable $P_EP always returns the current
WCS setpoint position in the interpreter. The numerical
value is not inevitably the same as the programmed value in
the parts program. In the following situations there are
differences
- during incremental programming
- when changing the WCS by frame or tool selection
If an ASUB starts after a block search with calculation, this
event will synchronize positions in the interpreter. $P_EP
then returns in ASUB the position at which the axes actually
are. The search run position that is picked up can be
queried via system variable $AC_RETPOINT.
Axes: channel axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-677
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_EPM REAL $P_EPM[X] R 6
Current MCS position in the interpreter (also see $P_EP). .
Axes: channel axis 1
$P_APR REAL $P_APR[X] R 4
Position of axis in the workpiece coordinate system at the
start of the approach motion for soft approach to the
contour. Axes: channel axis
$P_AEP REAL $P_AEP[X] R 4
Approach point: first contour point in the workpiece
coordinate system for soft approach to contour. Axes:
channel axis
$P_POLF REAL $P_POLF[X] R 6
X: Axis .
returns the programmed return position of the axis 4
Axes: geometry axis, channel axis, machine axis
$P_POLF_VALID INT $P_POLF_VALID[X] R 6
X: Axis .
0: no axis return programmed 4
1: return programmed in abs. position
2: return programmed as distance
Axes: geometry axis, channel axis, machine axis
$AA_IW REAL $AA_IW[X] RS R 2
Actual value in workpiece coordinate system (WCS)
Axes: channel axis
$AA_REPOS_D BOOL $AA_REPOS_DELAY[X] RS R + 6
ELAY TRUE: For this axis REPOS suppression is just active. .
FALSE: otherwise 4
Axes: channel axis
$AA_IEN REAL $AA_IEN[X] RS R 5
Actual value in the settable origin system (SOS).
Axes: channel axis
$AA_IBN REAL $AA_IBN[X] RS R 5
Actual value in the basic origin system (BOS).
Axes: channel axis
$AA_IB REAL $AA_IB[X] RS R 2
Actual value in basic coordinate system (BCS)
Axes: channel axis
$AA_IM REAL $AA_IM[X] RS R 2
Actual value in machine coordinate system (MCS).
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
15-678 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
15.2.45 Indexing axes
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_ACT_INDE INT $AA_ACT_INDEX_AX_POS_NO[X] RS R 5
X_AX_POS_NO 0: No indexing axis, therefore no indexing position available.
> 0: Number of indexing position last reached or crossed
Axes: geometry axis, channel axis, machine axis
$AA_PROG_INDE INT $AA_PROG_INDEX_AX_POS_NO[X] RS R 5
X_AX_POS_NO 0: No indexing axis, thus no indexing position
available or indexing axis currently not approaching
an indexing position
> 0: Number of programmed indexing position
Axes: geometry axis, channel axis, machine axis
15.2.46 Encoder values
$AA_ENC_ACTI BOOL $AA_ENC_ACTIVE[X] RS R 4
VE Active measuring system is operating below encoder limit
frequency
Axes: geometry axis, channel axis, machine axis
$AA_ENC1_ACT BOOL $AA_ENC1_ACTIVE[X] RS R 4
IVE Encoder 1 is operating below encoder limit frequency
Axes: geometry axis, channel axis, machine axis
$AA_ENC2_ACT BOOL $AA_ENC2_ACTIVE[X] RS R 4
IVE Encoder 2 is operating below encoder limit frequency
Axes: geometry axis, channel axis, machine axis
$VA_IM REAL $VA_IM[X] RS R 4
Encoder actual value in machine coordinate system
(measured on active measuring system), actual value
compensations are corrected (leadscrew error
compensation, backlash compensation, quadrant error
compensation)
With active spindle/axis disable, the default return is the
current setpoint. If the actual value is then returned, BIT3
must be set in $MA_MISC_FUNCTION_MASK.
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-679
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$VA_IM1 REAL $VA_IM1[X] RS R 4
Actual value in the machine coordinate system (measured
Encoder 1), compensations are corrected
With active spindle/axis disable the default return is the
current setpoint. If the actual value is then returned, BIT3
must be set in $MA_MISC_FUNCTION_MASK.
$VA_IM2 REAL $VA_IM2[X] RS R 4
Actual value in the machine coordinate system (measured
Encoder 2), compensations are corrected
With active spindle/axis disable the default return is the
current setpoint. If the actual value is then returned, BIT3
must be set in $MA_MISC_FUNCTION_MASK.
$AA_MW REAL $AA_MW[X] R WS R W 2
Measured value in workpiece coordinate system
Axes: channel axis
$AA_MM REAL $AA_MM[X] R WS R W 2
Measured value in machine coordinate system
$AA_MW1 REAL $AA_MW1[X] R WS R W 4
Measurement result of axial measurement
Trigger event 1 in WCS
Axes: channel axis
$AA_MW2 REAL $AA_MW2[X] R WS R W 4
Measurement result of axial measurement
Trigger event 2 in WCS
Axes: channel axis
$AA_MW3 REAL $AA_MW3[X] R WS R W 4
Measurement result of axial measurement
Trigger event 3 in WCS
Axes: channel axis
$AA_MW4 REAL $AA_MW4[X] R WS R W 4
Measurement result of axial measurement
Trigger event 4 in WCS
Axes: channel axis
15.2.47 Axial measurement
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_MM1 REAL $AA_MM1[X] R WS R W 4
Measurement result of axial measurement
Trigger event 1 in MCS
$AA_MM2 REAL $AA_MM2[X] R WS R W 4
Measurement result of axial measurement
Trigger event 2 in MCS
$AA_MM3 REAL $AA_MM3[X] R WS R W 4
Measurement result of axial measurement
Trigger event 3 in MCS
Siemens AG, 2002. All rights reserved
15-680 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_MM4 REAL $AA_MM4[X] R WS R W 4
Measurement result of axial measurement
Trigger event 4 in MCS
$AA_MEAACT BOOL $AA_MEAACT[X] R 4
Value is TRUE if axial measurement is active for X
Axes: geometry axis, channel axis, machine axis
15.2.48 Offsets
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_DRF REAL $AC_DRF[X] RS R 2
DRF offset
Axes: channel axis
$AC_PRESET REAL $AC_PRESET[X] RS R 2
Last given PRESET value
Axes: channel axis
$AA_ETRANS REAL $AA_ETRANS[X] R W 2
External zero offset
Axes: channel axis
$AA_MEAS_P1_ INT $AA_MEAS_P1_VALID[X] = 1 R WS R W 6
VALID Writing the actual axis value to the 1st measuring point. .
Axes: geometry axis, channel axis, machine axis 1
$AA_MEAS_P2_ INT $AA_MEAS_P2_VALID[X] = 1 R WS R W 6
VALID Writing the actual axis value to the 2nd measuring point. .
Axes: geometry axis, channel axis, machine axis 1
$AA_MEAS_P3_ INT $AA_MEAS_P3_VALID[X] = 1 R WS R W 6
VALID Writing the actual axis value to the 3rd measuring point. .
Axes: geometry axis, channel axis, machine axis 1
$AA_MEAS_P4_ INT $AA_MEAS_P4_VALID[X] = 1 R WS R W 6
VALID Writing the actual axis value to the 4th measuring point. .
Axes: geometry axis, channel axis, machine axis 1
$AA_MEAS_POI REAL $AA_MEAS_POINT1[x] = $AA_IW[x] R W 6
NT1 $AA_MEAS_POINT1[y] = $AA_IW[y] .
$AA_MEAS_POINT1[z] = $AA_IW[z] 1
First measuring point for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
$AA_MEAS_POI REAL $AA_MEAS_POINT2[x] = $AA_IW[x] R W 6
NT2 $AA_MEAS_POINT2[y] = $AA_IW[y] .
$AA_MEAS_POINT2[z] = $AA_IW[z] 1
Second measuring point for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-681
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_MEAS_POI REAL $AA_MEAS_POINT3[x] = $AA_IW[x] R W 6
NT3 $AA_MEAS_POINT3[y] = $AA_IW[y] .
$AA_MEAS_POINT3[z] = $AA_IW[z] 1
Third measuring point for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
$AA_MEAS_POI REAL $AA_MEAS_POINT4[x] = $AA_IW[x] R W 6
NT4 $AA_MEAS_POINT4[y] = $AA_IW[y] .
$AA_MEAS_POINT4[z] = $AA_IW[z] 1
Fourth measuring point for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
$AA_MEAS_SP INT $AA_MEAS_SP_VALID[X] = 0 R W 6
_VALID Invalidating the x-axis setpoint for part and tool gauging. .
Axes: geometry axis, channel axis, machine axis 1
$AA_MEAS_SE REAL $AA_MEAS_SETPOINT[X] = 0.0 R W 6
TPOINT $AA_MEAS_SETPOINT[y] = 0.0 .
$AA_MEAS_SETPOINT[z] = 0.0 1
Setpoint position for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
$AA_MEAS_SE REAL $AA_MEAS_SETANGLE[x] = 0.0 R W 6
TANGLE $AA_MEAS_SETANGLE[y] = 0.0 .
$AA_MEAS_SETANGLE[z] = 0.0 4
Setpoint angle for part and tool gauging.
Axes: geometry axis, channel axis, machine axis
$AA_OFF REAL $AA_OFF[X] RS W R W 3
Overlaid motion for programmed axis
Axes: geometry axis, channel axis, machine axis
$AA_OFF_LIMIT INT $AA_OFF_LIMIT[axis] RS R 4
Limit value for axial offset $AA_OFF[axis]
0: Limit value not reached
1: Limit value reached in positive axis direction
-1: Limit value reached in negative axis direction
Axes: geometry axis, channel axis, machine axis
$AA_OFF_VAL REAL $AA_OFF_VAL[axis] RS R 6
Integrated value of the overlaid movement for one axis. .
An overlaid movement can be undone by using the negative 1
value of these variables.
For example $AA_OFF[axis] = -$AA_OFF_VAL[axis]
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
15-682 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AC_RETPOINT REAL $AC_RETPOINT[X] RS R 2
$AC_RETPOINT[] returns the WCS position of an axis at
which an ASUB was started. Then repositioning to this
position can take place in the ASUB.
If an ASUB is started up directly after a block search with
calculation, $AC_RETPOINT returns the search run
position that has been picked up.
Axes: channel axis
$AA_TOFF REAL $AA_TOFF[geometry axis] RS W R W 6
Overlaid value in the tool coordinate system. .
Axes: geometry axis 4
$AA_TOFF_VAL REAL $AA_TOFF_VAL[geometry axis] RS R 6
Overlaid value in the tool coordinate system (integrated). .
Axes: geometry axis 4
$AA_TOFF_LIMIT INT $AA_TOFF_LIMIT[geo axis] RS R 6
Limit value for axial offset $AA_TOFF[geo axis] .
0: Limit value not reached 4
1: Limit value reached in positive axis direction
-1: Limit value reached in negative axis direction
Axes: geometry axis
$AA_TOFF_PRE REAL $AA_TOFF_PREP_DIFF[geometry axis] RS R 6
P_DIFF Difference value of the override in the tool coordinate .
system between the main run and preprocessing. 4
Axes: geometry axis
$AA_SOFTENDP REAL $AA_SOFTENDP[X] RS R 2
Software end position, positive direction
Axes: geometry axis, channel axis, machine axis
$AA_SOFTENDN REAL $AA_SOFTENDN[X] RS R 2
Software end position, negative direction
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-683
15 Tables 11.0215.2 List of system variables 15
15.2.49 Axial paths
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_DTBW REAL $AA_DTBW[X] RS R 2
axial path from start of block in the workpiece coordinate
system for positioning and synchronized axes for motion
synchronized action
The programmed position is decisive for computing the
path; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_DTBB REAL $AA_DTBB[X] RS R 2
Axial distance from start of block in basic coordinate system
for positioning and synchronized axes with motion-
synchronized actions
The programmed position is decisive for computing the
path; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_DTEW REAL $AA_DTEW[X] RS R 2
Axial distance to end of block in workpiece coordinate
system
for positioning and synchronized axes with motion-
synchronized actions
The programmed position is decisive for computing the
path; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_DTEB REAL $AA_DTEB[X] RS R 2
Axial distance to end of block in basic coordinate system
for positioning and synchronized axes with motion-
synchronized actions
The programmed position is decisive for computing the
path; if the axis is a coupling axis, the position part that
results from axis coupling is not considered here.
This variable can only be accessed from synchronized
actions
Axes: channel axis
Siemens AG, 2002. All rights reserved
15-684 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
15.2.50 Oscillation
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_DTEPW REAL $AA_DTEPW[X] RS R 2
Axial distance-to-go for infeed oscillation in
workpiece coordinate system
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_DTEPB REAL $AA_DTEPB[X] RS R 2
Axial distance-to-go for infeed oscillation in basic coordinate
system
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_OSCILL_R REAL $AA_OSCILL_REVERSE_POS1[X] RS R 3
EVERSE_POS1 Current reversal position 1 for oscillation
In synchronized actions, the setting data value
$SA_OSCILL_REVERSE_POS1 is evaluated online
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_OSCILL_R REAL $AA_OSCILL_REVERSE_POS2[X] RS R 3
EVERSE_POS2 Current reversal position 2 for oscillation
In synchronized actions, the setting data value
$SA_OSCILL_REVERSE_POS2 is evaluated online
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_DELT REAL $AA_DELT[X] R 2
Stored axial distance-to-go path in the workpiece coordinate
system subsequent to deletion of the residual distance
during synchronized motion actions
Axes: geometry axis, channel axis, machine axis
15.2.51 Axial velocities
$P_FA REAL $P_FA[X] R 2
Last programmed axial feedrate
Axes: channel axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-685
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_OVR REAL $AA_OVR[X] R W 2
Axial override for motion-synchronized actions
Multiplicative override component acting in addition to the
user OV, programmed OV and transformation OV.
The value is limited to max. 200%. If a value < 0.0 is
entered, 0 is assumed and alarm 14756 reported.
Must be rewritten in every interpolator cycle, otherwise the
value is 100%.
The spindle override is changed with $AA_OVR[S1].
This variable can only be accessed from motion-
synchronized actions
Axes: channel axis
$AA_VC REAL $AA_VC[X] R W 2
Additive axial feed compensation for motion-synchronized
actions
It must be rewritten in every interpolator cycle, otherwise the
value is 0.
With an override of 0, the compensation value has no
effect, otherwise the override has no impact on the
compensation value.
The compensation value cannot make the total feedrate
negative.
The upper value is limited such that the maximum axis
velocities and accelerations are not exceeded.
The computation of the other feedrate components is not
affected by $AA_VC.
The override defined by machine data
$MN_OVR_FACTOR_LIMIT_BIN,
$MN_OVR_FACTOR_FEEDRATE[30],
$MN_OVR_FACTOR_AX_SPEED[30] and
$MN_OVR_FACTOR_SPIND_SPEED
Override values cannot be exceeded. The additive feedrate
override is limited such that the resulting feedrate does not
exceed the maximum override value of the programmed
feedrate.
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_VACTB REAL $AA_VACTB[X] RS R 2
Axis velocity in the base coordinate system
This variable can only be accessed from synchronized
actions
Axes: channel axis
$AA_VACTW REAL $AA_VACTW[X] RS R 2
Axis velocity in workpiece coordinate system
This variable can only be accessed from synchronized
actions
Axes: channel axis
Siemens AG, 2002. All rights reserved
15-686 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_VACTM REAL $AA_VACTM[X] RS R 4
Axis velocity, setpoint-related in machine coordinate system
Can also be read for replacement and PLC axes
This variable can only be accessed from synchronized
actions
Axes: channel axis
$VA_VACTM REAL $VA_VACTM[X] RS R 4
Axis velocity, actual value-related in machine coordinate
system
The variable returns an undefined value if the encoder limit
frequency is exceeded
This variable can only be accessed from synchronized
actions
Axes: channel axis
15.2.52 Drive data
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_LOAD REAL $AA_LOAD[X] RS R 2
Drive capacity utilization as % (for 611D or PROFIBUS
only)
Axes: channel axis, machine axis
$VA_LOAD REAL $VA_LOAD[X] RS R 5
Drive capacity utilization as % (for 611D or PROFIBUS .
only) 1
Axes: channel axis, machine axis
$AA_TORQUE REAL $AA_TORQUE[X] RS R 2
Drive torque setpoint in Nm (for 611D only)
Force actual value in N (611D-HLA only)
Axes: channel axis, machine axis
$VA_TORQUE REAL $VA_TORQUE[X] RS R 5
Drive torque setpoint in Nm (for 611D only) .
Force actual value in N (611D-HLA only) 1
Axes: channel axis, machine axis
AA_POWER REAL $AA_POWER[x] RS R 2
Drive active power in W (for 611D only)
Axes: channel axis, machine axis
$VA_POWER REAL $VA_POWER[x] RS R 5
Drive active power in W (for 611D only) .
Axes: channel axis, machine axis 1
$AA_CURR REAL $AA_CURR[X] RS R 2
Actual current value of axis or spindle in A (for 611D only)
Axes: channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-687
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$VA_CURR REAL $VA_CURR[X] RS R 5
Actual current value of axis or spindle in A (for 611D only) .
Axes: channel axis, machine axis 1
$VA_DIST_TOR REAL $VA_DIST_TORQUE[X] RS R 6
QUE Disturbing torque/max. motor torque (output of disturbance .
torque observer) 3
Axes: channel axis, machine axis
$VA_VALVELIFT REAL $VA_VALVELIFT[X] RS R 5
Actual valve stroke in mm (for 611D hydraulics only) .
Axes: channel axis, machine axis 1
$VA_PRESSUR REAL $VA_PRESSURE_A[X] RS R 5
E_A Pressure on A side of cylinder in bar (for 611D hydraulics .
only) 1
Axes: channel axis, machine axis
$VA_PRESSUR REAL $VA_PRESSURE_B[X] RS R 5
E_B Pressure on B side of cylinder in bar (for 611D hydraulics .
only) 1
Axes: channel axis, machine axis
$VA_DP_ACT_T INT $VA_DP_ACT_TEL[b,a] RS R 6
EL b: Word index (16-bit access) in PROFIBUS frame .
a: Machine axis 4
b: Word index in PROFIBUS actual value frame
Axes: geometry axis, channel axis, machine axis
15.2.53 Axis statuses
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_STAT INT $AA_STAT[X] RS R 4
Axis status:
0: No axis status available
1: Traversing motion in progress
2: Axis has reached IPO end applies only to axes in the
channel
3: Axis in position (exact stop coarse)for all axes
4: Axis in position (exact stop fine)for all axes
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
15-688 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_SNGLAX_ INT $AA_SNGLAX_STAT[X] RS R 6
STAT Axis status: .
0: Axis is not a single axis 4
1: Single axis in reset
2: Single axis is ended
3: Single axis is interrupted
4: Single axis is active
5: Single axis alarm pending
Axes: geometry axis, channel axis, machine axis
$AA_REF INT $AA_REF[X] RS R 5
Axis status:
0: Axis is not referenced
1: Axis is referenced
Axes: geometry axis, channel axis, machine axis
$AA_TYP INT $AA_TYP[X] RS R 4
Axis type:
0: Axis on other channel
1: Channel axis of local channel
2: Neutral axis
3: PLC axis
4: Oscillating axis
5: Neutral axis currently traversing in JOG mode
6: Master value linked following axis
7: Coupled motion following axis
8: Command axis
9: Compile cycle axis
10: Linked slave axis (master/slave function)
Axes: geometry axis, channel axis
15.2.54 Master/slave links
$AA_MASL_ST INT The current status of a master/slave link. RS R 6
AT Value 0: Axis is no slave axis, or no active link. .
Value > 0: Active link; the associated machine axis number 1
of the master axis is returned.
$AA_MASL_STAT[X]
Axes: geometry axis, channel axis, machine axis
$P_SEARCH_M INT $P_SEARCH_MASLC[axis identifier] R 6
ASLC The current status of a master/slave link was changed in .
search mode. 1
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-689
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_SEARCH_M REAL $P_SEARCH_MASLD[axis identifier] R 6
ASLD In search mode, the positional offset determined when .
closing the link between the master and the slave axis. 1
Axes: geometry axis, channel axis, machine axis
15.2.55 Travel to fixed stop
$AA_FXS INT $AA_FXS[X] RS WS R W 2
Setpoint status state "travel to fixed stop"
0: Axis not at fixed stop
1: Fixed stop successfully approached
2: Fixed stop approach has failed
3: Travel to fixed stop selection active
4: Fixed stop detected
5: Travel to fixed stop deselection active
Axes: geometry axis, channel axis, machine axis
$VA_FXS INT $VA_FXS[X] RS R 6
Actual status state "travel to fixed stop" .
0: Axis not at fixed stop 3
1: Fixed stop successfully approached
2: Fixed stop approach has failed
3: Travel to fixed stop selection active
4: Fixed stop detected
5: Travel to fixed stop deselection active
Axes: geometry axis, channel axis, machine axis
$VA_FXS_INFO INT $VA_FXS_INFO[X] RS R 6
Additional information for "travel to fixed stop" when .
$VA_FXS[]=2 3
0: No additional information available
1: No approach motion programmed
2: Programmed end position reached, motion ended
3: Abort caused by NC reset (pushbutton reset)
4: Exit fixed stop window
5: Drive has refused torque reduction
6: PLC has canceled enabling
Axes: geometry axis, channel axis, machine axis
$VA_TORQUE_ INT $VA_TORQUE_AT_LIMIT[X] RS R 6
AT_LIMIT Status "Torque limit reached" .
0: Torque limit not yet reached 1
1: Torque limit reached
In the digital 611D systems, the drive returns the status
indicating
whether the programmed torque limit has been reached.
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
15-690 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_FOC INT $AA_FOC[X] RS WS R W 6
Setpoint status state "ForceControl" .
0: ForceControl not active 1
1: ForceControl modal active
2: Block-related ForceControl active
Axes: geometry axis, channel axis, machine axis
$VA_FOC INT $VA_FOC[X] RS R 6
Actual status state "ForceControl" .
0: ForceControl not active 3
1: ForceControl modal active
2: Block-related ForceControl active
Axes: geometry axis, channel axis, machine axis
$AA_COUP_ACT INT $AA_COUP_ACT[SPI(2)] RS R 2
Current coupling status of following spindle/following axis:
0: Axis/spindle is not coupled to a leading spindle/leading
axis
3: Tangential follow-up of axis
4: synchronized spindle coupling
8: Axis is trailing
16: Following axis of master value coupling
The respective values apply to one coupling. If several
couplings are active for a following axis, this is represented
by the sum of the relevant numerical values.
Axes: geometry axis, channel axis, machine axis
15.2.56 Electronic gear
AA_EG_SYNFA REAL $AA_EG_SYNFA[a] RS R 5
a: Following axis
Synchronized position of the following axis
Axes: geometry axis, channel axis, machine axis
$P_EG_BC STRING $P_EG_BC[a] R 6
Block change condition for EGONSYN, EGON, WAITC. .
2nd dimension for TYPE_STRING is automatically 1
MAXSTRINGLEN
$AA_EG_NUM_ INT $AA_EG_NUM_LA[a] RS R 5
LA a: Following axis
Number of leading axes specified with EGDEF
Axes: geometry axis, channel axis
$VA_EG_SYNC REAL $VA_EG_SYNCDIFF[a] RS R 5
DIFF a: Following axis
Synchronized run difference
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-691
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$VA_EG_SYNC REAL $VA_EG_SYNCDIFF_S[a] RS R 6
DIFF_S a: Following axis .
Synchronized run difference with sign 4
Axes: geometry axis, channel axis, machine axis
$AA_EG_AX AXIS $AA_EG_AX[n,a] RS R 6
n: Index for leading axis .
a: Following axis 1
Identifier for nth leading axis
n: Index for leading axis (nth leading axis)
Axes: geometry axis, channel axis, machine axis
15.2.57 Leading value coupling
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_LEAD_SP REAL $AA_LEAD_SP[LW] RS WS R W 4
Simulated master value - position
$AA_LEAD_SV REAL $AA_LEAD_SV[LW] RS WS R W 4
Simulated master value - velocity
$AA_LEAD_P_T REAL $AA_LEAD_P_TURN[LW] RS R 4
URN current leading value position parts lost through modulo
reduction.
The actual master value position (which the control uses for
internal calculation) is
$AA_LEAD_P[LW] + $AA_LEAD_P_TURN[LW]
If MV is a modulo axis, $AA_LEAD_P_TURN
is an integral multiple of $MA_MODULO_RANGE.
If MV is not a modulo axis, $AA_LEAD_P_TURN is always
0.
Example_1:
$MA_MODULO_RANGE[LW]=360
$AA_LEAD_P[LW] =290
$AA_LEAD_P_TURN[LW] =720
The actual master value position
(used internally by the control in calculations) is 1010.
Example_2:
$MA_MODULO_RANGE[LW]=360
$AA_LEAD_P[LW] =290
$AA_LEAD_P_TURN[LW] =-360
The actual master value position
(used internally by the control in calculations) is -70.
$AA_LEAD_P REAL $AA_LEAD_P[LW] RS R 4
Current master value - position (modulo-reduced)
If MV is a modulo axis, the following always applies:
0 Coarse synchronism
2 => Fine synchronism
3 => Synchronized run coarse and fine
Axes: geometry axis, channel axis, machine axis
$AA_IN_SYNC INT $AA_IN_SYNC[FA] RS R 6
Synchronization status of the following axis for master value .
coupling and ELG 4
1 => Synchronization in progress, i.e. following axis is
synchronized out
Axes: geometry axis, channel axis, machine axis
15.2.58 Synchronized spindle
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$P_COUP_OFFS REAL $P_COUP_OFFS[S2] R 6
Programmed positional offset for the synchronous spindle .
(following spindle) 3
$AA_COUP_OF REAL $AA_COUP_OFFS[S2] RS R 2
FS Positional offset for synchronous spindle (following spindle)
setpoint value viewpoint
$VA_COUP_OF REAL $VA_COUP_OFFS[SPI(2)] RS R 2
FS Positional offset for synchronous spindle (following spindle)
actual value viewpoint
$AA_SCTRACE BOOL $AA_SCTRACE[X] = 1 RS WS R W 4
Write: Initiate IPO trigger for servo trace
0: No action
!0: Initiate trigger
Read:
Always 0, as the trigger cannot be read back
Axes: geometry axis, channel axis, machine axis
$VA_DPE BOOL $VA_DPE[X1] RS R 5
Status of power enable of a machine axis
Axes: Machine axis
$AA_ACC REAL $AA_ACC RS R 5
Current acceleration value of axis with 1-axis interpolation.
$AA_ACC = $MA_MAX_AX_ACCEL * progr.
acceleration correction
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-693
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$PA_ACCLIMA INT $PA_ACCLIMA R 6
Acceleration override set in preprocessing with ACCLIMA .
Axes: geometry axis, channel axis, machine axis 4
$PA_VELOLIMA INT $PA_VELOLIMA R 6
Velocity override set in preprocessing with VELOLIMA .
Axes: geometry axis, channel axis, machine axis 4
$PA_JERKLIMA INT $PA_JERKLIMA R 6
Jerk override set in preprocessing with JERKLIMA .
Axes: geometry axis, channel axis, machine axis 4
$AA_ACCLIMA INT $AA_ACCLIMA RS R 6
Acceleration override set in main run with ACCLIMA .
Axes: geometry axis, channel axis, machine axis 4
$AA_VELOLIMA INT $AA_VELOLIMA RS R 6
Velocity override set in main run with VELOLIMA .
Axes: geometry axis, channel axis, machine axis 4
$AA_JERKLIMA INT $AA_JERKLIMA RS R 6
Jerk override set in main run with JERKLIMA .
Axes: geometry axis, channel axis, machine axis 4
$AA_MOTEND INT $AA_MOTEND RS R 5
Current motion end criterion at 1-axis interpolation
1 = Motion end at exact stop FINE
2 = Motion end at exact stop COARSE
3 = Motion end at exact stop, IPO stop
4 = Block change in braking ramp of axis motion
5 = Block change in braking ramp of axis motion with
tolerance window with regard to setpoint
6 = Block change in braking ramp of axis motion with
tolerance window with regard to actual value
Axes: geometry axis, channel axis, machine axis
$AA_SCPAR INT $AA_SCPAR RS R 5
Read current servo parameter set
Axes: geometry axis, channel axis, machine axis
$AA_ESR_STAT INT $AA_ESR_STAT[X] RS R 5
Status of "Extended stop and retract", bit-coded:
BIT0: Generator operation triggered
BIT1: Retraction triggered
BIT2: Ext. stop triggered
BIT3: DC link undervoltage
BIT4: Generator minimum speed
Axes: geometry axis, channel axis, machine axis
$AA_ESR_ENA BOOL $AA_ESR_ENABLE[X] = 1 RS WS R W 5
BLE Enable "Extended stop and retract"
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
15-694 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_ESR_TRIG BOOL $AA_ESR_TRIGGER = 1 R W 6
GER Trigger "NC-driven ESR" for PLC controlled axis .
Axes: channel axis 4
$AA_POLFA REAL $AA_POLFA[X] RS R 6
X: Single axis .
returns the programmed return position of the single axis 4
Axes: geometry axis, channel axis, machine axis
$AA_POLFA_VA INT $AA_POLFA_VALID[X] RS R 6
LID X: Retraction programmed for this single axis, returns .
0: Single axis retraction not programmed 4
1: Retraction programmed as position
2: Retraction programmed as distance
Axes: geometry axis, channel axis, machine axis
$AA_ALARM_S INT $AA_ALARM_STAT RS R 6
TAT (Selected) alarm reactions for synchronized actions .
(SYNFCT) 4
Axes: channel axis
$AN_AXCTSWA BOOL EVERY $AN_AXCTSWA[n] == TRUE DO M99 R 5
Read:
TRUE: an axis container rotation is currently being
executed on the container with the axis container name n
FALSE: No active axis container rotation is active
$AN_AXCTAS INT Read: R 5
Axis container rotation current rotation:
The number of slots the axis container has currently been
advanced is indicated for the axis container with axis
container name n.
The value range is from 0 to the maximum number of
assigned slots in axis container -1
$AC_AXCTSWA BOOL IF $AC_AXCTSWA[n] == TRUE GOTOB MARK1 R 5
Read:
TRUE: The channel has enabled axis container rotation for
the axis container name n and the rotation has not yet been
completed.
FALSE: The axis container rotation is terminated.
$AA_EG_TYPE INT $AA_EG_TYPE[a,b] RS R 6
a: Following axis .
b: Leading axis 1
Type of coupling for leading axis b
0: Actual-value coupling
1: Setpoint linkage
Axes: geometry axis, channel axis, machine axis
$AA_EG_NUME REAL $AA_EG_NUMERA[a,b] RS R 6
RA a: Following axis .
b: Leading axis 1
Numerator of coupling factor for leading axis b
Axes: geometry axis, channel axis, machine axis
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-695
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$AA_EG_DENOM REAL $AA_EG_DENOM[a,b] RS R 6
a: Following axis .
b: Leading axis 1
Denominator of coupling factor for leading axis b
Axes: geometry axis, channel axis, machine axis
$AA_EG_SYN REAL $AA_EG_SYN[a,b] RS R 6
a: Following axis .
b: Leading axis 1
Synchronized position of leading axis b
Axes: geometry axis, channel axis, machine axis
$AA_EG_ACTIVE BOOL $AA_EG_ACTIVE[a,b] RS R 6
a: Following axis .
b: Leading axis 1
Coupling for leading axis b is active, i.e. switched on
Axes: geometry axis, channel axis, machine axis
15.2.59 Safety Integrated
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$A_STOPESI INT Current Safety Integrated Stop E for any axis: RS R 6
Value 0: no Stop E .
Value not equal to 0: There is currently a Stop E at one of 4
the axes
$A_INSE BOOL $A_INSE[n] RS R 6
Image of a Safety input signal (ext. NCK interface) .
n: Number of input 1 - ... 3
$A_INSED INT $A_INSED[n] RS R 6
Image of Safety input signals (ext. NCK interface) .
n: Number of input word 1 - ... 3
$A_INSEP BOOL $A_INSEP[n] RS R 6
Image of a Safety input signal (ext. PLC interface) .
n: Number of input 1 - ... 4
$A_INSEPD INT $A_INSEPD[n] RS R 6
Image of Safety input signals (ext. PLC interface) .
n: Number of input word 0 - ... 3
$A_OUTSE BOOL $A_OUTSE[n] RS WS R W 6
Image of a Safety output signal (ext. NCK interface) .
n: Number of output 1 - ... 4
$A_OUTSED INT $A_OUTSED[n] RS WS R W 6
Image of Safety output signals (ext. NCK interface) .
n: Number of output word 1 - ... 3
$A_OUTSEP BOOL $A_OUTSEP[n] RS R 6
Image of a Safety output signal (ext. PLC interface) .
n: Number of output 1 - ... 3
Siemens AG, 2002. All rights reserved
15-696 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$A_OUTSEPD INT $A_OUTSEPD[n] RS R 6
Image of Safety output signals (ext. PLC interface) .
n: Number of output word 0 - ... 4
$A_INSI BOOL $A_INSI[n] RS R 6
Image of a Safety input signal (int. NCK interface) .
n: Number of input 1 - ... 3
$A_INSID INT $A_INSID[n] RS R 6
Image of Safety input signals (int. NCK interface) .
n: Number of input word 1 - ... 4
$A_INSIP BOOL $A_INSIP[n] RS R 6
Image of a Safety input signal (int. PLC interface) .
n: Number of input word 1 - ... 4
$A_INSIPD INT $A_INSIPD[n] RS R 6
Image of Safety input signals (int. PLC interface) .
n: Number of input word 1 - ... 4
$A_OUTSI BOOL $A_OUTSI[n] RS WS R W 6
Image of a Safety output signal (int. NCK interface) .
n: Number of output 1 - ... 4
$A_OUTSID INT $A_OUTSID[n] RS WS R W 6
Image of Safety output signals (int. NCK interface) .
n: Number of output word 1 - ... 3
$A_OUTSIP BOOL $A_OUTSIP[n] RS R 6
Image of a Safety output signal (int. PLC interface) .
n: Number of output 1 - ... 3
$A_OUTSIPD INT $A_OUTSIPD[n] RS R 6
Image of Safety output signals (int. PLC interface) .
n: Number of output word 1 - ... 3
$A_MARKERSI BOOL $A_MARKERSI[n] RS WS R W + 6
Markers for Safety programming .
n: Number of marker 1 - ... 3
$A_MARKERSID INT $A_MARKERSID[n] RS WS R W + 6
Marker word (32 bits) for Safety programming .
n: Number of marker word 1 - ... 3
$A_MARKERSIP BOOL $A_MARKERSIP[n] RS R + 6
Image of PLC Safety markers .
n: Number of marker 1 - ... 3
$A_MARKERSI INT $A_MARKERSIPD[n] RS R + 6
PD Image of PLC Safety marker words .
n: Number of marker word 1 - ... 3
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-697
15 Tables 11.0215.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$A_TIMERSI REAL $A_TIMERSI[n] RS WS R W + 6
Safety timer - unit in seconds .
Time is counted internally in multiples of the interpolation 3
cycle;
Counting for the time variable is started by assigning the
value
$A_TIMERSI[n]=
To stop the counter variable, assign a negative value:
$A_TIMERSI[n]=-1
The current time can be read while the counter is active or
stopped. Stopping the counter variable, by assigning -1
stops the last current time value which can then be read
n: Number of timer 1 - ...
$A_STATSID INT $A_STATSID RS R 6
Safety: Status of cross-checking between NCK and PLC. .
If value is not equal to zero, there is a cross-checking error 3
$A_CMDSI BOOL $A_CMDSI[n] RS WS R W + 6
Safety: Control word for cross-checking between NCK and .
PLC. 3
Array index n = 1: Increase timer for signal change
monitoring to 10s
n: Number of control signal for cross-checking NCK - PLC
$A_LEVELSID INT $A_LEVELSID RS R 6
Safety: Display of signal change monitoring level. Indicates .
the current number of signals marked for cross-checking. 3
$A_XFAULTSI INT Information on Safety Integrated Stop F for an axis: RS R 6
Bit 0 is set: .
During crosschecking between NCK and 611D, an actual 4
value error has been discovered on an axis.
Bit 1 is set:
During crosschecking between NCK and 611D, an error has
been discovered on an axis and the wait time before Stop B
is triggered is running or has expired
($MA_SAFE_STOP_SWITCH_TIME_F).
$A_PLCSIIN BOOL $A_PLCSIIN[n] Communication from PLC-SPL to NCK-SPL RS R + 6
n: Number of signal 1 - ... from the PLC .
4
$A_PLCSIOUT BOOL $A_PLCSIOUT[n] Communication from NCK-SPL to PLC- RS WS R W + 6
SPL .
n: Number of signal 1 - ... to the PLC 4
Siemens AG, 2002. All rights reserved
15-698 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
15 11.02 Tables15.2 List of system variables 15
Identifier Type Description: System variable/value range/index Parts pr. Sync O S
$VA_IS REAL $VA_IS[X] RS R 6
Reliable actual position (SISITEC) .
Axes: geometry axis, channel axis, machine axis 4
$VA_STOPSI INT $VA_STOPSI[X] RS R 6
Current Safety Integrated Stop for the particular axis .
Value Meaning 4
-1 No stop
0 Stop A
1 Stop B
2 Stop C
3 Stop D
4 Stop E
5 Stop F
10 Test stop NC
11 Test ext. pulse suppression
Axes: geometry axis, channel axis, machine axis
$VA_XFAULTSI INT Information on Safety Integrated Stop F for this axis: R 6
Bit 0 is set: .
During crosschecking between NCK and 611D, an actual 4
value error has been discovered.
Bit 1 is set:
During crosschecking between NCK and 611D, an error has
been discovered and the wait time before
Stop B ($MA_SAFE_STOP_SWITCH_TIME_F) is triggered
is running or has expired
Axes: geometry axis, channel axis, machine axis
▀
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition 15-699
15 Tables 11.0215.2 List of system variables 15
Siemens AG, 2002. All rights reserved
15-700 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 Appendix A
Appendix
A Index ..............................................................................................................................A-702
B Commands, Identifiers....................................................................................................A-719
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-701
A Appendix 11.02Index A
A Index
$A_OUTA 15-657
$ $A_OUTSE 15-696
$A_OUTSED 15-696
$A_CMDSI 15-698 $A_OUTSEP 15-696
$A_DAY 15-662 $A_OUTSEPD 15-697
$A_DBB 15-657 $A_OUTSI 15-697
$A_DBD 15-657 $A_OUTSID 15-697
$A_DBR 15-657 $A_OUTSIP 15-697
$A_DBW 15-657 $A_OUTSIPD 15-697
$A_DLB 15-658 $A_PBB_IN 15-658
$A_DLD 15-658 $A_PBB_OUT 15-659
$A_DLR 15-658 $A_PBD_IN 15-658
$A_DLW 15-658 $A_PBD_OUT 15-659
$A_DNO 15-646 $A_PBR_IN 15-658
$A_GG 15-647 $A_PBR_OUT 15-659
$A_HOUR 15-662 $A_PBW_IN 15-658
$A_IN 15-657 $A_PBW_OUT 15-659
$A_INA 15-657 $A_PLCSIIN 15-698
$A_INCO 15-657 $A_PLCSIOUT 15-698
$A_INSE 15-696 $A_PROBE 15-652
$A_INSED 15-696 $A_PROTO 15-655
$A_INSEP 15-696 $A_PROTOC 15-655
$A_INSEPD 15-696 $A_SECOND 15-662
$A_INSI 15-697 $A_STATSID 15-698
$A_INSID 15-697 $A_STOPESI 15-696
$A_INSIP 15-697 $A_TIMERSI 15-698
$A_INSIPD 15-697 $A_TOOLMLN 15-641
$A_LEVELSID 15-698 $A_TOOLMN 15-641
$A_LINK_TRANS_RATE 15-658 $A_XFAULTSI 15-698
$A_MARKERSI 15-697 $A_YEAR 15-662
$A_MARKERSID 15-697 $AA_ACC 15-693
$A_MARKERSIP 15-697 $AA_ACCLIMA 15-694
$A_MARKERSIPD 15-697 $AA_ACT_INDEX_AX_POS_NO 15-679
$A_MINUTE 15-662 $AA_ALARM_STAT 15-695
$A_MONIFACT 15-641 $AA_COUP_ACT 9-361, 9-378, 13-503, 15-691
$A_MONTH 15-662 $AA_COUP_OFFS 13-503, 15-693
$A_MSECOND 15-662 $AA_CURR 15-687
$A_MYMLN 15-641 $AA_DELT 15-685
$A_MYMN 15-641 $AA_DTBB 15-684
$A_OUT 15-657 $AA_DTBW 15-684
Siemens AG, 2002. All rights reserved
A-702 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
$AA_DTEB 15-684 $AA_MEAS_P4_VALID 15-681
$AA_DTEPB 15-685 $AA_MEAS_POINT1 15-681
$AA_DTEPW 15-685 $AA_MEAS_POINT2 15-681
$AA_DTEW 15-684 $AA_MEAS_POINT3 15-682
$AA_EG_ACTIVE 15-696 $AA_MEAS_POINT4 15-682
$AA_EG_AX 15-692 $AA_MEAS_SETANGLE 15-682
$AA_EG_DENOM 15-696 $AA_MEAS_SETPOINT 15-682
$AA_EG_NUM_LA 15-691 $AA_MEAS_SP_VALID 15-682
$AA_EG_NUMERA 15-695 $AA_MM 15-680
$AA_EG_SYN 15-696 $AA_MM1 15-680
$AA_EG_SYNFA 15-691 $AA_MM2 15-680
$AA_EG_TYPE 15-695 $AA_MM3 15-680
$AA_ENC_ACTIVE 15-679 $AA_MM4 15-681
$AA_ENC_COMP 15-626 $AA_MOTEND 5-230, 15-694
$AA_ENC_COMP_IS_MODULO 15-627 $AA_MW 15-680
$AA_ENC_COMP_MAX 15-627 $AA_MW1 15-680
$AA_ENC_COMP_MIN 15-627 $AA_MW2 15-680
$AA_ENC_COMP_STEP 15-626 $AA_MW3 15-680
$AA_ENC1_ACTIVE 15-679 $AA_MW4 15-680
$AA_ENC2_ACTIVE 15-679 $AA_OFF 15-682
$AA_ESR_ENABLE 15-694 $AA_OFF_LIMIT 15-682
$AA_ESR_STAT 15-694 $AA_OFF_VAL 15-682
$AA_ESR_TRIGGER 15-695 $AA_OSCILL_REVERSE_POS1 15-685
$AA_ETRANS 15-681 $AA_OSCILL_REVERSE_POS2 15-685
$AA_FOC 15-691 $AA_OVR 15-686
$AA_FXS 15-690 $AA_POLFA 15-695
$AA_IB 15-678 $AA_POLFA_VALID 15-695
$AA_IBN 15-678 $AA_POWER 15-687
$AA_IEN 15-678 $AA_PROG_INDEX_AX_POS_NO 15-679
$AA_IM 15-678 $AA_QEC 15-627
$AA_IN_SYNC 15-693 $AA_QEC_ACCEL_1 15-627
$AA_IW 15-678 $AA_QEC_ACCEL_2 15-628
$AA_JERKLIMA 15-694 $AA_QEC_ACCEL_3 15-628
$AA_LEAD_P 15-692 $AA_QEC_COARSE_STEPS 15-627
$AA_LEAD_P_TURN 15-692 $AA_QEC_DIRECTIONAL 15-628
$AA_LEAD_SP 9-378, 15-692 $AA_QEC_FINE_STEPS 15-627
$AA_LEAD_SV 9-378, 15-692 $AA_QEC_LEARNING_RATE 15-628
$AA_LEAD_V 15-693 $AA_QEC_MEAS_TIME_1 15-628
$AA_LOAD 15-687 $AA_QEC_MEAS_TIME_2 15-628
$AA_MASL_STAT 15-689 $AA_QEC_MEAS_TIME_3 15-628
$AA_MEAACT 15-681 $AA_QEC_TIME_1 15-628
$AA_MEAS_P1_VALID 15-681 $AA_QEC_TIME_2 15-628
$AA_MEAS_P2_VALID 15-681 $AA_REF 15-689
$AA_MEAS_P3_VALID 15-681 $AA_REPOS_DELAY 15-678
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-703
A Appendix 11.02Index A
$AA_S 15-667 $AC_FCT3 15-671
$AA_SCPAR 5-232, 15-694 $AC_FCT3C 15-670
$AA_SCTRACE 15-693 $AC_FCT3LL 15-670
$AA_SNGLAX_STAT 15-689 $AC_FCT3UL 15-670
$AA_SOFTENDN 15-683 $AC_FCTLL 15-670
$AA_SOFTENDP 15-683 $AC_FCTUL 15-670
$AA_STAT 15-688 $AC_FIFO1 15-656
$AA_SYNC 15-693 $AC_FIFO2 15-656
$AA_TOFF 15-683 $AC_FIFO3 15-656
$AA_TOFF_LIMIT 15-683 $AC_G0MODE 15-673
$AA_TOFF_PREP_DIFF 15-683 $AC_IPO_BUF 15-651
$AA_TOFF_VAL 15-683 $AC_IW_STAT 15-651
$AA_TORQUE 15-687 $AC_IW_TU 15-651
$AA_TYP 15-689 $AC_JOG_COORD 15-652
$AA_VACTB 15-686 $AC_LIFTFAST 15-652
$AA_VACTM 15-687 $AC_MARKER 15-591
$AA_VACTW 15-686 $AC_MEA 15-652
$AA_VC 15-686 $AC_MEAS_ACT_PLANE 15-674
$AA_VELOLIMA 15-694 $AC_MEAS_CHBFR 15-674
$AC_ACTUAL_PARTS 15-672 $AC_MEAS_CHSFR 15-674
$AC_ALARM_STAT 15-672 $AC_MEAS_CORNER_ANGLE 15-676
$AC_ASUB 15-654 $AC_MEAS_CORNER_SETANGLE 15-674
$AC_AXCTSWA 15-695 $AC_MEAS_D_NUMBER 15-675
$AC_BLOCKTYPE 15-651 $AC_MEAS_DIAMETER 15-676
$AC_CONSTCUT_S 15-667 $AC_MEAS_DIR_APPROACH 15-674
$AC_CUTTING_TIME 15-672 $AC_MEAS_FINE_TRANS 15-674
$AC_CYCLE_TIME 15-672 $AC_MEAS_FRAME 15-676
$AC_DELT 15-665 $AC_MEAS_FRAME_SELECT 15-674
$AC_DRF 15-681 $AC_MEAS_LATCH 15-673
$AC_DTBB 15-664 $AC_MEAS_NCBFR 15-674
$AC_DTBW 15-663 $AC_MEAS_P1_COORD 15-673
$AC_DTEB 15-664 $AC_MEAS_P2_COORD 15-673
$AC_DTEW 15-664 $AC_MEAS_P3_COORD 15-673
$AC_ESR_TRIGGER 15-672 $AC_MEAS_P4_COORD 15-673
$AC_F 15-665 $AC_MEAS_PFRAME 15-675
$AC_FCT0 15-671 $AC_MEAS_RESULTS 15-677
$AC_FCT1 15-671 $AC_MEAS_SCALEUNIT 15-677
$AC_FCT1C 15-670 $AC_MEAS_SEMA 15-673
$AC_FCT1LL 15-670 $AC_MEAS_SET_COORD 15-673
$AC_FCT1UL 15-670 $AC_MEAS_T_NUMBER 15-675
$AC_FCT2 15-671 $AC_MEAS_TOOL_LENGTH 15-676
$AC_FCT2C 15-670 $AC_MEAS_TOOL_MASK 15-675
$AC_FCT2LL 15-670 $AC_MEAS_TYPE 15-675
$AC_FCT2UL 15-670 $AC_MEAS_UIFR 15-674
Siemens AG, 2002. All rights reserved
A-704 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
$AC_MEAS_VALID 15-676 $AC_TC_LTO 15-661
$AC_MEAS_WP_ANGLE 15-676 $AC_TC_MFN 15-660
$AC_MEAS_WP_SETANGLE 15-674 $AC_TC_MFO 15-661
$AC_MONMIN 15-646 $AC_TC_MMYN 15-660
$AC_MSNUM 15-669 $AC_TC_MTN 15-661
$AC_MTHNUM 15-670 $AC_TC_MTO 15-661
$AC_OPERATING_TIME 15-672 $AC_TC_STATUS 15-660
$AC_OVR 15-665 $AC_TC_THNO 15-660
$AC_PARAM 15-591 $AC_TC_TNO 15-660
$AC_PATHACC 15-666 $AC_TIME 15-662
$AC_PATHJERK 15-666 $AC_TIMEC 15-662
$AC_PATHN 15-663 $AC_TIMER 15-662
$AC_PLTBB 15-664 $AC_TOOLO_ACT 15-639
$AC_PLTEB 15-664 $AC_TOOLO_DIFF 15-639
$AC_PRESET 15-681 $AC_TOOLO_END 15-639
$AC_PROG 15-651 $AC_TOTAL_PARTS 15-672
$AC_PRTIME_A 15-663 $AC_TRAFO 15-652
$AC_PRTIME_A_INC 15-663 $AC_TRAFO_PAR 15-652
$AC_PRTIME_M 15-663 $AC_TRAFO_PARSET 15-652
$AC_PRTIME_M_INC 15-663 $AC_TRANS_SYS 15-651
$AC_REPOS_PATH_MODE 15-664 $AC_VACTB 15-666
$AC_REQUIRED_PARTS 15-672 $AC_VACTW 15-666
$AC_RETPOINT 15-683 $AC_VC 15-666
$AC_ROT_SYS 15-652 $AN_AXCTAS 15-695
$AC_SDIR 15-667 $AN_AXCTSWA 15-695
$AC_SERUPRO 15-677 $AN_BUS_FAIL_TRIGGER 15-672
$AC_SGEAR 15-668 $AN_CEC 15-629
$AC_SMODE 15-668 $AN_CEC_DIRECTION 15-629
$AC_SPECIAL_PARTS 15-672 $AN_CEC_INPUT_AXIS 15-629
$AC_STAT 15-651 $AN_CEC_IS_MODULO 15-629
$AC_SYNA_MEM 15-651 $AN_CEC_MAX 15-629
$AC_SYSTEM_MARKER 15-592 $AN_CEC_MIN 15-629
$AC_SYSTEM_PARAM 15-591 $AN_CEC_MULT_BY_TABLE 15-629
$AC_TANEB 15-651 $AN_CEC_OUTPUT_AXIS 15-629
$AC_TC 15-640 $AN_CEC_STEP 15-629
$AC_TC_ACKC 15-660 $AN_ESR_TRIGGER 15-672
$AC_TC_ACKT 15-659 $AN_NCK_VERSION 15-636
$AC_TC_CMDC 15-660 $AN_POWERON_TIME 15-636
$AC_TC_CMDT 15-659 $AN_SETUP_TIME 15-636
$AC_TC_FCT 15-660 $C_A 15-631
$AC_TC_LFN 15-660 $C_A_PROG 15-633
$AC_TC_LFO 15-661 $C_ALL_PROG 15-634
$AC_TC_LMYN 15-660 $C_B 15-631
$AC_TC_LTN 15-661 $C_B_PROG 15-633
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-705
A Appendix 11.02Index A
$C_DL 15-632 $P_CHBFRMASK 15-637
$C_DL_PROG 15-633 $P_CONSTCUT_S 15-667
$C_H 15-631 $P_COUP_OFFS 15-693
$C_I 15-632 $P_CTABDEF 15-648
$C_I_NUM 15-634 $P_CYCFR 15-592
$C_I_ORDER 15-635 $P_CYCFRAME 15-636
$C_IN 15-659 $P_D 15-641
$C_INC_PROG 15-634 $P_DLNO 15-638
$C_J 15-632 $P_DRYRUN 15-649
$C_J_NUM 15-634 $P_EG_BC 15-691
$C_J_ORDER 15-635 $P_EP 15-677
$C_K 15-632 $P_EPM 15-678
$C_K_NUM 15-634 $P_EXTFR 15-592
$C_K_ORDER 15-635 $P_EXTFRAME 15-636
$C_L 15-632 $P_EXTGG 15-647
$C_M 15-632 $P_F 15-665
$C_MACPAR 15-635 $P_FA 15-685
$C_ME 15-635 $P_GG 15-647
$C_OUT 15-659 $P_GWPS 15-670
$C_TE 15-635 $P_H 15-641
$C_TS 15-632 $P_IFRAME 15-637
$C_TS_PROG 15-634 $P_ISTEST 15-655
$C_TYP_PROG 15-634 $P_LIFTFAST 15-653
$C_Z 15-632 $P_MAG 15-643
$C_Z_PROG 15-633 $P_MAGA 15-645
$MC_COMPESS_VELO_TOL. 9-384 $P_MAGDISL 15-644
$P_ACTBFRAME 15-637 $P_MAGDISS 15-643
$P_ACTFRAME 15-637 $P_MAGHLT 15-645
$P_ACTGEOAX 15-647 $P_MAGN 15-643
$P_ACTID 15-650 $P_MAGNA 15-645
$P_AD 15-638 $P_MAGNDIS 15-643
$P_ADT 15-638 $P_MAGNH 15-645
$P_AEP 15-678 $P_MAGNHLT 15-645
$P_AP 15-646 $P_MAGNREL 15-644
$P_APDV 15-665 $P_MAGNS 15-644
$P_APR 15-678 $P_MAGREL 15-644
$P_ATPG 15-646 $P_MAGS 15-644
$P_AXN1 15-646 $P_MC 15-648
$P_AXN2 15-646 $P_MMCA 15-655
$P_AXN3 15-647 $P_MSNUM 15-669
$P_BFRAME 15-637 $P_MTHNUM 15-669
$P_CHANNO 15-677 $P_MTHSDC 15-645
$P_CHBFR 15-592 $P_NCBFR 15-593
$P_CHBFRAME 15-637 $P_NCBFRAME 15-637
Siemens AG, 2002. All rights reserved
A-706 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
$P_NCBFRMASK 15-637 $P_TOOLFRAME 15-636
$P_NUM_SPINDLES 15-669 $P_TOOLL 15-639
$P_OFFN 15-649 $P_TOOLND 15-641
$P_PARTFR 15-592 $P_TOOLNDL 15-642
$P_PARTFRAME 15-636 $P_TOOLNG 15-642
$P_PFRAME 15-637 $P_TOOLNO 15-639
$P_POLF 15-678 $P_TOOLNT 15-642
$P_POLF_VALID 15-678 $P_TOOLO 15-639
$P_PROG 15-649 $P_TOOLP 15-639
$P_PROG_EVENT 15-649 $P_TOOLR 15-640
$P_PROGPATH 15-649 $P_TOOLT 15-642
$P_REPINF 15-648 $P_TRAFO 15-652
$P_S 15-667 $P_TRAFO_PAR 15-652
$P_SAUTOGEAR 15-668 $P_TRAFO_PARSET 15-652
$P_SDIR 15-667 $P_TRAFR 15-593
$P_SEARCH 15-647 $P_UBFR 15-636
$P_SEARCH_MASLC 15-689 $P_UIFR 15-592
$P_SEARCH_MASLD 15-690 $P_UIFRNUM 15-637
$P_SEARCH_S 15-667 $P_USEKT 15-642
$P_SEARCH_SDIR 15-667 $P_VDITCP 15-646
$P_SEARCH_SGEAR 15-669 $P_WPFR 15-592
$P_SEARCH_SPOS 15-669 $P_WPFRAME 15-636
$P_SEARCH_SPOSMODE 15-669 $PA_ACCLIMA 15-694
$P_SEARCH1 15-647 $PA_JERKLIMA 15-694
$P_SEARCH2 15-647 $PA_VELOLIMA 15-694
$P_SEARCHL 15-648 $PI 15-649
$P_SETFR 15-592 $SA_LEAD_TYPE 9-377, 9-378
$P_SETFRAME 15-636 $SC_PA_ACTIV_IMMED 15-601
$P_SGEAR 15-668 $SC_PA_CENT_ABS 15-603
$P_SIM 15-648 $SC_PA_CENT_ORD 15-603
$P_SMODE 15-668 $SC_PA_CONT_ABS 15-603
$P_STACK 15-649 $SC_PA_CONT_NUM 15-602
$P_SUBPAR 15-648 $SC_PA_CONT_ORD 15-602
$P_TC 15-640 $SC_PA_CONT_TYP 15-602
$P_TCANG 15-640 $SC_PA_LIM_3DIM 15-602
$P_TCDIFF 15-640 $SC_PA_MINUS_LIM 15-602
$P_TCSOL 15-640 $SC_PA_ORI 15-602
$P_TCSTAT 15-640 $SC_PA_PLUS_LIM 15-602
$P_TOOL 15-638 $SC_PA_T_W 15-601
$P_TOOLD 15-642 $SN_PA_ACTIV_IMMED 15-630
$P_TOOLENV 15-646 $SN_PA_CENT_ABS 15-631
$P_TOOLENVN 15-646 $SN_PA_CENT_ORD 15-631
$P_TOOLEXIST 15-641 $SN_PA_CONT_ABS 15-631
$P_TOOLFR 15-592 $SN_PA_CONT_NUM 15-630
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-707
A Appendix 11.02Index A
$SN_PA_CONT_ORD 15-631 $TC_CARR37 15-601
$SN_PA_CONT_TYP 15-631 $TC_CARR38 15-601
$SN_PA_LIM_3DIM 15-630 $TC_CARR39 15-601
$SN_PA_MINUS_LIM 15-630 $TC_CARR4 15-594
$SN_PA_ORI 15-630 $TC_CARR40 15-601
$SN_PA_PLUS_LIM 15-630 $TC_CARR5 15-594
$SN_PA_T_W 15-630 $TC_CARR6 15-594
$TC_ADPT1 15-626 $TC_CARR7 15-594
$TC_ADPT2 15-626 $TC_CARR8 15-594
$TC_ADPT3 15-626 $TC_CARR9 15-594
$TC_ADPTT 15-626 $TC_DP1 15-603
$TC_CARR1 15-593 $TC_DP10 15-604
$TC_CARR1...14 8-346 $TC_DP11 15-605
$TC_CARR10 15-594 $TC_DP12 15-605
$TC_CARR11 15-594 $TC_DP13 15-605
$TC_CARR12 15-595 $TC_DP14 15-605
$TC_CARR13 15-595 $TC_DP15 15-605
$TC_CARR14 15-595 $TC_DP16 15-605
$TC_CARR15 15-595 $TC_DP17 15-606
$TC_CARR16 15-595 $TC_DP18 15-606
$TC_CARR17 15-595 $TC_DP19 15-606
$TC_CARR18 15-595 $TC_DP2 15-603
$TC_CARR18[m] 8-346 $TC_DP20 15-606
$TC_CARR19 15-595 $TC_DP21 15-606
$TC_CARR2 15-593 $TC_DP22 15-606
$TC_CARR20 15-595 $TC_DP23 15-607
$TC_CARR21 15-596 $TC_DP24 15-607
$TC_CARR22 15-596 $TC_DP25 15-607
$TC_CARR23 15-596 $TC_DP3 15-603
$TC_CARR24 15-596 $TC_DP4 15-604
$TC_CARR24[m] 8-348 $TC_DP5 15-604
$TC_CARR25 15-596 $TC_DP6 15-604
$TC_CARR26 15-596 $TC_DP7 15-604
$TC_CARR27 15-597 $TC_DP8 15-604
$TC_CARR28 15-597 $TC_DP9 15-604
$TC_CARR29 15-598 $TC_DPC1 15-609
$TC_CARR3 15-594 $TC_DPC10 15-609
$TC_CARR30 15-598 $TC_DPC2 15-609
$TC_CARR31 15-598 $TC_DPC3 15-609
$TC_CARR32 15-599 $TC_DPCE 15-607
$TC_CARR33 15-599 $TC_DPCS1 15-610
$TC_CARR34 15-600 $TC_DPCS10 15-610
$TC_CARR35 15-600 $TC_DPCS2 15-610
$TC_CARR36 15-600 $TC_DPCS3 15-610
Siemens AG, 2002. All rights reserved
A-708 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
$TC_DPH 15-607 $TC_MLSR 15-624
$TC_DPV 15-607 $TC_MOP1 15-617
$TC_DPV3 15-608 $TC_MOP11 15-617
$TC_DPV4 15-608 $TC_MOP13 15-617
$TC_DPV5 15-608 $TC_MOP15 15-617
$TC_ECP13 15-614 $TC_MOP2 15-617
$TC_ECP14 15-614 $TC_MOP3 15-617
$TC_ECP21 15-614 $TC_MOP4 15-617
$TC_ECP23 15-614 $TC_MOP5 15-617
$TC_ECP24 15-614 $TC_MOP6 15-617
$TC_ECP31 15-614 $TC_MOPC1 15-618
$TC_ECP33 15-615 $TC_MOPC10 15-618
$TC_ECP34 15-615 $TC_MOPC2 15-618
$TC_ECP41 15-615 $TC_MOPCS1 15-618
$TC_ECP43 15-615 $TC_MOPCS10 15-618
$TC_ECP44 15-615 $TC_MOPCS2 15-618
$TC_ECP51 15-615 $TC_MPP1 15-622
$TC_ECP53 15-616 $TC_MPP2 15-622
$TC_ECP54 15-616 $TC_MPP3 15-622
$TC_ECP61 15-616 $TC_MPP4 15-622
$TC_ECP63 15-616 $TC_MPP5 15-622
$TC_ECP64 15-616 $TC_MPP6 15-622
$TC_ECP71 15-616 $TC_MPP66 15-622
$TC_MAMP1 15-626 $TC_MPP7 15-622
$TC_MAMP2 15-626 $TC_MPPC1 15-623
$TC_MAMP3 15-626 $TC_MPPC10 15-623
$TC_MAP1 15-624 $TC_MPPC2 15-623
$TC_MAP10 15-625 $TC_MPPCS1 15-623
$TC_MAP2 15-624 $TC_MPPCS10 15-623
$TC_MAP3 15-624 $TC_MPPCS2 15-623
$TC_MAP4 15-624 $TC_MPTH 15-624
$TC_MAP5 15-624 $TC_SCP13 15-611
$TC_MAP6 15-624 $TC_SCP14 15-611
$TC_MAP7 15-625 $TC_SCP21 15-611
$TC_MAP8 15-625 $TC_SCP23 15-611
$TC_MAP9 15-625 $TC_SCP24 15-611
$TC_MAPC1 15-625 $TC_SCP31 15-611
$TC_MAPC10 15-625 $TC_SCP33 15-612
$TC_MAPC2 15-625 $TC_SCP34 15-612
$TC_MAPCS1 15-625 $TC_SCP41 15-612
$TC_MAPCS10 15-625 $TC_SCP43 15-612
$TC_MAPCS2 15-625 $TC_SCP44 15-612
$TC_MDP1 15-623 $TC_SCP51 15-612
$TC_MDP2 15-623 $TC_SCP53 15-613
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-709
A Appendix 11.02Index A
$TC_SCP54 15-613 $VA_IS 15-699
$TC_SCP61 15-613 $VA_LOAD 15-687
$TC_SCP63 15-613 $VA_POWER 15-687
$TC_SCP64 15-613 $VA_PRESSURE_A 15-688
$TC_SCP71 15-613 $VA_PRESSURE_B 15-688
$TC_TP1 15-619 $VA_STOPSI 15-699
$TC_TP10 15-619 $VA_TORQUE 15-687
$TC_TP11 15-619 $VA_TORQUE_AT_LIMIT 15-690
$TC_TP2 15-619 $VA_VACTM 15-687
$TC_TP3 15-619 $VA_VALVELIFT 15-688
$TC_TP4 15-619 $VA_XFAULTSI 15-699
$TC_TP5 15-619 $VC_TOOLO 15-639
$TC_TP6 15-619 $VC_TOOLO_DIFF 15-640
$TC_TP7 15-619 $VC_TOOLO_STAT 15-640
$TC_TP8 15-619
$TC_TP9 15-619
$TC_TPC1 15-619
$TC_TPC10 15-620
$TC_TPC2 15-620
$TC_TPCS1 15-620
$TC_TPCS10 15-620
$TC_TPCS2 15-620
$TC_TPG1 15-621
$TC_TPG2 15-621
$TC_TPG3 15-621
$TC_TPG4 15-621
$TC_TPG5 15-621
$TC_TPG6 15-621
$TC_TPG7 15-621
$TC_TPG8 15-621
$TC_TPG9 15-621
$VA_COUP_OFFS 15-693
$VA_CURR 15-688
$VA_DIST_TORQUE 15-688
$VA_DP_ACT_TEL 15-688
$VA_DPE 15-693
$VA_EG_SYNCDIFF 15-691
$VA_EG_SYNCDIFF_S 15-692
$VA_FOC 15-691
$VA_FXS 15-690
$VA_FXS_INFO 15-690
$VA_IM 15-679
$VA_IM1 15-680
$VA_IM2 15-680
Siemens AG, 2002. All rights reserved
A-710 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
B
A Backlash 13-493
Actual value and setpoint coupling 9-376 Block display 2-121, 2-125
Actual-value coupling 13-495 Block search 10-452
Adaptive control, additive 10-424
Adaptive control, multiplicative 10-425 C
Angle of rotation α1, α2 8-346
Calculate circle data 14-557
Angle offset/angle increment of the rotary axes
Calculate intersection of two contour elements
8-348
14-542
Angle reference 13-501
Calling frame 6-244
Approaching coded positions 5-186
Calling up a program in ISO language indirectly
Arithmetic functions 1-46
with ISOCALL 2-121
Arithmetic operations/functions 1-46
CANCEL 10-453
Arithmetic parameter 1-26
Cancel synchronized action 10-449
Array definition 1-34
CASE instruction 1-65
Array definition, value lists 1-36
Channel-specific frames 6-257
Array index 1-35
CHECKSUM 1-98
Assign and start interrupt routine 1-79
Circular interpolation 5-212
Assignments 1-45
Circumferential milling 8-328
ASUB 10-452
Clamping axis/spindle 13-526
Asynchronized oscillation 11-456
Clearance control 10-426
Automatic "GET" 1-87
Coarse offset 6-248
Automatic path segmentation 12-480
Command axes 10-430
Auxiliary functions 10-415
Command elements 10-397
Auxiliary functions 12-480
Comparison and logic operators 1-48
Axial feed 10-433
Priority of operators 1-53
Axial leading value coupling 9-375
Compressor 5-196, 5-211
Axis
Compressor for orientations
Container 13-526
COMPON, COMPCURV 5-197
Local 13-526
Computing capacity 13-522
Axis container 13-526, 13-528
Concatenation of strings 1-58
Axis coordination 10-434
Constraints for transformations 7-302
Axis functions 13-489
Contour element 14-546, 14-548
Axis transfer
Contour elements, intersection 14-554
Release axis 1-86
Contour preparation
Axis transfer
Relief cut elements 14-544
GET 1-85
Contour preparation 14-543, 14-550
Get axis 1-86
Contour table 14-543, 14-550
RELEASE 1-85
Control structures 1-67
Coupled motion 9-358
Coupled-motion axes 9-359
Coupling factor 9-360
Coupled-axis combinations 9-359
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-711
A Appendix 11.02Index A
Coupled-axis motion 10-438 Deactivating frames 6-252
Coupling 9-352, 9-358 Deactivation position 13-501
Coupling 13-495 Defining user data 3-156
Cov.com, user cycles 2-138 Degrees 9-364
Create interrupt routine as subprogram 1-78 DELETE 1-93
CS 9-352 Delete couplings 13-502
CTAB 9-369 Delete distance-to-go 5-221
CTABDEF 9-365 Delete distance-to-go with preparation 10-418
CTABEND 9-365 Deletion of distance-to-go 10-418, 11-462
CTABINV 9-369 Denominator polynomial 5-209
Current Deselect transformation: TRAFOOF 7-304
Angular offset 13-503 Direct axis transfer: GETD 1-87
Coupling status following spindle 13-503 Displaying the block number programmed last
Current block display 2-125 2-121
Current channel basic frames 6-259 DRF offset 6-249
Current first basic frame in the channel 6-260 Drive-independent reactions 13-514
Current NCU-global basic frames 6-259 Drive-independent retract 13-521
Current programmable frame 6-262 Drive-independent stop 13-520
Current settable frame 6-261 Dwell time 1-76
Current system frames 6-259, 6-261, 6-262
Current total frame 6-262 E
Curve parameter 5-211
Curve tables 9-362 EG
CUT 14-555 Electronic gear 13-505
Cutter EGONSYNE 13-508
Reference point (FH) 8-334 Electronic gear 13-505
Tip (FS) 8-334 End of program 10-451
Cutting edge number 8-341 Endless program 1-70
Cycles Error checkback 14-543, 14-550
Setting parameters for user cycles 2-136, Error responses 10-442
2-138 Euler angle 8-336
Cylinder peripheral curve transformation 7-290, Evaluation function 10-423
7-294 EXECTAB 14-542
Offset contour normal OFFN 7-292 EXECUTE 4-176
Executing external subprogram 2-132
EXTCALL 2-132
D
Extended measuring function 5-218, 7-279
D numbers Extended stopping and retract 13-513
Check 8-342 External zero offset 6-250
Determine T number 8-344
Free assignment 8-341
Rename 8-343
DC link backup 13-519
Deactivate/reactivate interrupt routine 1-79
Siemens AG, 2002. All rights reserved
A-712 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
F I
F word polynomial 5-212 Identification number 10-398
Face milling 7-272 Inclined axis programming
Face turning G05, G07 7-300
External machining 14-543 Inclined axis transformation 7-296
Internal machining 14-543 Inclined axis, TRAANG 7-276, 7-297
FAxis 9-352, 9-358, 9-364, 9-375 Indirect G code programming 1-42
Feed Indirect programming 1-40
Axial 10-433 Indirect subprogram call 1-41
FGROUP Infeed
Axes 5-211 Axis 11-472
FIFO variable 10-413 Motion 11-467, 11-469
Fine offset 6-248 Suppress 11-464
First basic frame in the channel 6-258 Initialization program 3-153
Flag variables 10-409 Generating an initialization program 3-154
Following axis 9-375 Loading initialization program 3-154
FOR 1-68 Saving initialization program 3-154
Frame calculation 6-253 User data definition 3-156
Frame chaining 6-245, 6-263 Initiation of stroke 12-478
Frame rotation definition 6-247 Interpolation cycle 13-523
Frame variable Interrupt routine 1-77
Coordinate transformation call 6-236 Define the priority 1-79
Frame variables 6-236 Programmable traverse direction 1-77
Assigning values 6-241 Rapid lift from contour 1-80
Definition of new frames 6-247 Save interrupt position 1-78
Predefined frame variables 6-237 Intersection procedure for 3D compensation
Reading or changing frame components 6-243 8-335
Friction 13-493 IPO cycle 11-470
ISD (Insertion Depth) 8-328
G ISFILE 1-97
G code 5-211
J
Group 5-213
G643 5-212 Jump instruction
Generator operation 13-519 CASE instruction 1-65
GUD
Automatic activation 3-162 L
Laser power control 10-422
H
LAxis 9-352, 9-358, 9-364, 9-375
Hold time 11-459 Lead angle 7-270
Leading axis 9-375
Leading value coupling 10-439
Leading value simulation 9-378
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-713
A Appendix 11.02Index A
Learn compensation characteristics 13-493 Mode change 10-450
Linear interpolation 5-211, 5-212 Motion control 13-534
Link axis 13-526 Motion-synchronized actions
Link communication 13-522 Actions 10-402
Link module 13-523 Overview 10-404
Link variable Motion-synchronous actions
Global 13-523 Programming 10-395
Logic operators 1-51
Longitudinal turning N
External machining 14-543
Internal machining 14-543 N 9-364
Lower/upper case 1-59 NC Stop 10-451
NCU
Link 13-523
M
NCU-global basic frames 6-256
M commands 12-479 NCU-global settable frames 6-257
M function NCU-to-NCU communication 13-523
Three-digit 2-143 Nesting depth 1-69
M6 Networked NCUs 13-523
Subprogram call 2-136 NEWCONF 1-90
MAC Nibbling 12-476
Automatic activation 3-162 Nibbling on 12-476
MACH 14-543
Machine O
State, global 13-523
Machine and setting data 10-412 OEM addresses 5-228
Macro technology 12-479 OEM functions 5-228
Macros 2-142 OEM interpolations 5-228
Max/min indicator 14-546, 14-548 Offset contour normal OFFN 7-292
MEAFRAME 6-253, 6-256 Offset of the rotary axes 8-348
Measured value recording 5-217 Online tool length compensation 7-284
Measurement 10-441 Online tool offset 10-428
Measurement results 5-221 Operating mode 5-220
Measurements with touch trigger probe Orientation axes 7-269, 7-274, 7-276
Programming measuring blocks 5-216 Oscillating axis 11-457
Status variable 5-216 Oscillation
Measuring probe status 5-222 Activate, deactivate oscillation 11-459
Memory Asynchronized oscillation 11-456, 11-458
Memory structure 3-146 Control via synchronized action 11-464
Program memory 3-146 Defining the sequence of motions 11-460
User memory 3-146 Synchronized oscillation 11-463
Minimum position/maximum position of the rotary Oscillation reversal points 11-457
axis 8-348 Override 11-470
Mode 11-463
Siemens AG, 2002. All rights reserved
A-714 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
P Program run with preprocessing memory 9-386
Program runtime 13-528
Parameterizable subprogram return 2-113
Programmable motion end criterion 5-229
Parameters of the rotary axes 8-348
Programmable search path for subprogram calls
Parts program 13-523, 13-526
2-123
Partial infeed 11-464
Programming search paths for subprogram call
Partial length 11-463
3-152
Path
Protection levels for user data 3-160
Absolute 1-73
Protection zones 4-175
Relative 1-73
Activating/deactivating protection zones 4-180
Path axes 5-211
Contour definition of protection zones 4-178
Path feed 5-211
Define channel-specific protection zones 4-176
Path section 12-480
Define machine-specific protection zones 4-176
Path segmentation 12-482
Defining protection zones 4-177
Path segmentation for path axes 12-481
Punching 12-476, 12-480
Path segmentation for single axes 12-482
Punching on 12-476
Polynomial
Punching with delay Off 12-476
Interpolation 5-211
Punching with delay On 12-476
Polynomial coefficient 5-205
Punching, nibbling Off 12-476
Polynomial definition 10-420
Polynomial interpolation 5-204
Denominator polynomial 5-209 Q
Position axis 10-432 Quadrant error compensation
Position synchronism 13-496 Activate learning process 13-494
Positioning movements 10-430 Deactivate learning process 13-494
Power On 10-450 Subsequent learning 13-494
Preprocessing memory 9-386 Quantity of parts, fixed 1-71
Preprocessing stop 10-417
Preset offset 6-251
R
Program coordination 1-72
Example 1-75 R 15-591
Instructions for program coordination 1-73 R parameters 10-411
Program end 1-76 READ 1-94
Program memory 3-146 Read-in disable 10-416
Creating workpiece directories 3-150 Real-time variables 10-406
Directories 3-148 Relief cut 14-543
File types 3-148 Relief cut elements 14-544
Overview 3-147 REPEAT 1-69
Programming a search path for a subprogram Repeating program sections with indirect
call 3-152 Programming CALL 2-120
Search path with subprogram call 3-151 Repositioning 10-453
Selecting workpiece 3-151 Repositioning on contour 9-388
Workpiece directory 3-149 Approach along a straight line 9-391
Program repetition 2-117 Approach along quadrant 9-391
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-715
A Appendix 11.02Index A
Approach along semi-circle 9-392 Station/position change 13-526
Approach with new tool 9-390 Status of coupling 9-378
Repositioning point 9-389 Stock removal 14-542
Reset 10-450 Stopping and retract
Resolved kinematics 8-346 Extended 13-513
Reversal String length 1-60
Area 11-464 String operations 1-55
Point 11-464 Structuring instruction for the Step editor 3-173
Rotary axes Subprogram call
Distance vectors l1, l2 8-346 Indirect 1-41
Rotary axis Subprogram call with M/T function 2-136
Direction vectors V1, V2 8-346 Subprogram call, search path 3-151
RPY angle 8-336 Subprogram with path specification and
Run string as parts program line 1-44 parameters 2-122
Runtime response 1-69 Subprogram, external 2-132
Subprograms 2-102
S Indirect subprogram call 2-119
Modal subprogram call 2-118
SBLON 2-126 Nesting 2-103
Search for character 1-60 Program repetition 2-117
Selecting a substring 1-62 SAVE mechanism 2-104
Selection of a single character 1-63 Subprogram call 2-109
Servo parameter block programmable 5-232 Subprogram with parameter transfer 2-109
Set actual value 10-436 Subprograms with parameter transfer
Set up variable axis transfer response 1-89 Array definition 2-108
Setpoint coupling 13-495 Parameter transfer between main program and
Settable path reference 5-211 subprogram 2-105
Setting data 11-458 Supplementary conditions 1-70, 5-212, 10-450
Single axis motion 12-482 SW limit switch 10-434
Single block suppression 2-126 Switchable geometry axes 7-308
Singular positions 7-275 Synchronization run
Sparking-out stroke 11-462 Coarse 13-495
Speed ratio 13-499 Fine 13-495
Spindle motions 10-437 Setpoint synchronization 13-495
Spindle transfer Synchronized action parameters 10-410
GET 1-85 Synchronized actions 13-523
RELEASE 1-85 Static 9-379
Spline grouping 5-193 Synchronized oscillation
Spline interpolation 5-187, 5-211 Assignment of oscillating and infeed axes
A spline 5-188 11-465
B spline 5-189 Definition of infeed 11-465
C spline 5-190 Infeed in reversal area 11-467
Compressor 5-193 Stop at reversal point 11-469
Start/stop axis 10-432 Synchronized action 11-466
Siemens AG, 2002. All rights reserved
A-716 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixIndex A
Synchronized spindle 13-495 Tool orientation 8-336
Activate synchronized mode 13-501 Toolholder 8-348
Block change behavior 13-500 Clear/edit/read data 8-349
Coupling type 13-500 Kinematics 8-346
Deactivate synchronized mode 13-501 Torsion 13-493
Define pair 13-497 Total basic frame 6-260
Delete coupling 13-502 TRACYL transformation 7-290
Pair 13-496 TRAFOOF 7-304
Speed ratio 13-499 Transformation TRAORI 7-268
Synchronized spindle Transformation with a swiveling linear axis 7-267
System variable 1-27 Transformation, 3/4-axis 7-268
System variables 1-26, 13-523 Transformation, 5-axis
Global 13-523 Programming in Euler angles 7-270
Programming in RPY angles 7-271
T Programming the direction vector 7-271
Tool orientation 7-269
TANG 9-353 Transformation, 5-axis, face milling 7-272
Tangential control Transformation, 5-xis, programming via
Angle limit through working area limitation LEADITILT 7-269
9-354 TRANSMIT transformation 7-287
Defining following axis and leading axis 9-353 TRAORI 7-266
Tangential control, activation, TANGON 9-354 Travel to fixed stop FXS and FOCON/FOCOF
Tangential control, deactivation 9-354 10-442
Technology cycles 10-445 Travel-dependent acceleration PUNCHACC
Thread blocks 5-212 12-476, 12-477
Three-digit M/G function 2-143 Traversing a contour element 14-556
Tilt angle 7-270 Trigger events 5-220
Timer variable 10-409 Type conversion 1-56
Tool management 8-316 Type of kinematics 8-349
Tool monitoring, grinding-specific 8-321 Type of kinematics M 8-346
Tool offset Type of kinematics P 8-346
3D face milling 8-331 Type of kinematics T 8-346
Offset memory 8-314
Online 8-319
U
Tool offsets
Face milling 8-328 Uc.com, user cycles 2-139
Tool orientation 7-269, 8-336 User memory 3-153
with LEAD and TILT 7-273 Data areas 3-153
Tool radius compensation, 3D 8-328 Initialization programs 3-153
Behavior at outside corners 8-337 Reserved module names 3-156
Circumferential milling 8-330, 8-331
Insertion depth (ISD) 8-334
Inside corners/outside corners 8-334
Programming tool orientation 8-336
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-717
A Appendix 11.02Index A
V W
Variable 1-26 Wait marks 10-441
Arithmetic variable 1-27 WCS 3-149
Array definition 1-34 WHEN-DO 11-466
Assignments 1-45 WHILE 1-68
Indirect programming 1-40 Workpiece clamping 13-523
System variable 1-27 Workpiece counter 13-530
Type conversion 1-54 Workpiece directory 3-149
User-defined 1-26 WPD 3-149
User-defined variable 1-29 WRITE 1-91
Variable classes 1-26
Variable types 1-27 Z
Variable definition 1-29
Variable type 1-31 Zero frame 6-252
Variables Zero offset
NCK-specific global variables 1-76 Deactivating transformations 6-252
Vocabulary word 10-399 External zero offset 6-250
Offset using handwheel 6-249
PRESETON 6-251
Siemens AG, 2002. All rights reserved
A-718 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixCommands, Identifiers A
A5 7-236
B Commands, Identifiers ABS 1-41
ACC 13-453
- ACOS 1-41
ACTFRAME 6-204
- 1-41
ALF 1-70
Amax 12-434
* Amin 12-434
* 1-41 AND 1-44
ANZHINT 14-493, 14-495
applim 9-325
/
aproxLW 9-325
/ 1-41 APW 3-139
AROTS 6-213
: AS 2-122
ASIN 1-41
: 1-41 ASPLINE 5-155
ATAN2 1-41
+ AV 13-455
AX 13-446
+ 1-41
AXCTSWE 13-480
AXIS 1-29
< AXNAME 1-50, 13-446
< 1-43 AXSTRING 1-50, 13-446
1-43 B5 7-236
>= 1-43 BAUTO 5-159
BFRAME 6-203
A BNAT 5-159
BOOL 1-29
A 7-259
BRISK 11-415
A1, A2 8-310, 8-312
BSPLINE 5-155
A2 7-236
BTAN 5-159
A3 7-236
A4 7-236
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-719
A Appendix 11.02Commands, Identifiers A
C CTABDEL 9-325
CTABEND 9-325
C2 7-236
CTABINV 9-325
C3 7-236
CTRANS 6-207
C4 7-236
CUT3DC 8-292
C5 7-236
CUT3DF 8-292
CAC 5-154
CUT3DFF 8-292
CACN 5-154
CUT3DFS 8-292
CACP 5-154
CUTCONOF 8-289
CALCDAT 14-490, 14-505
CUTCONON 8-289
CALL 2-107
CANCEL 10-354
CASE 1-58 D
CDC 5-154 DEF 1-29
CFINE 6-214 DEFAULT 1-58
CHANDATA 3-134 DEFINE 2-122
CHAR 1-29 DELDTG 5-194
CHKDNO 8-306 DELT 8-280
CIC 5-154 DISABLE 1-70
CLEARM 1-67 DISPLOF 2-109
CLRINT 1-70 DISPR 9-346
CMIRROR 6-207 DIV 1-41
COARSE 13-450, 13-454, 13-455 DO 10-354, 11-421
COARSEA 5-197 DRFOF 6-218
COMPLETE 3-132, 3-133 DUPLO_NR 8-280
COMPOF 5-169, 5-179 DV 13-455
COMPON 5-179, 9-342 DZERO 8-309
CONTDCON 14-498
CONTPRON 14-490, 14-491, 14-503, 14-504
E
COS 1-41
COUPDEF 13-450, 13-452, 13-454 EAUTO 5-159
COUPDEL 13-450, 13-452, 13-457 ELSE 1-60
COUPOF 13-450, 13-456, 13-457 ENABLE 1-70
COUPON 13-450, 13-456, 13-457 ENAT 5-159
COUPRES 13-450, 13-457 ENDFOR 1-60
CP 7-245 ENDIF 1-60
CPROT 4-148 ENDLOOP 1-60
CPROTDEF 4-144, 4-146 ENDPOS 11-421
CROT 6-207 ENDPROC 10-384
CROTS 6-213 ENDWHILE 1-60
CSCALE 6-207 ERG 14-505
CSPLINE 5-155 ERROR 14-491, 14-498
CTAB 9-325 ETAN 5-159
CTABDEF 9-325 EVERY 10-354
Siemens AG, 2002. All rights reserved
A-720 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixCommands, Identifiers A
EXECTAB 14-504 GOTOB 1-58
EXECUTE 4-144, 4-146, 14-491, 14-498 GOTOF 1-58
EXP 1-41 GUD 3-128, 3-132, 3-137, 3-139
EXTCALL 2-113
EXTERN 2-101 I
I1,I2 8-310
F
ID 10-353
FA 11-418, 13-453 IDS 10-353
FALSE 1-25 IF 1-60
FCTDEF 8-283 IF-ELSE-ENDIF 1-60
FCUB 9-339 IFRAME 6-204
FINE 13-450, 13-455 II1,II2 11-422
FINEA 5-197 INDEX 1-53
FLIN 9-339 INIT 1-66
FMA 15-517 INITIAL 3-133
FNORM 9-339 INT 1-29
FOR 1-60 INTERSEC 14-490, 14-503
FPO 9-339 IPOENDA 5-197
FRAME 1-29 IPOSTOP 13-450, 13-453, 13-455
FRC 15-518 ISAXIS 13-446
FRCM 15-518 ISD 8-292, 8-298
FROM 10-354 ISNUMBER 1-50
FS 13-450
FTOC 8-283 K
FTOCOF 8-283
FTOCON 8-283 KTAB 14-493, 14-495, 14-501, 14-504
FW 9-325
L
G LEAD 7-236, 8-300
G05 7-263 LEADOF 9-333
G07 7-263 LEADON 9-333
G1 11-415 LIFTFAST 1-70
G153 6-218 LOCK 10-354
G25,G26 9-318 LOOP 1-60
G4 11-417 LOOP-ENDLOOP 1-61
GEOAX 7-271 LS 13-450
GET 1-78 LW 9-325
GETACTTD 8-308
GETD 1-78 M
GETDNO 8-307
M 8-312
GETSELT 8-280
M17 2-97
GETT 8-280
MATCH 1-53
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-721
A Appendix 11.02Commands, Identifiers A
MCALL 2-106 OSCTRL 11-414, 11-418
MEAC 5-186, 5-194 OSE 11-414, 11-418
MEAFRAME 6-220 OSNSC 11-414, 11-421
MEAS 5-183 OSO2 11-414
MEASA 5-186 OSOF 8-300
MEAW 5-183 OSP 11-415
MEAWA 5-186 OSP1 11-414, 11-421
MI 6-209 OSP2 11-421
MIRROR 6-204 OSS 8-300
MMC 13-486 OSSE 8-300
MOD 1-41 OST 11-417
MOV 10-390 OST1 11-414, 11-421
MPF 3-128 OST2 11-414, 11-421
MU 7-261 OVRA 13-453
MZ 7-261
P
N
PDELAYOF 12-434
NEWT 8-280 PDELAYON 12-434
Nibbling 12-438 PFRAME 6-204
NN 14-491 PKT 14-505
NO. 14-505 PL 5-158, 5-175
NOC 13-455 PO 5-175
NOT 1-44 POLY 5-175
NPROT 4-148 POLYNOMIAL 14-492, 14-499
NPROTDEF 4-144, 4-146 POLYPATH 5-175
NUMBER 1-50 PON 12-434, 12-440
PONS 12-434
O POS 13-456
POSP 11-421
OEMIPO1/2 5-196 POT 1-41
OF 1-59 PRESETON 6-217, 6-220
OFFN 7-252, 7-253 PRIO 1-70
OR 1-44 PROC 2-97
ORIC 8-300 PUNCHACC 12-434
ORID 8-300 PUTFTOC 8-283
ORIMCS 8-300 PUTFTOCF 8-283
ORIMKS 7-240, 7-242 PW 5-157
ORIS 8-300
ORIWCS 8-300
Q
ORIWKS 7-240, 7-242
OS 11-414, 11-417 QEC 13-448
OSC 8-300 QECDAT.MPF 13-449
OSCILL 11-421, 11-423 QECLRN.SPF 13-449
Siemens AG, 2002. All rights reserved
A-722 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
A 11.02 AppendixCommands, Identifiers A
QECLRNOF 13-448 Smin 12-434
QECLRNON 13-448 SOFT 11-415
QECTEST.MPF 13-449 SON 12-434, 12-439, 12-440
SONS 12-434
R SPI 13-446, 13-453
SPIF1 15-530
RDISABLE 10-374 SPIF2 15-530
REAL 1-29 SPLINE 14-492, 14-499
RELEASE 1-78 SPLINEPATH 5-161
REP 1-36 SPN 12-438
REPEAT 1-60 SPOF 12-434
REPOS 1-70, 1-77 SPOS 13-453
REPOSA 9-346 SPP 12-438
REPOSH 9-346 SQRT 1-41
REPOSHA 9-346 SR 15-531
REPOSL 1-77, 9-346 SRA 15-531
REPOSQ 9-346 ST 15-531
REPOSQA 9-346 STA 15-531
RET 2-97 START 1-66
RINDEX 1-53 STARTFIFO 9-344
RMB 9-346 STOPFIFO 9-344
RME 9-346 STOPRE 5-183, 5-190, 5-192, 9-344, 11-416
RMI 9-346 STOPREOF 10-375
ROTS 6-213 STRING 1-29
ROUND 1-41 STRINGFELD 1-48
RPY 8-300 STRINGVAR 1-48
RT 6-209 STRLEN 1-53
SUBSTR 1-55
S SUPA 6-218
SYNFCT 10-381
S1,S2 13-452, 13-457
SYNR 3-137
SAVE 1-71, 2-96
SYNRW 3-137
SBLOF 2-110
SBLON 2-110
SC 6-209 T
SCPARA 5-198 TABNAME 14-491, 14-498, 14-502, 14-504
SD 5-157 TAN 1-41
SET 1-34 TANG 9-316
SETDNO 8-307 TANGOF 9-316
SETINT 1-70 TANGON 9-316
SETM 1-67 TE 5-186
SETPIECE 8-280 THREAD 14-492, 14-499
SIN 1-41 TILT 7-236, 8-300
Smax 12-434 TLIFT 9-316
Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition A-723
A Appendix 11.02Commands, Identifiers A
TOLOWER 1-52 X
TOUPPER 1-52
x 8-280
TR 6-209
XOR 1-44
TRAANG 7-253, 7-259
TRACYL 7-250, 7-253
TRAFOOF 7-232, 7-250, 7-253, 7-259, 7-267
TRAILOF 9-321
TRAILON 9-321
TRANSMIT 7-250
TRAORI 7-234
TRUE 1-25
TRUNC 1-41
U
U1,U2 11-422
UNLOCK 10-354
UNTIL 1-60, 1-62
V
V1,V2 8-310
VAR 2-99
VARIB 14-502, 14-505
W
WAIT 1-67
WAITC 13-450, 13-453
WAITE 1-67
WAITM 1-66
WAITMC 1-67
WAITP 11-417
WALIMON 9-318
WCS 11-428
WHEN 10-354
WHEN-DO 11-421
WHENEVER 10-354
WHENEVER-DO 11-421, 11-424
WHILE 1-60
WZ 8-280
Siemens AG, 2002. All rights reserved
A-724 SINUMERIK 840D/840Di/810D Programming Guide Advanced (PGA) – 11.02 Edition
To Suggestions
SIEMENS AG
Corrections
A&D MC BMS For publication/manual:
P.O. Box 3180 SINUMERIK 840D/840Di/810D
Programming Guide
D-91050 Erlangen, Germany Advanced
Phone: ++49-(0)180-5050-222 [Hotline]
Fax: ++49-(0)9131-98-2176 [Documentation]
User Documentation
Email: [email protected]
From
Name Order No.: 6FC5298-6AB10-0BP2
Edition: 11.02
Company/Dept.
Should you come across any printing errors when
Address: reading this publication, please notify us on this sheet.
Suggestions for improvement are also welcome.
Zip code:
Phone: /
Fax: /
Suggestions and/or corrections
Overview of SINUMERIK 840D/840Di/810D Documentation (11.2002)
General Documentation User Documentation
SINUMERIK
SIROTEC
SINUMERIK SINUMERIK SIMODRIVE SINUMERIK SINUMERIK SINUMERIK SINUMERIK
840D/810D 840D/840Di/ Accessories 840D/810D/ 840D/840Di/ 840D/840Di/ 840D/840Di/
810D/ FM-NC 810D 810D 810D
Brochure Catalog Catalog AutoTurn Operator’s Guide Diagnostics Operator’s Guide *)
Ordering Info. Accessories – Short Guide – HT 6 Guide *) – Short Guide
NC 60 *) NC-Z – Programming/ – HMI Embedded
Setup – HMI Advanced
User Documentation Manufacturer/Service Documentation
SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK
840D/840Di/ 840D/810D 840Di 840D/840Di/ 840D/810D 840D/840Di/
810D 810D 810D
Program. Guide Operator’s Guide System Overview Configuring Operator Description of Description of
– Short Guide – ManualTurn (HW) *) Components Functions Functions
– Fundamentals *) – Short Guide ManualTurn – 810D (HW) *) – ManualTurn Synchronized
– Advanced *) – ShopMill – 840D – ShopMill Actions
– Cycles – Short Guide ShopMill – ShopTurn
– Measuring Cycles – ShopTurn
– ISO Turning/Milling – Short Guide ShopTurn
Manufacturer/Service Documentation
SINUMERIK
SIMODRIVE SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK
611D 840D/840Di/ 840D/840Di/ 840D/810D 840D/810D 840D/810D
840D/810D 810D 810D
Description of Description of Description of Configuring Kit Description of IT Solutions
Functions Functions Functions HMI Embedded Functions – Computer Link
Drive Functions *) – Basic Machine *) Tool Manage- Operator Interface – Tool Data Information System
– Extended Functions ment OP 030 – NC Data Management
– Special Functions – NC Data Transfer
– Tool Data Communication
Manufacturer/Service Documentation
SINUMERIK
SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK SIMODRIVE
SIMODRIVE SINUMERIK SIMODRIVE SIMODRIVE SIMODRIVE SIMODRIVE SIROTEC
840D 840D/840Di 840D 840D
810D 611D 611D
611D
Description of Description of Installation & Lists *) Description of Description of Functions EMC
Functions Functions Start-Up Guide *) Functions – Hydraulics Module Guidelines
SINUMERIK Digitizing – 810D Linear Motor – Analog Module
Safety Integrated – 840D/611D
– HMI Manufacturer/Service Documentation
Electronic Documentation
SINUMERIK SINUMERIK SINUMERIK SINUMERIK SINUMERIK
SIMODRIVE
840D/840Di/ 840Di 840D/810D 840D/840Di/
840D/840Di/ 810D 810D
810D
611, Motors
DOC ON CD *) Description of Manual Description of Manual
The SINUMERIK System Functions (HW + Installation Functions @ Event
ISO Dialects for and Start-Up) Remote Diagnosis
SINUMERIK
*) These documents are a minimum requirement
Siemens AG
Automation & Drives
Motion Control Systems
P.O. Box 3180, D-91050 Erlangen © Siemens AG, 2002
Subject to change without prior notice
Germany Order No.: 6FC5298-6AB10-0BP2
www.ad.siemens.de Printed in Germany
Comments