siemens 840D User Manual

Description of Functions 11/2002 Edition

ISO Dialects for SINUMERIK SINUMERIK 840D/840Di/810D

SINUMERIK 840D/840Di/810D

ISO Dialects for SINUMERIK

Description of Functions

Valid for
Control	Software version
SINUMERIK 840D		6
SINUMERIK 840DE (export version)		6
SINUMERIK 840D powerline		6
SINUMERIK 840DE powerline		6
SINUMERIK 840Di		2
SINUMERIK 840DiE (export version)		2
SINUMERIK 810D		3
SINUMERIK 810DE (export version)		3
SINUMERIK 810D powerline		6
SINUMERIK 810DE powerline		6

11.2002 Edition

Brief Description	1
Programming	2
Cycles and Contour
Definition	3
Start-Up	4
Boundary Conditions	5
Data Description (MD, SD)	6
Signal Description	7
Example	8
Data Fields, Lists	9
Alarms	10
References	A
Index

Order No. 6FC5-297-6AE10-0BP3 Printed in Germany

Aktiengesellschaft

Siemens

Siemens AG, 1999–2002. All rights reserved

Subject to changes without prior notice.

This publication was produced with Interleaf V7.

The reproduction, transmission or use of this document or its contents is not permitted without express written authority. Offenders will be liable for damages. All rights, including those created by patent grant or registration of a utility model or design, are reserved.

We have checked that the contents of this document correspond to the hardware and software described. Nonetheless, differences might exist and therefore we cannot guarantee that they are completely identical. The information contained in this document is, however, reviewed regularly and any necessary changes will be included in the next edition. We welcome suggestions for improvement.

Further information is available on the Internet under: http://www.ad.siemens.de/sinumerik

Other functions not described in this documentation might be executable in the control. However, no claim can be made regarding the availability of these functions when the equipment is first supplied or for service cases.

Trademarks

SIMATICr, SIMATIC HMIr, SIMATIC NETr, SIROTECr, SINUMERIKr and SIMODRIVEr are trademarks of Siemens. Other product names used in this documentation may be trademarks which, if used by third parties, could infringe the rights of their owners.

11.02 6FC5 298-6CA00-0BG3

Edition

Order No.

This book is part of the documentation on CD-ROM (DOCONCD)

Remarks

C

08.99 6FC5297–5AE10–0BP0

04.00 6FC5297–5AE10–0BP1

10.00 6FC5297–6AE10–0BP0

09.01 6FC5297–6AE10–0BP1

12.01 6FC5297–6AE10–0BP2

11.02 6FC5297–6AE10–0BP3

Remarks

A

C

C

C

C

C

Edition

Order No.

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 in relation to the same software version, this is indicated by a new edition coding in the header on that page.

Documentation

SINUMERIK

3ls

Preface

Structure of the	The SINUMERIK documentation is structured in three levels:
documentation	S	General documentation
	S	User documentation
	S	Manufacturer/service documentation.
	For detailed information on further publications on SINUMERIK 840D/840Di/
	810D, as well as on publications applicable to all SINUMERIK control systems,
	please contact your regional Siemens branch office.
Reader group	This documentation is intended for use by manufacturers of machine tools with
	SINUMERIK 840D or SINUMERIK 810D and SIMODRIVE 611D.
Hotline	If you have any questions about the control, please contact the hotline:
	A&D Technical Support		Phone.: ++49-180-5050-222
			Fax:	++49-180-5050-223
			Email:	adsupport@.siemens.com
	Please send any questions about the documentation (suggestions for
	improvement, corrections) to the following fax number or email address:
			Fax:	++49-9131-98-2176
			Email:	[e-mail]

Fax form: see reply form at the end of the manual.

Internet address http://www.ad.siemens.de/sinumerik

SINUMERIK 840D With effect from 09.2001 the

powerline

S SINUMERIK 840D powerline and

S SINUMERIK 840DE powerline

have been given improved performance. See the hardware description below for the list of the available powerline modules:

References: /PHD/, Configuring Manual SINUMERIK 840D

Siemens AG, 2002. All rights reserved	v
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

Preface

10.02

SINUMERIK 810D With effect from 12.2001 the

powerline

S SINUMERIK 810D powerline and

S SINUMERIK 810DE powerline

have been given improved performance. See the hardware description below for the list of the available powerline modules:

References: /PHC/, Configuring Manual SINUMERIK 810D

Target readers	S
	S
	S

Configuring engineers,

Electricians and start-up specialists

Service and operating personnel

The purpose of this manual

Indexes and references

The information in this manual makes it possible to import and use parts programs from external CNC systems.

For your better orientation, this manual offers a list of contents and the following appendices:

SReferences

SIndex

SIndex of commands

vi	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

Preface

Warning notes	The following warning notes with graded degrees of importance are used in this
	documentation:

Danger

!Indicates an imminently hazardous situation which, if not avoided, will result in death or serious injury or in substantial property damage.

Warning

!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.

Notice

Used without the safety alert symbol indicates a potential situation which, if not avoided, may result in an undesirable result or state.

Further information

Important

!Important indicates an important or especially relevant item of information.

Note

The “note” symbol is displayed in this document to draw your attention to information relevant to the subject in hand.

Machine manufacturer

The symbol shown is found in this documentation whenever the machine manufacturer can influence or amend the feature described. Please note the machine manufacturer’s specifications.

Siemens AG, 2002. All rights reserved	vii
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

Preface

10.02

Trademarks	IBM is a registered trademark of the International Business Corporation.
	MS DOS and WINDOWSTM are registered tradmarks of the Microsoft
	Corporation.

viii	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

Contents

1	Brief Description . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		1-13
2	Programming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		2-15
	2.1	Activation of functions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-15
	2.1.1	Switchover from ISO mode to Siemens mode . . . . . . . . . . . . . . . . . . .	2-16
	2.2	G commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-18
	2.2.1	G code display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-23
	2.2.2	Display of non–modal G codes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-23
	2.2.3	G code output to PLC (as from SW 6.4) . . . . . . . . . . . . . . . . . . . . . . . .	2-24
	2.2.4	Zero offset . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-26
	2.2.5	Writing a zero offset with G10 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-27
	2.2.6	Decimal point programming . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-27
	2.2.7	Dwell time in spindle revolutions G04 . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-29
	2.2.8	Scaling and mirroring: G51, G51.1 (ISO Dialect M) . . . . . . . . . . . . . . .	2-29
	2.2.9	2D/3D rotation G68 / G69 (ISO Dialect M) . . . . . . . . . . . . . . . . . . . . . . .	2-32
	2.2.10	Polar coordinates: G15 (ISO Dialect M) . . . . . . . . . . . . . . . . . . . . . . . . .	2-33
	2.2.11	Polar coordinate interpolation G12.1 / G13.1 (G112/G113) . . . . . . . . .	2-34
	2.2.12	Cylindrical interpolation G07.1 (G107) . . . . . . . . . . . . . . . . . . . . . . . . . .	2-35
	2.2.13	Interrupt program with M96 / M97 (ASUB) . . . . . . . . . . . . . . . . . . . . . . .	2-37
	2.2.14	Comments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-39
	2.2.15	Block skip . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-40
	2.2.16	Auxiliary function output . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-41
	2.2.17	Align first reference point G28 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-42
	2.2.18	Enable/disable feed–forward control using G08 P.. . . . . . . . . . . . . . . .	2-42
	2.2.19	Compressor in ISO dialect mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-43
	2.2.20	Automatic corner override G62 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-44
	2.3	Subprogram and macro technology . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-46
	2.3.1	Subprogram technology: M98 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-46
	2.3.2	Siemens language commands in ISO Dialect mode . . . . . . . . . . . . . .	2-48

2.3.3Extending the subprogram call for contour preparation

		with CONTPRON . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-49
	2.3.4	Macro commands with G65, G66 and G67 . . . . . . . . . . . . . . . . . . . . . .	2-51
	2.3.5	Mode changing in macro calls with G65 / G66 . . . . . . . . . . . . . . . . . . .	2-54
	2.3.6	Macro call with M function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-55
	2.3.7	Macro call with G function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-56
	2.3.8	High-speed cycle cutting G05 P.. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-58
	2.3.9	Switchover modes for DryRun and skip levels . . . . . . . . . . . . . . . . . . .	2-59
	2.3.10	Eight–digit program numbers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-60
	2.4	Tool change and tool offsets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-61
	2.4.1	Tool offsets: T, D, M (ISO Dialect M) . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-61
	2.4.2	Possible H numbers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-62
	2.4.3	Tool offset: T (ISO Dialect T) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-65
	2.4.4	Tool-changing cycle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	2-67
3	Cycles and Contour Definition . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		3-69
	3.1	Calling cycles in the external CNC system using G commands . . . . .	3-69
	3.2	Global user data (GUD) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-71
	3.3	Drilling cycles (ISO Dialect M) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-74

Siemens AG, 2002. All rights reserved	ix
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

	3.3.1	Overview and parameter description . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-74
	3.3.2	Description of shell cycle CYCLE381M . . . . . . . . . . . . . . . . . . . . . . . . .	3-77
	3.3.3	Description of shell cycle CYCLE383M . . . . . . . . . . . . . . . . . . . . . . . . .	3-77
	3.3.4	Description of shell cycle CYCLE384M . . . . . . . . . . . . . . . . . . . . . . . . .	3-78
	3.3.5	Description of shell cycle CYCLE387M . . . . . . . . . . . . . . . . . . . . . . . . .	3-79
	3.4	Turning and drilling cycles (ISO Dialect T) . . . . . . . . . . . . . . . . . . . . . . .	3-80
	3.4.1	Turning cycles G70 to G76 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-80
	3.4.2	Turning cycles G77 to G79 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-86
	3.4.3	Drilling cycles G80 to G89 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-88
	3.4.4	Description of shell cycle CYCLE383T . . . . . . . . . . . . . . . . . . . . . . . . . .	3-90
	3.4.5	Description of shell cycle CYCLE384T . . . . . . . . . . . . . . . . . . . . . . . . . .	3-91
	3.4.6	Description of shell cycle CYCLE385T . . . . . . . . . . . . . . . . . . . . . . . . . .	3-92
	3.5	System variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-93
	3.6	Programming contour definitions (ISO Dialect T) . . . . . . . . . . . . . . . . .	3-96
	3.6.1	End point programming with angles . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-97
	3.6.2	Straight line with angle . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-98
	3.6.3	Two straight lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-99
	3.6.4	Three straight lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-101
	3.6.5	Polygon turning with G51.2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-103
	3.6.6	Contour repetition G72.1 / G72.2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	3-104
4	Start-Up .	. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-107
	4.1	Machine data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-107
	4.1.1	Active G command to PLC . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-112
	4.1.2	Tool change, tool data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-112
	4.1.3	G00 always with exact stop . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-113
	4.1.4	Response to syntax errors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-113
	4.1.5	Selection of code system A, B, C (ISO Dialect T) . . . . . . . . . . . . . . . .	4-114
	4.1.6	Fixed feedrates F0–F9 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-115
	4.1.7	Parallel axes G17<axis name>.. (G18 / G19) . . . . . . . . . . . . . . . . . . . .	4-116
	4.1.8	Insertion of chamfers and radii . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-117
	4.1.9	Rotary axis function . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	4-118
	4.1.10	Program coordination between two channels and M functions . . . . . .	4-119
	4.2	Default assignment of machine data for ISO Dialect . . . . . . . . . . . . . .	4-120
5	Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		5-123
	5.1	Restrictions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	5-123
	5.1.1	Program commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	5-124
	5.1.2	Tool management . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	5-126
	5.1.3	Control system response to Power ON, Reset and block search . . .	5-127
6	Data Descriptions (MD, SD) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		6-129
	6.1	General machine data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	6-129
	6.2	Channel-specific machine data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	6-145
	6.3	Axis-specific setting data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	6-152
	6.4	Channel-specific setting data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	6-153

x	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

7	Signal Descriptions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		8-157
8	Example	. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	8-157
9	Data Fields, Lists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		9-159
	9.1	Machine data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	9-159
	9.2	Setting data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	9-161
10	Alarms . .	. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	10-163
A	References . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		A-167
	Index . . .	. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .	I-179
	Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .		I-181

Siemens AG, 2002. All rights reserved	xi
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

Notes

xii	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

Brief Description

1

Introduction	Parts programs can be read in from external CNC systems, and can then be
	edited and executed.
	This manual describes the startup measures and procedures necessary to run
	NC programs created on an external CNC system. Functional differences are
	also explained.
	Note
	For a detailed description of the external programming functions, please refer
	to the original documentation of the external CNC system.

Terms used	The following terms are defined for this manual:
	S ISO Dialect M is similar to the G code of the “Fanuc16 Milling” control
	S	ISO Dialect T is similar to the G code of the “Fanuc16 Turning” control
		System B
	S	ISO Dialect Original is equivalent to the original Fanuc16 control.

J

Siemens AG, 2002. All rights reserved	1-13
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

1 Brief Description

10.02

Notes

1-14	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

Programming

2

2.1Activation of functions

Machine data 18800 $MN_EXTERN_LANGUAGE is used to activate the external language. The language type, ISO Dialect–M or T is selected with machine data 10880 $MN_EXTERN_CNC_SYSTEM.

The external language can be activated separately for each channel. For example, channel 1 can operate in ISO mode but channel 2 is active in Siemens mode.

Switchover	The following two G commands from Group 47 are used to switch between
	Siemens mode and ISO Dialect mode:
	S	G290	Siemens NC programming language active
	S	G291	ISO Dialect NC programming language active

The active tool, tool offsets and zero offsets remain active here (see Subsection 2.2.4 and Section 2.4).

Siemens mode	The following conditions apply when Siemens mode is active:
	S Siemens G commands are interpreted on the control by default.
	S It is not possible to extend the Siemens programming system with ISO
	Dialect functions because some of the G functions have different meanings.
	S Downloadable MD files can be used to switch the control to ISO Dialect
	mode. In this case, the user sees the ISO Dialect mode by default.

ISO Dialect mode The following conditions apply when ISO Dialect mode is active:

SOnly ISO Dialect G codes can be programmed, not Siemens G codes.

SIt is not possible to use a mixture of ISO Dialect code and Siemens code in the same NC block.

SIt is not possible to switch between ISO Dialect M and ISO Dialect T via G command

SIf further Siemens functions are to be used, it is necessary to switch to Siemens mode first (exception: program branches and subprogram calls, see Subsection 2.3.2)

Siemens AG, 2002. All rights reserved	2-15
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming	10.02
2.1 Activation of functions
Power ON/Reset	Table 2-1 shows the possible combinations of machine data
	$MN_EXTERN_CNC_SYSTEM and $MC_GCODE_RESET_VALUE. This
	specifies the Power ON/Reset response.

Table 2-1	Activation of functions
After Power ON/Reset...		$MC_GCODE_RESET_VA-		$MN_EXTERN_CNC_SYSTEM
		LUES[46] =		=
Siemens mode active, switch-		1	G290 Siemens mode	1	ISO Dialect M
over to ISO Dialect M possible
Siemens mode active, switch-		1	G290 Siemens mode	2	ISO Dialect T
over to ISO Dialect T possible
ISO Dialect M active, switchover		2	G291 ISO Dialect mode	1	ISO Dialect M
to Siemens mode possible
ISO Dialect T active, switchover		2	G291 ISO Dialect mode	2	ISO Dialect T
to Siemens mode possible

Modal

G commands

Modal G commands which have the same function in both systems (Siemens and ISO Dialect) are treated as follows.

When these G codes are programmed in one language, the equivalent G code in the other language is determined and activated. The following G codes are affected:

Data management ISO programs can be both read into and output from the MMC 103 in punchtape format.

ISO programs which have been read in are stored in the NC data management system as main programs in the default path: _N_WKS_DIR/_N_SHOPMILL_WPD.

	You can change the entry by editing the file DINO.INI in the USER directory. You
	will find further information in the publication
	References: /IAM/, IM3: MMC Installation and Startup Guide, Section 3.1.
2.1.1	Switchover from ISO mode to Siemens mode
G290/291	G commands 290/291 can be used from the parts program to change mode.
	On switchover, the display of current G codes also changes.
G65/66	Non-modal and modal macro:
	The programmed subprogram is called. Switchover to Siemens mode only
	takes place when the PROC instruction is used in the first line of the

subprogram.

If a program of this type is terminated with M17 or RET, when the subprogram returns, the mode is switched back to ISO mode.

2-16	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02

2 Programming

Siemens subprogram call in ISO mode

Modal, non-modal cycles

2.1 Activation of functions

Modal and non-modal subprogram calls, e.g.

N100 CALL “SHAFT”

or

N100 MCALL SHAFT

or

N100 SHAFT

Modal and non–modal subprogram calls with parameter passing

N100 MCALL SHAFT(”ABC”, 33.5) or

N100 SHAFT(“ABC”, 33.5)

Subprogram calls with path name
N100 CALL “/_N_SPF_DIR/SHAFT		or
N100	MCALL /_N_SPF_DIR/SHAFT	or
N100	PCALL /_N_SPF_DIR/SHAFT

Siemens mode is selected implicitly on subprogram calls, and the system is switched back to ISO Dialect mode at the end of the subprogram.

If a modal or non-modal cycle is programmed in ISO mode, a shell cycle will be called.

This call results in switchover to Siemens mode.

Siemens AG, 2002. All rights reserved	2-17
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming	10.02
2.2 G commands

2.2G commands

The G codes of ISO Dialect T refer to G code system B (see also 4.1.5).

The active G codes in ISO mode can be read using system variable $P_EXTGG[...]. The numbers alongside the G code specify the respective value in $P_EXTGG[...]. Machine data 20154 EXTERN_GCODE_RESET_VALUES[n]: 0, ..., 30 is used to specify the G codes that are effective on start–up when the NC channel is not operating in Siemens mode.

Table 2-2			The default setting is indicated by 1)
	ISO			ISO		Description
Dialect T				Dialect M
Group 1
G00 1)		1		G00 1)	1	Rapid traverse
G01		2		G01	2	Linear motion
G02		3		G02	3	Circle/helix, clockwise
				G02.2	6	Involute, clockwise
G03		4		G03	4	Circle/helix, counterclockwise
				G03.2	7	Involute, counterclockwise
G33		5		G33	5	Thread cutting with constant lead
G34		9				Thread cutting with variable lead
G77		6				Longitudinal turning cycle
G78		7				Thread cutting cycle
G79		8				Face turning cycle
Group 2
				G17 1)	1	XY plane
				G18	2	ZX plane
				G19	3	YZ plane
G96		1				Constant cutting rate ON
G97 1)		2				Constant cutting rate OFF
Group 3
G90	1)	1		G90 1)	1	Absolute programming
G91		2		G91	2	Incremental programming
Group 4
				G22	1	Working area limitation, protection zone 3 ON
				G23 1)	2	Working area limitation, protection zone 3 OFF
G68		1				Double turret/slide on
G69		2				Double turret/slide off

2-18	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02						2 Programming
						2.2 G commands
	Table 2-2		The default setting is indicated by 1)
	ISO			ISO		Description
	Dialect T			Dialect M
	Group 5
				G93	3	Inverse–time feedrate (rpm)
	G94	1		G94 1)	1	Feed in [mm/min, inch/min]
	G95 1)	2		G95	2	Revolutional feedrate in [mm/rev, inch/rev]
	Group 6
	G20 1)	1		G201)	(G70) 1	Input system inch
	G21	2		G21	(G71) 2	Input system metric
	Group 7
	G40 1)	1		G40 1)	1	Deselect cutter radius compensation
	G41	2		G41	2	Compensation to left of contour
	G42	3		G42	3	Compensation to right of contour
	Group 8
				G43	1	Tool length compensation positive ON
				G44	2	Tool length compensation negative ON
				G49 1)	3	Tool length compensation OFF
	Group 9
	G22	1				Working area limitation, protection zone 3 ON
	G23	2				Working area limitation, protection zone 3 OFF
				G73	1	Deep hole drilling cycle with chipbreaking
				G74	2	Counterclockwise tapping cycle
				G76	3	Fine drilling cycle
				G80 1)	4	Cycle OFF
				G81	5	Counterbore drilling cycle
				G82	6	Countersink drilling cycle
				G83	7	Deep hole drilling cycle with swarf removal
				G84	8	Clockwise tapping cycle
				G85	9	Drilling cycle
				G86	10	Drilling cycle, retraction with G00
				G87	11	Reverse countersinking
				G89	13	Drilling cycle, retraction with machining feed
	Group 10
	G80 1)	1				Drilling cycle OFF
	G83	2				Face deep hole drilling
	G84	3				Face tapping
	G85	4				End face drilling cycle

Siemens AG, 2002. All rights reserved	2-19
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming								10.02
2.2 G commands
	Table 2-2			The default setting is indicated by 1)
		ISO				ISO		Description
	Dialect T				Dialect M
	G87		5					Side deep hole drilling
	G88		6					Side tapping
	G89		7					Side drilling
					G98 1)		1	Return to starting point for fixed cycles
					G99		2	Return to point R for fixed cycles
	Group 11
	G98 1)		1					Return to starting point for drilling cycles
	G99		2					Return to point R for drilling cycles
					G50 1)		1	Scaling OFF
					G51		2	Scaling ON
	Group 12
	G66		1		G66		1	Modal macro call
	G67 1)		2		G67 1)			Delete modal macro call
	Group 13
					G96		1	Constant cutting rate ON
					G97 1)		2	Constant cutting rate OFF
	Group 14
	G54		1		G54 1)		1	Select zero offset
	G55		2		G55		2	Select zero offset
	G56		3		G56		3	Select zero offset
	G57		4		G57		4	Select zero offset
	G58		5		G58		5	Select zero offset
	G59		6		G59		6	Select zero offset
	G54	P{1...48}1			G54	P{1...48}1		Extended zero offsets
					G54.1		7	Extended zero offset
	G54	P0	1		G54	P0	1	“External ZO extOffset”
	Group 15
					G61		1	Exact stop modal
					G62		4	Automatic corner override
					G63		2	Tapping mode
					G64 1)		3	Continuous-path mode
	Group 16
	G17		1					XY plane
	G18 1)		2					ZX plane
	G19		3					YZ plane

2-20	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02								2 Programming
								2.2 G commands
	Table 2-2		The default setting is indicated by 1)
	ISO			ISO			Description
	Dialect T			Dialect M
				G68	1	Rotation ON	2D	3D
				G69	2	Rotation OFF
	Group 17
				G15 1)	1	Polar coordinates OFF
				G16	2	Polar coordinates ON
	Group 18 (non-modal)
	G04	1		G04	1	Dwell time in [s] or spindle revolutions
	G05	20		G05	18	High–speed cycle cutting
	G05.1	22		G05.1	20	High speed cycle –> call CYCLE305
	G07.1	18		G07.1	16	Cylindrical interpolation
				G08	12	Feedforward control ON/OFF
				G09	2	Exact stop
	G10	2		G10	3	Write zero offset/tool offset
	G10.6	19		G10.6	17	Rapid lift ON/OFF (T)
						Retraction from contour (POLF) (M)
				G11	4	Terminate parameter input
	G27	16		G27	13	Referencing check (available soon)
	G28	3		G28	5	Approach 1st reference point
	G30	4		G30	6	Approach 1st reference point
	G30.1	21		G30.1	19	Floating reference position
	G31	5		G31	7	Measurement with touch-trigger probe
	G52	6		G52	8	Programmable zero offset
	G53	17		G53	9	Approach position in machine coordinate system
	G65	7		G65	10	Call macro
	G70	8				Finishing cycle
	G71	9				Stock removal cycle longitudinal axis
	G72	10				Stock removal cycle transverse axis
				G72.1	14	Contour repetition with rotation
				G72.2	15	Contour repetition, linear
	G73	11				Repeat contour
	G74	12				Deep hole drilling and recessing in longitudinal axis
						(Z)
	G75	13				Deep hole drilling and recessing in facing axis (X)
	G76	14				Multiple thread cutting cycle
	G92	15		G92	11	Preset actual value memory, spindle speed limitation
	G92.1	23		G92.1	21	Reset actual value, reset WCS

Siemens AG, 2002. All rights reserved	2-21
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming						10.02
2.2 G commands
	Table 2-2		The default setting is indicated by 1)
	ISO			ISO		Description
	Dialect T			Dialect M
	Group 20
	G50.2	1				Polygon turning OFF
	G51.2	2				Polygon turning ON
	Group 21
	G13.1	1				TRANSMIT OFF
	G12.1	2				TRANSMIT ON
	Group 22
				G50.1	1	Mirroring on programmed axis OFF
				G51.1	2	Mirroring on programmed axis ON
	Group 25
				G13.1	1	Polar coordinates, interpolation
				G12.1	2	Polar coordinates, interpolation
	Group 31
	G290 1)	1		G290 1)	1	Select Siemens mode
	G291	2		G291	2	Select ISO Dialect mode

Table 2-3	G commands are functionally identical in Siemens mode and in ISO Dialect mode
G commands in Siemens mode		Corresponding G commands in	Corresponding G commands in
		ISO Dialect T	ISO Dialect M
Group 1: G00, G01, G02, G03,		Group 1: G00, G01, G02, G03, G33	Group 1: G00, G01, G02, G03, G33
G33
Group 6: G17, G18, G19		Group 16: G17, G18, G19	Group 2: G17, G18, G19
Group 7: G40, G41, G42		Group 7: G40, G41, G42	Group 7: G40, G41, G42
Group 8: G54 to G554			Group 14: G54 to G59, G54 P1 to P48
Group 10: G60, G64			Group 15: G60, G64
Group 13: G700, G710		Group 6: G20, G21	Group 6: G20, G21
Group 14: G90, G91		Group 3: G90, G91	Group 3: G90, G91
Group 15:	G94	Group 5: G94 Group 2: G97	Group 5: G94 Group 13: G97
	G95	Group 5: G95 Group 2: G97	Group 5: G95 Group 13: G97
	G96	Group 5: G95 Group 2: G96	Group 5: G95 Group 13: G96
	G961	Group 5: G94 Group 2: G96	Group 5: G94 Group 13: G96
	G97	Group 5: G95 Group 2: G97	Group 5: G95 Group 13: G97
	G971	Group 5: G94 Group 2: G97	Group 5: G94 Group 13: G97

2-22	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02	2 Programming
	2.2 G commands

Note

If individual G codes of the groups in Table 2-3 cannot be mapped, the default setting in machine data

$MC_EXTERN_GCODE_RESET_VALUES and/or $MC_GCODE_RESET_VALUES

is activated.

Example: ISO mode

N5	G00	X100. Y100.
N10	G90		;Activate G90 in ISO mode Group 3
			;In Siemens mode Group 14
N15	G290		;Switch over to Siemens, G90 is active
N20	G91		;Activate G91 in ISO mode Group 3
			;In Siemens mode Group 14
N25	G291		;Switch over to ISO mode
N30	G291		;G91 is active

2.2.1G code display

In the G code display, the G codes for the currently active language are displayed. G290/G291 also causes the G code display to switch over.

Example:

The Siemens standard cycles are called up using some of the ISO Dialect mode G functions (e.g. G28). DISPLOF is programmed at the start of the cycle, with the result that the ISO Dialect G commands remain active for the display.

PROC CYCLE328 SAVE DISPLOF

N10 ...

...

N99 RET

Sequence:

SExternal main program calls Siemens shell cycle. Siemens mode is selected implicitly on the shell cycle call.

SDISPLOF freezes the block display at the call block;

the G code display remains in external mode. This display is refreshed while the Siemens cycle is running.

2.2.2Display of non–modal G codes

As of SW 6.4 the external non–modal G codes (group 18) will no longer be reset on block change if these G codes call up subprograms. The G codes remain visible on the display until the next jump out of this subprogram.

Switching to external language mode in the subprogram and programming another G code from group 18 overwrites the previous value and the new value is retained until the return jump.

Example:

Siemens AG, 2002. All rights reserved	2-23
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming					10.02
2.2 G commands
Main program					Display group 18
N05	G00		X0 Y0		empty
N08	G27		X10	–> calls Cycle328	empty
N09	M0				empty
N40	M30				empty
Subprogram Cycle328					Display group 18
N100 G290					G27
N102		X=$C_X			G27
N103		M0			G27
N104		G291			G27
N105		G30 X10 Y12 Z13			G30
N120		M99			G30

2.2.3G code output to PLC (as from SW 6.4)

The behavior of G group transfer to PLC is described in machine data $MC_GCODE_GROUPS_TO_PLC_MODE.

The previous behavior was for the G group to be the array index of a 64 byte field (DBB 208 – DBB 271). That way, up to the 64th G group can be reached. Only the G groups of the standard or external language can be displayed.

The new behavior is for the data storage in the PLC to be up to 8 bytes (DBB 208 – DBB 215), i.e. up to 8 G groups can be output.

This method has the array index of machine data $MC_GCODE_GROUPS_TO_PLC[ ] or $MC_EXTERN_GCODE_GROUPS_TO_PLC[ ] equal to the array index of the data storage in the PLC (DBB 208 – DBB215).

The G code group from MD $MC_GCODE_GROUPS_TO_PLC[ ] is output in DBB 208.

The advantage is that Siemens mode and ISO mode G codes can be output simultaneously.

Because only the G code of one language can be output in a DBB2xx, each index (0 –7) can only be set on one of the two machine data, and the value 0 must be entered in the other MD. Errors are signaled with Alarm 4045.

Example $MC_GCODE_GROUPS_TO_PLC[0]=3 $MC_GCODE_GROUPS_TO_PLC[1]=0 $MC_GCODE_GROUPS_TO_PLC[2]=0 $MC_GCODE_GROUPS_TO_PLC[3]=0 $MC_GCODE_GROUPS_TO_PLC[4]=1 $MC_GCODE_GROUPS_TO_PLC[5]=2 $MC_GCODE_GROUPS_TO_PLC[6]=0 $MC_GCODE_GROUPS_TO_PLC[7]=0

$MC_EXTERN_GCODE_GROUPS_TO_PLC[0]=0 $MC_EXTERN_GCODE_GROUPS_TO_PLC[1]=3 $MC_EXTERN_GCODE_GROUPS_TO_PLC[2]=18 $MC_EXTERN_GCODE_GROUPS_TO_PLC[3]=1 $MC_EXTERN_GCODE_GROUPS_TO_PLC[4]=0 $MC_EXTERN_GCODE_GROUPS_TO_PLC[5]=0 $MC_EXTERN_GCODE_GROUPS_TO_PLC[6]=6 $MC_EXTERN_GCODE_GROUPS_TO_PLC[7]=31

The following G codes are then available on the PLC

2-24	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02	2 Programming
	2.2 G commands

DBB 208 = group 03 Siemens

DBB 209 = group 03 ISO dialect

DBB 210 = group 18 ISO dialect

DBB 211 = group 01 ISO dialect

DBB 212 = group 01 Siemens

DBB 213 = group 02 Siemens

DBB 214 = group 06 ISO dialect

DBB 215 = group 31 ISO dialect

Example of faulty configuration:

$MC_GCODE_GROUPS_TO_PLC[0]=3 $MC_GCODE_GROUPS_TO_PLC[1]=0 $MC_GCODE_GROUPS_TO_PLC[2]=0

$MC_EXTERN_GCODE_GROUPS_TO_PLC[0]=3 –>

Alarm 4045, channel K1 conflict between machine data {S$MC_GCODE_GROUPS_TO_PLC} and machine data {S$MC_EXTERN_GCODE_GROUPS_TO_PLC}

$MC_EXTERN_GCODE_GROUPS_TO_PLC[1]=0

$MC_EXTERN_GCODE_GROUPS_TO_PLC[2]=18

The method enables simultaneous display of G codes of standard mode and

ISO dialect mode.

Siemens AG, 2002. All rights reserved	2-25
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming	10.02
2.2 G commands

2.2.4Zero offset

The zero offsets (ZO) of Siemens mode are shown in Fig. 2-1.

						Progr. frame	G52 ZO
						$P_BFRAME	G51 scale
					Settable frame G54 – G59 ZO
					$P_UIFR		G54 P1..100 ZO
					Channel-specific base frame
				$P_CHBFRAME[3]		G68 3DRot
				$P_CHBFRAME[2]		G68 2DRot/3DRot
			$P_CHBFRAME[1]			Mirroring on progr. axis
			$P_CHBFRAME[0]			G92 Preset actual value memory
			$P_CHBFRAME[0]			ZO extOffset

Fig. 2-1 Instantaneous mapping of the ISO functions onto the Siemens frames

The zero offsets that are available in ISO mode are mapped onto the existing Siemens frames. No separate frames exist for ISO mode. Active zero offsets are incorporated in both language modes.

Changes in ISO mode have an immediate effect in Siemens mode and vice–versa.

Zero offsets exist in both ISO Dialect T and ISO Dialect M:

SG52 is a programmable, additive ZO that remains active until the end of the program or a reset

SG54 to G59 are settable zero offsets

SG54 P1...P100 are additional settable zero offsets

SG54 P0 is an “external ZO” extOffset

2-26	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02	2 Programming
	2.2 G commands
G54.1	G54.1 Pxx is provided as an alternative notation to G54 Pxx. The functionality is
	identical. With G54.1 the P address must always be programmed in the block. If
	P is not programmed, alarm 12080 (syntax error) is produced.

2.2.5Writing a zero offset with G10

G10 can be used from the parts program to write the zero offsets.

G10 L2		P1...P6 X.. Y..	; G54.. G59
G10	L20 P1...P100		; Additional, settable ZO
G10	L2	P0	External ZO extOffset

These zero offsets are mapped onto the same frames as the zero offsets that already exist in ISO Dialect M.

The G10 command is extended for ISO dialect T :

Writing of system data

G10 Pxx X Y Z ;writing of tool offset data

Depending on machine data $MC_EXTERN_FUNCTION_MASK, bit1, G10

Pxx is used to write either tool geometry or tool wear.

$MC_EXTERN_FUNCTION_MASK, bit1 = 0: P > 100 write geometry values

P < 100 write wear values

$MC_EXTERN_FUNCTION_MASK, bit 1=1: P > 10000 write geometry values

P < 10000 write wear values

2.2.6Decimal point programming

There are two notations for the interpretation of programming values without a decimal point in ISO Dialect mode:

SPocket calculator type notation

Values without decimal points are interpreted as mm, inch or degrees.

SStandard notation

Values without decimal points are multiplied by a conversion factor.

The setting is defined by MD 10884, see Chapter 4 “Startup”.

There are two different conversion factors, IS-B and IS-C. This evaluation refers to addresses X Y Z U V W A B C I J K Q R and F.

Example of linear axis in mm:

X 100.5 corresponds to value with decimal point: 100.5mm X 1000 pocket calculator type notation: 1000mm

standard notation: IS-B: 1000* 0.001= 1mm IS-C: 1000* 0.0001 = 0.1mm

Siemens AG, 2002. All rights reserved	2-27
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming	10.02
2.2 G commands

ISO dialect Milling

Table 2-4	Different conversion factors for IS-B and IS-C
Address		Unit	IS-B	IS-C
Linear axis		mm	0.001	0.0001
		inch	0.0001	0.00001
Rotary axis		deg	0.001	0.0001
F feed G94 (mm/inch per min.)		mm	1	1
		inch	0.01	0.01
F feed G95 (mm/inch per min.)		mm	0.01	0.01
		inch	0.0001	0.0001
F thread pitch		mm	0.01	0.01
		inch	0.0001	0.0001
C chamfer		mm	0.001	0.0001
		inch	0.0001	0.00001
R radius, G10 toolcorr		mm	0.001	0.0001
		inch	0.0001	0.00001
Q		mm	0.001	0.0001
		inch	0.0001	0.00001
I, J, K interpolation parameters		mm	0.001	0.0001
		inch	0.0001	0.00001
G04 X or U		S	0.001	0.001
A contour angle		deg	0.001	0.0001
G74, G84 thread drilling cycles
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0 F feedrate like G94, G95
Bit8 = 1 F thread pitch

ISO dialect

Turning

Table 2-5	Different conversion factors for IS-B and IS-C
Address		Unit	IS-B	IS-C
Linear axis		mm	0.001	0.0001
		inch	0.0001	0.00001
Rotary axis		deg	0.001	0.0001
F feed G94 (mm/inch per min.)		mm	1	1
		inch	0.01	0.01
F feed G95 (mm/inch per rev)
$MC_EXTERN_FUNCTION_MASK
Bit8 = 0		mm	0.01	0.01
		inch	0.0001	0.0001
Bit8 = 1		mm	0.0001	0.0001
		inch	0.000001	0.000001
F thread pitch		mm	0.0001	0.0001
		inch	0.000001	0.000001
C chamfer		mm	0.001	0.0001
		inch	0.0001	0.00001
R radius, G10 toolcorr		mm	0.001	0.0001
		inch	0.0001	0.00001

2-28	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

10.02				2 Programming
				2.2 G commands
	Table 2-5	Different conversion factors for IS-B and IS-C
	Address		Unit	IS-B	IS-C
	I, J, K interpolation parameters		mm	0.001	0.0001
			inch	0.0001	0.00001
	G04 X or U			0.001	0.001
	A contour angle			0.001	0.0001
	G76, G78 thread drilling cycles
	$MC_EXTERN_FUNCTION_MASK
	Bit8 = 0 F feedrate like G94, G95
	Bit8 = 1 F thread pitch
	G84, G88 thread drilling cycles
	$MC_EXTERN_FUNCTION_MASK
	Bit9 = 0	G95 F	mm	0.01	0.01
			inch	0.0001	0.0001
	Bit8 = 1	G95 F	mm	0.0001	0.0001
			inch	0.000001	0.000001

2.2.7Dwell time in spindle revolutions G04

MD $MC_EXTERN_FUNCTION_MASK, bit 2 defines how the programmed dwell time will be interpreted in a G04 block. The hold time can be programmed using G04 X U or P.

Bit 2 = 0: Dwell time is always interpreted in [s].

Bit 2 = 1: If G95 is active, dwell time is interpreted in spindle revolutions.

In the case of standard notation, X and U values without a decimal point are converted into internal units depending on IS-B or IS-C. P is always interpreted in internal units.

Example:

N5 G95 G04 X1000 Standard notation 1000 * 0.001 = 1 spindle revolution pocket calculator notation: 1000 spindle revolutions

2.2.8Scaling and mirroring: G51, G51.1 (ISO Dialect M)

G51 selects scaling and mirroring, G51.1.

There are two scaling modes:

SAxial scaling with parameters I, J, K

If I, J, K is not programmed in the G51 block, the default value from the setting data is effective.

Negative axial scaling factors have the additional effect of mirroring.

SScaling in all axes with scale factor P

If P is not programmed in the G51 block, the default value from the setting data is effective. Negative P values are not possible.

The scale factors are multiplied by either 0.001 or 0.00001.

Siemens AG, 2002. All rights reserved	2-29
SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition

2 Programming

10.02

2.2 G commands

Example

Note

If a factor other than “1” is programmed for parameters I, J, K or if the address is missing (default value is active for I, J, K), the contour is also scaled.

00512 (parts program)
N10	G17	G90	G00 X0 Y0	Approach start position
N30	G90	G01	G94 F6000
N32	M98	P0513		1) Contour programmed as in the
				subprogam
N34	G51	X0.	Y0. I-1000 J1000	2) Mirror contour around X
N36	M98	P0513
N38	G51	X0.	Y0. I-1000 J-1000	3) Mirror contour around X and Y
N40	M98	P0513
N42	G51	X0.	Y0. I1000 J-1000	4) Mirror contour around Y
N44	M98	P0513
N46	G50			Deselect scaling and mirroring
N50	G00	X0 Y0
N60	M30
00513 (subprogram)
N10	G90	X10. Y10.
N20	X50
N30	Y50
N40	X10. Y10.
N50	M99

50
2)				1)
10		Starting point
0
–10				4)
3)
–50
–50	–10	0	10	50

Fig. 2-2 Scaling and mirroring

System parameter settings for the scaling and mirroring example:

MD 22910 $MC_WEIGHTING_FACTOR_FOR_SCALE = 0 MD 22914 $MC_AXES_SCALE_ENABLE = 1

MD 10884 $MN_EXTERN_FLOATINGPOINT_PROG = 0 MD 10886 $MN_EXTERN_INCREMENT_SYSTEM = 0

Axial scaling is not possible when MD $MC_AXES_SCALE_ENABLE = 0.

2-30	Siemens AG, 2002. All rights reserved
	SINUMERIK 840D/840Di/810D, Description of Functions ISO Dialects (FBFA) – 11.02 Edition