Siemens SINUMERIK 828D Turning Owner's manual

SINUMERIK
SINUMERIK 828D
Fundamentals
Programming Manual
Valid for:
CNC system software Version 4.3
07/2010
6FC5398-1BP40-0BA0
Preface
Fundamental Geometrical
Principles
1
Fundamental Principles of
NC Programming
2
Creating an NC program
3
Tool change
4
Tool offsets
5
Spindle motion
6
Feed control
7
Geometry settings
8
Motion commands
9
Tool radius compensation
10
Path action
11
Coordinate transformations
(frames)
12
Auxiliary function outputs
13
Supplementary commands
14
Other information
15
Tables
16
Appendix
A

Legal information
Warning notice system
This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent
damage to property. The notices referring to your personal safety are highlighted in the manual by a safety alert
symbol, notices referring only to property damage have no safety alert symbol. These notices shown below are
graded according to the degree of danger.
DANGER
indicates that death or severe personal injury will result if proper precautions are not taken.
WARNING
indicates that death or severe personal injury may result if proper precautions are not taken.
CAUTION
with a safety alert symbol, indicates that minor personal injury can result if proper precautions are not taken.
CAUTION
without a safety alert symbol, indicates that property damage can result if proper precautions are not taken.
NOTICE
indicates that an unintended result or situation can occur if the corresponding information is not taken into
account.
If more than one degree of danger is present, the warning notice representing the highest degree of danger will
be used. A notice warning of injury to persons with a safety alert symbol may also include a warning relating to
property damage.
Qualified Personnel
The product/system described in this documentation may be operated only by personnel qualified for the specific
task in accordance with the relevant documentation for the specific task, in particular its warning notices and
safety instructions. Qualified personnel are those who, based on their training and experience, are capable of
identifying risks and avoiding potential hazards when working with these products/systems.
Proper use of Siemens products
Note the following:
WARNING
Siemens products may only be used for the applications described in the catalog and in the relevant technical
documentation. If products and components from other manufacturers are used, these must be recommended
or approved by Siemens. Proper transport, storage, installation, assembly, commissioning, operation and
maintenance are required to ensure that the products operate safely and without any problems. The permissible
ambient conditions must be adhered to. The information in the relevant documentation must be observed.
Trademarks
All names identified by ® are registered trademarks of the Siemens AG. The remaining trademarks in this
publication may be trademarks whose use by third parties for their own purposes could violate the rights of the
owner.
Disclaimer of Liability
We have reviewed the contents of this publication to ensure consistency with the hardware and software
described. Since variance cannot be precluded entirely, we cannot guarantee full consistency. However, the
information in this publication is reviewed regularly and any necessary corrections are included in subsequent
editions.
Siemens AG
Industry Sector
Postfach 48 48
90026 NÜRNBERG
GERMANY
order number: 6FC5398-1BP40-0BA0
Ⓟ 06/2010
Copyright © Siemens AG 2010.
Technical data subject to change

Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 3
Preface
SINUMERIK Documentation
The SINUMERIK documentation is organized in three parts:
● General Documentation
● User Documentation
● Manufacturer/service documentation
Information on the following topics is available at
http://www.siemens.com/motioncontrol/docu:
● Ordering documentation
Here you can find an up-to-date overview of publications
● Downloading documentation
Links to more information for downloading files from Service & Support.
● Researching documentation online
Information on DOConCD and direct access to the publications in DOConWeb.
● Compiling individual documentation on the basis of Siemens contents with the My
Documentation Manager (MDM), refer to http://www.siemens.com/mdm.
My Documentation Manager provides you with a range of features for generating your
own machine documentation.
● Training and FAQs
Information on our range of training courses and FAQs (frequently asked questions) are
available via the page navigation.
Target group
This publication is intended for:
● Programmers
● Project engineers
Benefits
With the programming manual, the target group can develop, write, test, and debug
programs and software user interfaces.

Preface
Fundamentals
4 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Standard scope
This Programming Guide describes the functionality afforded by standard functions.
Extensions or changes made by the machine tool manufacturer are documented by the
machine tool manufacturer.
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.
Further, for the sake of simplicity, this documentation does not contain all detailed
information about all types of the product and cannot cover every conceivable case of
installation, operation or maintenance.
Technical Support
If you have any questions, please contact our hotline:
Europe / Africa
Phone [phone]
Fax [phone]
Internet http://www.siemens.de/automation/support-request
America
Phone [phone]
Fax [phone]
E-mail mailto:[email protected]
Asia/Pacific
Phone [phone]
Fax [phone]
E-mail mailto:support.asia.automatio[email protected]
Note
You will find telephone numbers for other countries for technical support on the Internet:
http://www.automation.siemens.com/partner

Preface
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 5
Questions about the manual
If you have any queries (suggestions, corrections) in relation to this documentation, please
fax or e-mail us:
Fax: [phone]
E-mail: mailto:[email protected]m
A fax form is available in the appendix of this document.
SINUMERIK Internet address
http://www.siemens.com/sinumerik
"Fundamentals" and "Advanced" Programming Manual
The description of the NC programming is divided into two manuals:
1. Fundamentals
This "Fundamentals" Programming Manual is intended for use by skilled machine
operators with the appropriate expertise in drilling, milling and turning operations. Simple
programming examples are used to explain the commands and statements which are
also defined according to DIN 66025.
2. Job planning
The Programming Manual "Advanced" is intended for use by technicians with in-depth,
comprehensive programming knowledge. By virtue of a special programming language,
the SINUMERIK control enables the user to program complex workpiece programs (e.g.
for free-form surfaces, channel coordination, ...) and makes programming of complicated
operations easy for technologists.
Availability of the described NC language elements
All NC language elements described in the manual are available for the SINUMERIK
840D sl. The availability regarding SINUMERIK 828D can be found in table "Operations:
Availability for SINUMERIK 828D (Page 503)".

Preface
Fundamentals
6 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0

Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 7
Table of contents
Preface ...................................................................................................................................................... 3
1 Fundamental Geometrical Principles ....................................................................................................... 13
1.1 Workpiece positions.....................................................................................................................13
1.1.1 Workpiece coordinate systems....................................................................................................13
1.1.2 Cartesian coordinates ..................................................................................................................15
1.1.3 Polar coordinates .........................................................................................................................18
1.1.4 Absolute dimensions....................................................................................................................19
1.1.5 Incremental dimension.................................................................................................................21
1.2 Working planes ............................................................................................................................23
1.3 Zero points and reference points .................................................................................................25
1.4 Coordinate systems .....................................................................................................................27
1.4.1 Machine coordinate system (MCS)..............................................................................................27
1.4.2 Basic coordinate system (BCS) ...................................................................................................30
1.4.3 Basic zero system (BZS) .............................................................................................................32
1.4.4 Settable zero system (SZS).........................................................................................................33
1.4.5 Workpiece coordinate system (WCS)..........................................................................................34
1.4.6 What is the relationship between the various coordinate systems?............................................34
2 Fundamental Principles of NC Programming........................................................................................... 35
2.1 Name of an NC program..............................................................................................................35
2.2 Structure and contents of an NC program ...................................................................................37
2.2.1 Blocks and block components .....................................................................................................37
2.2.2 Block rules....................................................................................................................................39
2.2.3 Value assignments.......................................................................................................................41
2.2.4 Comments....................................................................................................................................42
2.2.5 Skipping blocks ............................................................................................................................43
3 Creating an NC program.......................................................................................................................... 45
3.1 Basic procedure ...........................................................................................................................45
3.2 Available characters.....................................................................................................................47
3.3 Program header ...........................................................................................................................49
3.4 Program examples.......................................................................................................................51
3.4.1 Example 1: First programming steps ...........................................................................................51
3.4.2 Example 2: NC program for turning .............................................................................................52
3.4.3 Example 3: NC program for milling..............................................................................................54
4 Tool change............................................................................................................................................. 57
4.1 Tool change without tool management........................................................................................58
4.1.1 Tool change with T command......................................................................................................58
4.1.2 Tool change with M6....................................................................................................................59
4.2 Tool change with tool management (option)................................................................................61
4.2.1 Tool change with T command with active tool management (option)..........................................61
4.2.2 Tool change with M6 with active tool management (option)........................................................64
4.3 Behavior with faulty T programming ............................................................................................66

Table of contents
Fundamentals
8 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
5 Tool offsets .............................................................................................................................................. 67
5.1 General information about the tool offsets.................................................................................. 67
5.2 Tool length compensation........................................................................................................... 68
5.3 Tool radius compensation........................................................................................................... 69
5.4 Tool compensation memory........................................................................................................ 70
5.5 Tool types.................................................................................................................................... 72
5.5.1 General information about the tool types.................................................................................... 72
5.5.2 Milling tools ................................................................................................................................. 72
5.5.3 Drills ............................................................................................................................................ 74
5.5.4 Grinding tools .............................................................................................................................. 75
5.5.5 Turning tools ............................................................................................................................... 77
5.5.6 Special tools................................................................................................................................ 79
5.5.7 Chaining rule ............................................................................................................................... 80
5.6 Tool offset call (D) ....................................................................................................................... 81
5.7 Change in the tool offset data ..................................................................................................... 85
5.8 Programmable tool offset (TOFFL, TOFF, TOFFR).................................................................... 86
6 Spindle motion......................................................................................................................................... 91
6.1 Spindle speed (S), direction of spindle rotation (M3, M4, M5).................................................... 91
6.2 Cutting rate (SVC)....................................................................................................................... 95
6.3 Constant cutting rate (G96/G961/G962, G97/G971/G972, G973, LIMS, SCC) ....................... 101
6.4 Constant grinding wheel peripheral speed (GWPSON, GWPSOF).......................................... 107
6.5 Programmable spindle speed limitation (G25, G26)................................................................. 109
7 Feed control........................................................................................................................................... 111
7.1 Feedrate (G93, G94, G95, F, FGROUP, FL, FGREF).............................................................. 111
7.2 Traversing positioning axes (POS, POSA, POSP, FA, WAITP, WAITMC) .............................. 120
7.3 Position-controlled spindle operation (SPCON, SPCOF) ......................................................... 124
7.4 Positioning spindles (SPOS, SPOSA, M19, M70, WAITS)....................................................... 125
7.5 Feedrate for positioning axes/spindles (FA, FPR, FPRAON, FPRAOF) .................................. 134
7.6 Programmable feedrate override (OVR, OVRRAP, OVRA) ..................................................... 138
7.7 Programmable acceleration override (ACC) (option)................................................................ 140
7.8 Feedrate with handwheel override (FD, FDA) .......................................................................... 142
7.9 Feedrate optimization for curved path sections (CFTCP, CFC, CFIN)..................................... 146
7.10 Several feedrate values in one block (F, ST, SR, FMA, STA, SRA)......................................... 149
7.11 Non-modal feedrate (FB) .......................................................................................................... 152
7.12 Tooth feedrate (G95 FZ) ........................................................................................................... 153

Table of contents
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 9
8 Geometry settings.................................................................................................................................. 159
8.1 Settable work offset (G54 to G57, G505 to G599, G53, G500, SUPA, G153) ..........................159
8.2 Selection of the working plane (G17/G18/G19).........................................................................165
8.3 Dimensions ................................................................................................................................169
8.3.1 Absolute dimensions (G90, AC).................................................................................................169
8.3.2 Incremental dimensions (G91, IC) .............................................................................................172
8.3.3 Absolute and incremental dimensions for turning and milling (G90/G91) .................................175
8.3.4 Absolute dimension for rotary axes (DC, ACP, ACN)................................................................177
8.3.5 Inch or metric dimensions (G70/G700, G71/G710) ...................................................................180
8.3.6 Channel-specific diameter/radius programming (DIAMON, DIAM90, DIAMOF,
DIAMCYCOF) ............................................................................................................................183
8.3.7 Axis-specific diameter/radius programming (DIAMONA, DIAM90A, DIAMOFA,
DIACYCOFA, DIAMCHANA, DIAMCHAN, DAC, DIC, RAC, RIC)............................................186
8.4 Position of workpiece for turning................................................................................................191
9 Motion commands ................................................................................................................................. 193
9.1 General information about the travel commands.......................................................................193
9.2 Travel commands with Cartesian coordinates (G0, G1, G2, G3, X..., Y..., Z...)........................195
9.3 Travel commands with polar coordinates ..................................................................................197
9.3.1 Reference point of the polar coordinates (G110, G111, G112).................................................197
9.3.2 Travel commands with polar coordinates (G0, G1, G2, G3, AP, RP)........................................199
9.4 Rapid traverse movement (G0, RTLION, RTLIOF) ...................................................................204
9.5 Linear interpolation (G1) ............................................................................................................209
9.6 Circular interpolation ..................................................................................................................212
9.6.1 Circular interpolation types (G2/G3, ...) .....................................................................................212
9.6.2 Circular interpolation with center point and end point (G2/G3, X... Y... Z..., I... J... K...) ...........216
9.6.3 Circular interpolation with radius and end point (G2/G3, X... Y... Z.../ I... J... K..., CR).............220
9.6.4 Circular interpolation with opening angle and center point (G2/G3, X... Y... Z.../ I... J...
K..., AR)......................................................................................................................................223
9.6.5 Circular interpolation with polar coordinates (G2/G3, AP, RP)..................................................226
9.6.6 Circular interpolation with intermediate point and end point (CIP, X... Y... Z..., I1... J1...
K1...)...........................................................................................................................................229
9.6.7 Circular interpolation with tangential transition (CT, X... Y... Z...)..............................................233
9.7 Helical interpolation (G2/G3, TURN) .........................................................................................237
9.8 Involute interpolation (INVCW, INVCCW)..................................................................................240
9.9 Contour definitions .....................................................................................................................246
9.9.1 General information about contour definitions...........................................................................246
9.9.2 Contour definitions: One straight line (ANG) .............................................................................247
9.9.3 Contour definitions: Two straight lines (ANG)............................................................................248
9.9.4 Contour definitions: Three straight line (ANG)...........................................................................252
9.9.5 Contour definitions: End point programming with angle ............................................................256
9.10 Thread cutting with constant lead (G33)....................................................................................257
9.10.1 Thread cutting with constant lead (G33, SF) .............................................................................257
9.10.2 Programmable run-in and run-out paths (DITS, DITE)..............................................................265
9.11 Thread cutting with increasing or decreasing lead (G34, G35) .................................................268
9.12 Tapping without compensating chuck (G331, G332) ................................................................270

Table of contents
Fundamentals
10 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
9.13 Tapping with compensating chuck (G63).................................................................................. 275
9.14 Fast retraction for thread cutting (LFON, LFOF, DILF, ALF, LFTXT, LFWP, LFPOS,
POLF, POLFMASK, POLFMLIN).............................................................................................. 277
9.15 Chamfer, rounding (CHF, CHR, RND, RNDM, FRC, FRCM) ................................................... 282
10 Tool radius compensation...................................................................................................................... 289
10.1 Tool radius compensation (G40, G41, G42, OFFN) ................................................................. 289
10.2 Contour approach and retraction (NORM, KONT, KONTC, KONTT)....................................... 299
10.3 Compensation at the outside corners (G450, G451, DISC) ..................................................... 306
10.4 Smooth approach and retraction............................................................................................... 310
10.4.1 Approach and retraction (G140 to G143, G147, G148, G247, G248, G347, G348, G340,
G341, DISR, DISCL, FAD, PM, PR) ......................................................................................... 310
10.4.2 Approach and retraction with enhanced retraction strategies (G460, G461, G462)................. 321
10.5 Collision monitoring (CDON, CDOF, CDOF2) .......................................................................... 325
10.6 2D tool compensation (CUT2D, CUT2DF)................................................................................ 329
10.7 Keep tool radius compensation constant (CUTCONON, CUTCONOF) ................................... 332
10.8 Tools with a relevant cutting edge position............................................................................... 335
11 Path action............................................................................................................................................. 337
11.1 Exact stop (G60, G9, G601, G602, G603)................................................................................ 337
11.2 Continuous-path mode (G64, G641, G642, G643, G644, G645, ADIS, ADISPOS)................. 341
12 Coordinate transformations (frames) ..................................................................................................... 351
12.1 Frames ...................................................................................................................................... 351
12.2 Frame instructions..................................................................................................................... 353
12.3 Programmable zero offset......................................................................................................... 357
12.3.1 Zero offset (TRANS, ATRANS)................................................................................................. 357
12.3.2 Axial zero offset (G58, G59)...................................................................................................... 361
12.4 Programmable rotation (ROT, AROT, RPL) ............................................................................. 364
12.5 Programmable frame rotations with solid angles (ROTS, AROTS, CROTS) ........................... 374
12.6 Programmable scale factor (SCALE, ASCALE)........................................................................ 375
12.7 Programmable mirroring (MIRROR, AMIRROR) ...................................................................... 379
12.8 Frame generation according to tool orientation (TOFRAME, TOROT, PAROT) ...................... 384
12.9 Deselect frame (G53, G153, SUPA, G500) .............................................................................. 388
12.10 Deselecting overlaid movements (DRFOF, CORROF) ............................................................ 389
13 Auxiliary function outputs....................................................................................................................... 393
13.1 M functions................................................................................................................................ 397

Table of contents
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 11
14 Supplementary commands .................................................................................................................... 401
14.1 Output messages (MSG) ...........................................................................................................401
14.2 Writing string in OPI variable (WRTPR).....................................................................................403
14.3 Working area limitation ..............................................................................................................404
14.3.1 Working area limitation in BCS (G25/G26, WALIMON, WALIMOF)..........................................404
14.3.2 Working area limitation in WCS/SZS (WALCS0 ... WALCS10).................................................408
14.4 Reference point approach (G74) ...............................................................................................411
14.5 Fixed-point approach (G75, G751) ............................................................................................412
14.6 Travel to fixed stop (FXS, FXST, FXSW) ..................................................................................417
14.7 Acceleration behavior ................................................................................................................422
14.7.1 Acceleration mode (BRISK, BRISKA, SOFT, SOFTA, DRIVE, DRIVEA) .................................422
14.7.2 Influence of acceleration on following axes (VELOLIMA, ACCLIMA, JERKLIMA)....................425
14.7.3 Activation of technology-specific dynamic values (DYNNORM, DYNPOS, DYNROUGH,
DYNSEMIFIN, DYNFINISH) ......................................................................................................427
14.8 Traversing with feedforward control, FFWON, FFWOF.............................................................429
14.9 Contour accuracy, CPRECON, CPRECOF...............................................................................430
14.10 Dwell time (G4) ..........................................................................................................................431
14.11 Internal preprocessing stop........................................................................................................433
15 Other information................................................................................................................................... 435
15.1 Axes ...........................................................................................................................................435
15.1.1 Main axes/Geometry axes .........................................................................................................437
15.1.2 Special axes...............................................................................................................................438
15.1.3 Main spindle, master spindle .....................................................................................................438
15.1.4 Machine axes.............................................................................................................................439
15.1.5 Channel axes .............................................................................................................................439
15.1.6 Path axes ...................................................................................................................................439
15.1.7 Positioning axes.........................................................................................................................440
15.1.8 Synchronized axes.....................................................................................................................441
15.1.9 Command axes..........................................................................................................................441
15.1.10 PLC axes....................................................................................................................................441
15.1.11 Link axes....................................................................................................................................442
15.1.12 Lead link axes ............................................................................................................................443
15.2 From travel command to machine movement ...........................................................................446
15.3 Path calculation..........................................................................................................................447
15.4 Addresses ..................................................................................................................................448
15.5 Identifiers....................................................................................................................................452
15.6 Constants...................................................................................................................................454

Table of contents
Fundamentals
12 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
16 Tables.................................................................................................................................................... 457
16.1 Instructions................................................................................................................................ 457
16.2 Operations: Availability for SINUMERIK 828D.......................................................................... 503
16.3 Addresses ................................................................................................................................. 524
16.4 G function groups...................................................................................................................... 533
16.5 Predefined subroutine calls....................................................................................................... 551
16.6 Predefined subroutine calls in motion-synchronous actions..................................................... 566
16.7 Predefined functions ................................................................................................................. 567
A Appendix................................................................................................................................................ 573
A.1 List of abbreviations .................................................................................................................. 573
A.2 Feedback on the documentation............................................................................................... 578
A.3 Documentation overview........................................................................................................... 580
A.3.1 828D document tree.................................................................................................................. 580
Glossary ................................................................................................................................................ 581
Index...................................................................................................................................................... 603

Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 13
Fundamental Geometrical Principles 1
1.1 Workpiece positions
1.1.1 Workpiece coordinate systems
In order that the machine or the control can work with the positions specified in the NC
program, these specifications have to be made in a reference system that can be transferred
to the directions of motion of the machine axes. A coordinate system with the axes X, Y and
Z is used for this purpose.
DIN 66217 stipulates that machine tools must use clockwise, right-angled (Cartesian)
coordinate systems.
;
;
<
<
=
=
r
r
r
:
Figure 1-1 Workpiece coordinate system for milling

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
14 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
=
= ;
;
<
r
r
r:
<
Figure 1-2 Workpiece coordinate system for turning
The workpiece zero (W) is the origin of the workpiece coordinate system.
Sometimes it is advisable or even necessary to work with negative position specifications.
For this reason, positions that are to the left of the zero point are assigned a negative sign
("-").

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 15
1.1.2 Cartesian coordinates
The axes in the coordinate system are assigned dimensions. In this way, it is possible to
clearly describe every point in the coordinate system and therefore every workpiece position
through the direction (X, Y and Z) and three numerical values The workpiece zero always
has the coordinates X0, Y0, and Z0.
Position specifications in the form of Cartesian coordinates
To simplify things, we will only consider one plane of the coordinate system in the following
example, the X/Y plane:
;
;
<
<




3
3
3
3




Points P1 to P4 have the following coordinates:
Position Coordinates
P1 X100 Y50
P2 X-50 Y100
P3 X-105 Y-115
P4 X70 Y-75

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
16 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Example: Workpiece positions for turning
With lathes, one plane is sufficient to describe the contour:
=
;




3
3 3
3



Points P1 to P4 have the following coordinates:
Position Coordinates
P1 X25 Z-7.5
P2 X40 Z-15
P3 X40 Z-25
P4 X60 Z-35

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 17
Example: Workpiece positions for milling
For milling, the feed depth must also be described, i.e. the third coordinate (in this case Z)
must also be assigned a numerical value.



3
3
3
3
 



3
3

<
=
<
;
Points P1 to P3 have the following coordinates:
Position Coordinates
P1 X10 Y45 Z-5
P2 X30 Y60 Z-20
P3 X45 Y20 Z-15

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
18 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
1.1.3 Polar coordinates
Polar coordinates can be used instead of Cartesian coordinates to describe workpiece
positions. This is useful when a workpiece or part of a workpiece has been dimensioned with
radius and angle. The point from which the dimensioning starts is called the "pole".
Position specifications in the form of polar coordinates
Polar coordinates are made up of the polar radius and the polar angle.
The polar radius is the distance between the pole and the position.
The polar angle is the angle between the polar radius and the horizontal axis of the working
plane. Negative polar angles are in the clockwise direction, positive polar angles in the
counterclockwise direction.
Example
3ROH
;
<
3
3
r
r




Points P1 and P2 can then be described – with reference to the pole – as follows:
Position Polar coordinates
P1 RP=100 AP=30
P2 RP=60 AP=75
RP: Polar radius
AP: Polar angle

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0 19
1.1.4 Absolute dimensions
Position specifications in absolute dimensions
With absolute dimensions, all the position specifications refer to the currently valid zero
point.
Applied to tool movement this means:
the position, to which the tool is to travel.
Example: Turning
=
;




3
3 3
3



In absolute dimensions, the following position specifications result for points P1 to P4:
Position Position specification in absolute dimensions
P1 X25 Z-7.5
P2 X40 Z-15
P3 X40 Z-25
P4 X60 Z-35

Fundamental Geometrical Principles
1.1 Workpiece positions
Fundamentals
20 Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Example: Milling
;
<



3
3
3



In absolute dimensions, the following position specifications result for points P1 to P3:
Position Position specification in absolute dimensions
P1 X20 Y35
P2 X50 Y60
P3 X70 Y20