SINUMERIK 840D sl. Service - Functions. Manual (2018-2020)

Table of contents

Preface

Fundamental safety instructions

1.1

General safety instructions

1.2

Warranty and liability for application examples

1.3

Industrial security

Short description

Programming

3.1

Function activation

3.1.1

Switching between the operating modes

3.2

G commands

3.2.1

Display of the G code

3.2.2

Display of non-modal G codes

3.2.3

G code output to PLC

3.2.4

Decoupling the frames between Siemens and ISO mode

3.2.5

Writing work offset with G10

3.2.6

Programming the decimal point

3.2.7

Rapid lifting with G10.6

3.2.8

Multiple-start threads with G33

3.2.9

Thread with variable lead G34 (ISO dialect T)

3.2.10

Dwell time in spindle revolutions G04

3.2.11

Scaling (G50, G51) and mirroring G50.1, G51.1 (ISO dialect M)

3.2.12

G60 directed positioning

3.2.13

2D/3D rotation G68/G69 (ISO dialect M)

3.2.14

Double slide or double turret processing G68/G69

3.2.15

Polar coordinates G15/G16 (ISO dialect M)

3.2.16

Interpolation of polar coordinates G12.1/G13.1 (G112/G113)

3.2.17

Cylindrical interpolation G07.1 (G107)

3.2.18

Interrupt program with M96/M97 (ASUB)

3.2.19

Comments

3.2.20

Skip block

3.2.21

Auxiliary function output

3.2.22

Approach 1st home position with intermediate point (G28)

3.2.23

Switching precontrol on/off with G08 P

3.2.24

Compressor in ISO dialect mode

3.2.25

Automatic corner override G62

3.3

Substitution by a substitution cycle with a tool selection block

3.3.1

Milling

3.3.2

Turning

3.3.3

Indirect programming in ISO mode using $ variables

3.4

Subprogram and macro technology

3.4.1

Subprogram technique: M98

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Table of contents

3.4.2

Siemens language commands in ISO dialect mode

3.4.3

Expansion of subprogram call for contour preparation with CONTPRON

3.4.4

Macro commands with G65, G66 and G67

3.4.5

Changing mode during macro calls with G65/G66

3.4.6

Macro call via M function

3.4.7

Macro call via G function

3.4.8

High-speed cycle cutting G05 P

3.4.9

Switchover modes for DryRun and skip planes

3.4.10

Eight-digit program number

3.4.11

System variable for level stack in ISO mode

Tool changes and tool offsets

4.1

Shared tool offset memory

4.1.1

Tool offsets: T, D (ISO dialect M)

4.1.2

Possible H numbers

4.1.3

Tool offset T (ISO dialect T)

4.1.4

Tool change cycle

Cycles and contour definition

5.1

Sequence of cycle calls in the external CNC system using G commands

5.2

Global user data (GUD)

5.3

Drilling cycles (ISO dialect M)

5.3.1

Overview and parameter description

5.3.2

Description of shell cycle CYCLE381M

5.3.3

Description of shell cycle CYCLE383M

5.3.4

Description of shell cycle CYCLE384M

5.3.5

Description of shell cycle CYCLE387M

5.4

Turning and drilling cycles (ISO dialect T)

5.4.1

Turning cycles G70 to G76

5.4.2

Turning cycles G77 to G79

105

5.4.3

Drilling cycles G80 to G89

107

5.4.4

Description of shell cycle CYCLE383T

110

5.4.5

Description of shell cycle CYCLE384T

111

5.4.6

Description of shell cycle CYCLE385T

112

5.5

System variables

112

5.6

Programming contour definitions

115

5.6.1

End point programming with angles

116

5.6.2

Straight line with angle

117

5.6.3

Two straight lines

118

5.6.4

Three straight lines

119

5.6.5

Multi-edge turning with G51.2

121

5.6.6

Contour repetition G72.1/G72.2

122

5.6.7

Output on an external device / an external file

124

5.6.8

Convex thread with G35 and G36

126

Commissioning

127

6.1

Machine data

127

6.1.1

Active G command for PLC

132

6.1.2

Tool change, tool data

132

6.1.3

G00 always with exact stop

133

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Table of contents

6.1.4

Response to syntax faults

133

6.1.5

Selection of code system A, B, C (ISO dialect T)

134

6.1.6

Fixed feedrates F0 - F9

135

6.1.7

Parallel axes G17 (G18/G19)<Axis name>

136

6.1.8

Inserting chamfers and radii

137

6.1.9

Rotary axis function

138

6.1.10

Program coordination between 2 channels and M commands

139

6.2

Standard machine data assignment for ISO dialect

140

Supplementary conditions

143

7.1

Supplementary conditions

143

7.2

Constraints

143

7.2.1

Program commands

143

7.2.2

Tool management

145

7.2.3

Control response with power on, reset and block search

146

Data descriptions (MD, SD)

149

8.1

General NC machine data

149

8.2

Channel-specific machine data

164

8.3

Axis-specific machine data

179

8.4

Channel-specific setting data

181

8.5

Axis-specific setting data

184

8.6

Channel-specific cycle machine data

185

8.7

Channel-specific cycle setting data

187

Data fields, lists

189

9.1

Machine data

189

9.2

Setting data

191

Alarms

193

Appendix

197

11.1

Documentation overview SINUMERIK 840D sl

197

11.2

Documentation overview SINUMERIK 828D

198

Index

199

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Fundamental safety instructions

1.1

General safety instructions

WARNING

Danger to life if the safety instructions and residual risks are not observed

If the safety instructions and residual risks in the associated hardware documentation are not

observed, accidents involving severe injuries or death can occur.

● Observe the safety instructions given in the hardware documentation.

● Consider the residual risks for the risk evaluation.

WARNING

Malfunctions of the machine as a result of incorrect or changed parameter settings

As a result of incorrect or changed parameterization, machines can malfunction, which in turn

can lead to injuries or death.

● Protect the parameterization against unauthorized access.

● Handle possible malfunctions by taking suitable measures, e.g. emergency stop or

emergency off.

1.2

Warranty and liability for application examples

Application examples are not binding and do not claim to be complete regarding configuration,

equipment or any eventuality which may arise. Application examples do not represent specific

customer solutions, but are only intended to provide support for typical tasks.

As the user you yourself are responsible for ensuring that the products described are operated

correctly. Application examples do not relieve you of your responsibility for safe handling when

using, installing, operating and maintaining the equipment.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Fundamental safety instructions

1.3 Industrial security

1.3

Industrial security

Note

Industrial security

Siemens provides products and solutions with industrial security functions that support the

secure operation of plants, systems, machines and networks.

In order to protect plants, systems, machines and networks against cyber threats, it is

necessary to implement - and continuously maintain - a holistic, state-of-the-art industrial

security concept. Products and solutions from Siemens constitute one element of such a

concept.

Customers are responsible for preventing unauthorized access to their plants, systems,

machines and networks. Such systems, machines and components should only be connected

to an enterprise network or the Internet if and to the extent such a connection is necessary and

only when appropriate security measures (e.g. using firewalls and/or network segmentation)

are in place.

For additional information on industrial security measures that can be implemented, please

visit:

Industrial security (https://www.siemens.com/industrialsecurity )

Siemens’ products and solutions undergo continuous development to make them more secure.

Siemens strongly recommends that product updates are applied as soon as they become

available, and that only the latest product versions are used. Use of product versions that are

no longer supported, and failure to apply the latest updates may increase customer’s exposure

to cyber threats.

To stay informed about product updates, subscribe to the Siemens Industrial Security RSS

Feed at:

Industrial security (https://www.siemens.com/industrialsecurity )

Further information is provided on the Internet:

Industrial Security Configuration Manual (https://support.industry.siemens.com/cs/ww/en/

view/108862708)

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Fundamental safety instructions

1.3 Industrial security

WARNING

Unsafe operating states resulting from software manipulation

Software manipulations, e.g. viruses, Trojans, or worms, can cause unsafe operating states

in your system that may lead to death, serious injury, and property damage.

● Keep the software up to date.

● Incorporate the automation and drive components into a holistic, state-of-the-art industrial

security concept for the installation or machine.

● Make sure that you include all installed products into the holistic industrial security concept.

● Protect files stored on exchangeable storage media from malicious software by with

suitable protection measures, e.g. virus scanners.

● On completion of commissioning, check all security-related settings.

● Protect the drive against unauthorized changes by activating the "Know-how protection"

converter function.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Short description

Introduction

Part programs from external CNC systems can be read in and executed.

This brochure describes the commissioning required for this and how NC programs from an

external CNC system are processed. Functional differences are also explained.

Note

You will find a detailed description of the external program functions in the original

documentation provided for the external CNC system.

Terms used

The following terms are defined for this brochure:

● ISO dialect M is similar to the G code of the "Fanuc16-Milling" control system

● ISO dialect T is similar to the G code of the "Fanuc16-Turning" system B control system

● ISO dialect original corresponds to the original Fanuc16 control system

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.1

Function activation

Switchover

The 18800 $MN_EXTERN_LANGUAGE machine data is used to activate the external

language. The ISO dialect M or T language types can be selected via 10880

$MN_EXTERN_CNC_SYSTEM machine data.

The external language can be activated separately for each channel. For example, channel 1

can run in ISO mode while channel 2 is active in Siemens mode.

The two G commands from group 47 are used to switch from Siemens mode to ISO dialect

mode:

● G290: Siemens NC programming language active

● G291: ISO dialect NC programming language active

The active tool, tool offsets and work offsets are retained.

G290 and G291 must be the only components of an NC program block.

Siemens mode

The following conditions are valid in the Siemens mode:

● The default of the G commands can be defined for each channel via the 20150

$MC_GCODE_RESET_VALUE machine data.

● No language commands from the ISO dialects can be programmed in Siemens mode.

ISO dialect mode

The following conditions apply when ISO dialect mode is active:

● The ISO dialect mode can be set with machine data as the default setting for the control

system. In ISO dialect mode, the control system then reboots by default.

● Only G commands from the ISO dialect can be programmed; the programming of Siemens

G functions is not possible in ISO mode.

● ISO dialect and Siemens language cannot be mixed in the same NC block.

● G commands cannot be used to switch between ISO dialect M and ISO dialect T

● Subprograms that are programmed in Siemens mode can be called.

● If Siemens functions are to be used, a switchover to Siemens mode must first be made.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.1 Function activation

PowerOn/Reset

The table below shows the possible combinations of MD10880

$MN_MM_EXTERN_CNC_SYSTEM and MD20150 $MC_GCODE_RESET_VALUE[46]. This

defines the Power On/Reset behavior.

Table 3-1

Function activation

After PowerOn/Reset

$MC_GCODE_RESET_VALUES[46]=

$MN_EXTERN_CNC_SYSTEM =

Siemens mode active, switching to ISO

1 G290 Siemens mode

1 ISO dialect M

dialect M possible

Siemens mode active, switching to ISO

1 G290 Siemens mode

2 ISO dialect T

dialect T possible

ISO dialect M active, switching to Sie-

2 G291 ISO dialect mode

1 ISO dialect M

mens mode possible

ISO dialect T active, switching to Sie-

2 G291 ISO dialect mode

2 ISO dialect T

mens mode possible

Data storage

Imported ISO programs are stored as main programs in the NC data storage under the default

address:

_N_WKS_DIR/_N_SHOPMILL_WPD.

The input can be changed by editing the DINO.INI file in the USER folder. More information can

be found in the following brochure:

3.1.1

Switching between the operating modes

G290/291

The following G functions can be used to switch between the Siemens mode and the ISO

dialect mode:

● G290 - Siemens NC programming language active

● G291 - ISO Dialect NC Programming language active

The active tool, tool compensation and work offsets are not influenced by the switchover.

G290 and G291 must be programmed alone in an NC block.

G65/66

Macro, non-modal and modal:

The programmed subprogram is called. A switch will only be made to Siemens mode if the

PROC instruction is used in the first line of the subprogram.

If such a program ends with M17 or RET, a mode switch is made back to ISO mode during the

return.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Siemens up call in ISO mode

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

N100 CALL "SHAFT"

N100 MCALL SHAFT

N100 SHAFT

Modal and non-modal subprogram calls with parameter transfer

N100 MCALL SHAFT ("ABC", 33.5)

N100 SHAFT ("ABC", 33.5)

Subprogram calls with path details

N100 CALL "/_N_SPF_DIR/SHAFT

N100 MCALL /_N_SPF_DIR/SHAFT

N100 PCALL /_N_SPF_DIR/SHAFT

During subprogram calls, Siemens mode is selected implicitly and a switch is made back to ISO

dialect mode at the end of the subprogram.

Modal, non-modal cycles

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

A switch is made to Siemens mode during this call.

3.2

G commands

The G codes of ISO dialect T and M relate to the G code system B.

The active G codes of ISO mode can be read using system variable $P_EXTGG[...]. The

numbers next to the G code specify the respective value in $P_EXTGG[...]. The 20154

EXTERN_GCODE_RESET_VALUES[n] 0, ..., 30 MD is used to define the G codes which are

effective in the power up if the NC channel isn't in Siemens mode.

Table 3-2

The default setting is marked as ¹⁾

ISO dialect T

ISO dialect M

Description

System A

System C

Group 1

G00 ¹⁾

Rapid traverse

G01

Linear motion

G01

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

ISO dialect T

ISO dialect M

Description

System A

System C

G02

Circle/helix in clockwise direction

G02

G02.2

Involute in clockwise direction

G03

Circle/helix in counter-clockwise direction

G03

G03.2

Involute in counter-clockwise direction

G33

Thread cutting with constant lead

G32

G33

G34

Thread cutting with variable lead

G34

G35

Convex thread in the clockwise direction

G35

G36

Convex thread in the counter-clockwise direction

G36

G77

Longitudinal turning cycle

G90

G20

G78

Thread cutting cycle

G92

G21

G79

Face turning cycle

G94

G24

Group 2

G17 ¹⁾

XY plane

G18

ZX plane

G19

YZ plane

G96

Constant cutting rate on

G96

G97 ¹⁾

Constant cutting rate off

G97

Group 3

G90 ¹⁾

Absolute programming

not

G90

G91

Incremental programming

not

G91

Group 4

G22

Working area limitation, protection zone 3 on

G23 ¹⁾

Working area limitation, protection zone 3 off

G68

Double slide/turret on

G68

G69 ¹⁾

Double slide/turret off

G69

Group 5

G23 ¹⁾

Inverse-time feedrate (rpm)

G94

G94 ¹⁾

Feedrate in [mm/min, inch/min]

G98

G94

G95 ¹⁾

G95

Revolutional feedrate in [mm/rev, inch/rev]

G99

G95

Group 6

G20 ¹⁾

G20 ¹⁾ (G70)

Inch input system

G20

G70

G21

G21 (G71)

Metric input system

G21

G71

Group 7

G40 ¹⁾

Deselection of cutter radius compensation

G40

G41

Compensation left of contour

G41

G42

Offset to right of contour

G42

Group 8

G43

Positive tool length compensation on

G43

G44

Negative tool length compensation on

G44

G49 ¹⁾

Tool length compensation off

G49

Group 9

G22

Working area limitation, protection zone 3 on

G22

G23 ¹⁾

Working area limitation, protection zone 3 off

G23

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

ISO dialect T

ISO dialect M

Description

System A

System C

G73

Deep-hole drilling cycle with chip breakage

G73

G74

Left tapping cycle

G74

G76

Precision drilling cycle

G76

G80 ¹⁾

Cycle off

G80

G81

Drilling cycle counterboring

G81

G82

Countersink drilling cycle

G82

G83

Deep-hole drilling cycle with chip removal

G83

G84

Right tapping cycle

G84

G85

Drilling cycle

G85

G86

Drilling cycle, retraction with G00

G86

G87

Reverse countersinking

G87

G89

Drilling cycle, retraction with machining feedrate

G89

Group 10

G80 ¹⁾

Drilling cycle off

G80

G83

Front face deep-hole drilling

G83

G84

Front face tapping

G84

G85

Front face drilling cycle

G85

G87

Side surface deep-hole drilling

G87

G88

Side surface tapping

G88

G89

Side surface drilling

G89

G98 ¹⁾

Return to starting point in fixed cycles

G98

G99

Return to point R in fixed cycles

G99

Group 11

G98 ¹⁾

Return to starting point in drilling cycles

G98

G99

Return to point R in drilling cycles

G99

G50 ¹⁾

Scaling off

G50

G51

Scaling on

G51

Group 12

G66

Macro module call

G66

G67 ¹⁾

Delete macro module call

G67

Group 13

G96

Constant cutting rate on

G96

G97 ¹⁾

Constant cutting rate off

G97

Group 14

G54 ¹⁾

Select work offset

G54

G55

Select work offset

G55

G56

Select work offset

G56

G57

Select work offset

G57

G58

Select work offset

G58

G59

Select work offset

G59

G54 P{1...48} 1

Extended work offsets

G54.1

Extended work offsets

G54.1

G54 P0

"External work offset"

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

ISO dialect T

ISO dialect M

Description

System A

System C

Group 15

G61

Exact stop modal

G61

G62

Automatic corner override

G62

G63

Tapping mode

G63

G64 ¹⁾

Continuous-path mode

G64

Group 16

G17

XY plane

G17

G18 ¹⁾

ZX plane

G18

G19

YZ plane

G19

G68

Rotation ON 2D 3D

G68

G69 ¹⁾

Rotation OFF

G69

Group 17

G15 ¹⁾

Polar coordinates off

G15

G16

Polar coordinates on

G16

Group 18 (non-modal effective)

G04

Dwell time in [s] or spindle revolutions

G04

G05

High-speed cycle cutting

G05

G05.1

High-speed cycle -> Call CYCLE305

G05.1

G07.1

Cylindrical interpolation

G07.1

G08

Feedforward control ON/OFF

G08

G09

Exact stop

G09

G10

Write work offset / tool offset

G10

G10.6

Rapid lifting ON/OFF (T)

G10.6

Retraction from contour (POLF) (M)

G11

End parameter entry

G11

G27

Referencing check (under development)

G27

G28

Approach 1st reference point

G28

G30

Apporach 2nd/3rd/4th reference point

G30

G30.1

Reference point position

G30.1

G31

Measuring with touch-trigger probe

G31

G52

Programmable work offset

G52

G53

Approach position in machine coordinate system

G53

G60

Directed positioning

G60

G65

Macro call

G65

G70

Finishing cycle

G70

G72

G71

Stock removal cycle, longitudinal axis

G71

G73

G72

Stock removal cycle, transverse axis

G72

G74

G72.1

Contour repetition with rotation

G72.1

G72.2

Linear contour repetition

G72.2

G73

Contour repetition

G73

G75

G74

Deep-hole boring and grooving in the longitudinal axis (Z)

G74

G76

G75

Deep-hole boring and grooving in the transverse axis (X)

G75

G77

G76

Multiple thread cutting cycle

G76

G78

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

ISO dialect T

ISO dialect M

Description

System A

System C

G92

Set actual value, spindle speed limitation

G50

G92

G92.1

Delete actual value, reset the WCS

G92.1

Group 20

G50.2 ¹⁾

Multi-edge turning OFF

G50.2

G50.2-

G51.2

Multi-edge turning ON

G51.2

-G51.2

Group 21

G13.1 ¹⁾

TRANSMIT OFF

G13.1

G12.1

TRANSMIT ON

G12.1

Group 22

G50.1

Mirroring on programmed axis OFF

G50.1

G51.1

Mirroring on programmed axis ON

G51.1

Group 25

G13.1

Polar coordinates interpolation OFF

G13.1

G12.1

Polar coordinates interpolation ON

G12.1

Group 31

G290 ¹⁾

Select Siemens mode

G290

G291

Select ISO dialect mode

G291

Modally effective G commands

Modally effective G commands which have an identical function in both systems (Siemens and

ISO dialect) are treated as follows:

When programming these G codes in one language, the corresponding G code for the other

language is determined and activated. The following G codes are affected by this:

Table 3-3

G codes have an identical function in Siemens mode and ISO dialect mode

G commands in Siemens mode

Corresponding G commands

ISO dialect T

ISO dialect M

Group 1: G00, G01, G02, G03, G33

Group 6: G17, G18, G19

Group 16: G17, G18, G19

Group 2: G17, G18, G19

Group 7: G40, G41, G42

Group 8: G54 to G554

Group 14: G54 to G59, G54 P1 to P48

Group 10: G60, G64

Group 18: G60, G64

Group 13: G700, G710

Group 6: G20, G21

Group 14: 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

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Note

If individual G commands from the groups stated in the table cannot be depicted, the basic

setting saved in MD20154 $MC_EXTERN_GCODE_RESET_VALUES and/or MD20152

$MC_GCODE_RESET_VALUES is activated.

Example: ISO mode

N5 G00 X100. Y100.

N10 G90

;activates G90 in ISO mode group 3

;in Siemens mode group 14

N15 G290

;switches over to Siemens, G90 is active

N20 G91

;activates G91 in ISO mode group 3

;in Siemens mode group 14

N25 G291

;switches over to ISO mode

N30 G291

;G91 is active

3.2.1

Display of the G code

The G code must always be displayed in the same language (Siemens or ISO Dialect) as the

relevant current block. If the display of the blocks is suppressed with DISPLOF, the current G

codes continue to be displayed in the same language as the active block.

Example

The G functions of the ISO dialect mode are used to call the Siemens standard cycles. To do

this, DISPLOF is programmed at the start of the relevant cycle; this way the G functions that are

programmed in the ISO dialect language continue to be displayed.

PROC CYCLE328 SAVE DISPLOF

N10

N99 RET

Procedure

The Siemens shell cycles are called via main programs. The Siemens mode is selected

automatically by calling the shell cycle.

With DISPLOF, the block display is frozen on calling the cycle; the G code continues to be

displayed in ISO mode.

The G codes that were changed in the shell cycle, are reset to their original status at the end

of the cycle with the "SAVE" attribute.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.2

Display of non-modal G codes

The external non-modal G codes (group 18) are no longer reset when changing block if these

G codes call subprograms. The G codes remain visible in the display until this subprogram is

exited.

However if a switch is made in the subprogram to the external language mode and if another

G code from group 18 is programmed, the previous value is overwritten and the new value

retained until the return.

Example:

Main program

Display group 18

N05 G00 X0 Y0 empty

N08 G27 X10 -> calls Cycle328

Empty

N09 M0

Empty

N40 M30

Empty

Cycle328 subprogram

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

3.2.3

G code output to PLC

The response of G group transfer to PLC is described in MD22515

$MC_GCODE_GROUPS_TO_PLC_MODE.

With the previous response, the G group is the array index of a 64-byte field (DBB 208 - DBB

271). At the most, the 64th G group can therefore be reached. Only the G groups of the

standard or external language can be displayed.

With the new response, data storage in the PLC is 8 bytes at most (DBB 208 - DBB 215) , i.e.

a total of 8 G groups can be output at most.

With this response, the array index of the following machine data is the same as the array index

of data storage in the PLC (DBB 208 - DBB215):

MD22515 $MC_GCODE_GROUPS_TO_PLC[ ] and/or

MD22512 $MC_EXTERN_GCODE_GROUPS_TO_PLC[ ]

The G code group from MD22515 $MC_GCODE_GROUPS_TO_PLC[ ] is output in DBB 208.

The benefit of this is that G codes of the Siemens and ISO mode can be output at the same time.

Since only the G code of one language can be output in a DBB2xx, each index (0 -7) may only

be set for one of the two machine data and 0 must be entered for the other MD. Faults are

reported with alarm 4045 " Channel %1 conflict between machine datum %2 and machine

datum %3".

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

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 available on the PLC:

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 incorrect 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 datum {S

$MC_GCODE_GROUPS_TO_PLC} and machine datum {S

$MC_EXTERN_GCODE_GROUPS_TO_PLC}

$MC_EXTERN_GCODE_GROUPS_TO_PLC[1]=0

$MC_EXTERN_GCODE_GROUPS_TO_PLC[2]=18

This process can now be used to display G codes of standard mode and ISO dialect mode at

the same time.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.4

Decoupling the frames between Siemens and ISO mode

Frames

In ISO mode, some G codes can be found in the programmable frame $P_FRAME, the

adjustable frame $P_UIFR and three basic frames $P_CHBFRAME[ ]. If a switch is made from

ISO mode to Siemens mode, these frames are not available to the Siemens language user. The

following are affected:

G52 programmable work offset -> progr. frame $P_PFRAME

G51 scaling -> progr. frame $P_BFRAME SCALE

G54-G59 work offset -> adjustable frame $P_UIFR

G54 P1..100 work offset -> adjustable frame $P_UIFR

G68 3D Rot -> basic frame $P_CHBFRAME[3]

G68 2D Rot -> basic frame $P_CHBFRAME[2]

G51.1 mirroring -> basic frame $P_CHBFRAME[1]

G92 set actual value -> basic frame $P_CHBFRAME[0]

G10 L2 P0 ext. work offset -> basic frame $P_CHBFRAME[0]

There are four new system frames, $P_ISO1FRAME to $P_ISO4FRAME for decoupling the

frames in question between Siemens and ISO mode. The frames are created with the 28082

$MC_MM_SYSTEM_FRAME_MASK machine data, bits 7 to 10. The reset behavior is set

using the 24006 $MC_CHSFRAME_RESET_MASK machine data, bits 7 to 10.

The following figure shows the G codes in ISO mode and the assignment of frames, when

system frames $P_ISO1FRAME to $P_ISO4FRAME, $P_SETFRAME and $P_EXTFRAME

are created.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3B,62 )5$0( * VFDOH

3B3)5$0( *

6HWWDEOH IUDPH *

3B8,)5 *

3B,62 )5$0( *

'5RW

3B,62 )5$0( *

'5RW '5RW

3B,62 )5$0( *

PLUURU DW SURJU D[LV

3B(;7)5$0( *

/ 3

H[W2IIVHW :2

3B6(7)5$0( * VHW DFWXDO YDOXH

Figure 3-1

Mapping of ISO functions on the ISO and Siemens frames

Note

If new frames are created, the ISO G codes write in these frames. If they are not created, the

frames are created as described in the previous section.

The section below shows which G codes describe which frames, how they are created and how

the frames' reset behavior must be set to ensure a compatible response to the ISO mode

original. The reset behavior may be set to deviate from the ISO mode original with the MD

described. This may be necessary when switching from ISO mode to Siemens mode.

G51 scaling

G51 X10 writes in

$P_ISO4FRAME

Component

TRANS, SCALE

Create

$MC_MM_SYSTEM_FRAME_MASK bit 10 = 1

Reset behavior

Delete frame

$MC_CHSFRAME_RESET_MASKBit 10 = 0

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

G52 programmable work offset

G52 X10 writes in

$P_PFRAME

Component

TRANS

Create

Is always present

Reset behavior

Is deleted at Reset

G54 - G59 P1...100 adjustable work offset

G52 - G59

$P_UIFER

Component

TRANS

Create

Is always present

Reset behavior

G54 is active after Reset

$MC_EXTERN_GCODE_RESET_VALUES[13] = 1

G68 3DRot

G68 X Y I J K R

$P_ISO3FRAME

Component

TRANS, SCALE

Create

$MC_MM_SYSTEM_FRAME_MASK bit 9 = 1

Reset behavior

Delete frame

$MC_CHSFRAME_RESET_MASKBit 9 = 0

G68 2DRot

G68 X Y R

$P_ISO2FRAME

Component

TRANS, SCALE

Create

$MC_MM_SYSTEM_FRAME_MASK bit 8 = 1

Reset behavior

Delete frame

$MC_CHSFRAME_RESET_MASKBit 8 = 0

G51.1 mirroring

G51.1 X Y

$P_ISO1FRAME

Component

TRANS, MIRROR

Create

$MC_MM_SYSTEM_FRAME_MASK bit 7 = 1

Reset behavior

Delete frame

$MC_CHSFRAME_RESET_MASKBit 7 = 0

G92 set actual value

G92 X Y R

$P_SETFRAME

Component

TRANS

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Create

$MC_MM_SYSTEM_FRAME_MASK bit 0 = 1

Reset behavior

Frame is retained after Reset

$MC_CHSFRAME_RESET_MASKBit 0 = 1

G10 L2 P0

$P_EXTFRAME

Component

TRANS

Create

$MC_MM_SYSTEM_FRAME_MASK bit 1 = 1

Reset behavior

Delete frame

$MC_CHSFRAME_RESET_MASKBit 1 = 0

If all frames are created, the frames with FINE components no longer have to be configured for

ISO mode. The MD18600 $MN_MM_FRAME_FINE_TRANS does not have to be set to 1. If a

switch is made from ISO mode to Siemens mode and a function used there which requires a

fine offset (e.g. G58, G59), $MN_MM_FRAME_FINE_TRANS = 1 must always be true.

G54.1

G54.1 Pxx is an alternative way of writing G54 Pxx. The functionality is identical. The P address

must always be programmed in the block for G54.1. If P is not programmed, alarm 12080

(syntax fault) is output.

Display of extended work offset G54 Pxx

In the past when working in ISO dialect T, G54.1 P.. could not be programmed. G code group

14 in ISO dialect T has now had G code G54.1 added to it and G54.1 is now displayed for the

programmed P by default.

When programming G54 Pxx or G54.1 Pxx, to date when working in ISO dialect M, G code

display G54.1 was used.

MD20734 $MC_EXTERN_FUNCTION_MASK bit 11 can now be used to activate the system

such that the programmed P is also displayed after the dot in the G code display.

Programmed

Bit 11 = 1

Bit 11 = 0

G54 P1

Display G54P1

G54.1

G54 P28

Display G54P28

G54.1

G54.1 P28

Display G54P28

G54.1

G54 P48

Display G54P48

G54.1

G54.1 P48

Display G54P48

G54.1

3.2.5

Writing work offset with G10

G10 can be used to write out the work offsets from the part program.

G10 L2 P1...P6 X.. Y..

;G54.. G59

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

G10 L20 P1...P100

;additional adjustable NV

G10 L2 P0

;external extOffset NV

These work offsets are mapped on the same frames as the work offsets which already exist for

ISO dialect M.

The G10 command is extended for ISO dialect T:

Writing system data

G10 Pxx X Y Z ;writing tool compensation data

Depending on the MD20734 $MC_EXTERN_FUNCTION_MASK, bit 1, G10 Pxx is used to

write tool geometry or tool wear.

$MC_EXTERN_FUNCTION_MASK, bit 1 = 0:

P > 100 writing geometry values

P < 100 writing wear values

$MC_EXTERN_FUNCTION_MASK, bit 1 = 1:

P > 10000 writing geometry values

P < 10000 writing wear values

See also

Decoupling the frames between Siemens and ISO mode (Page 25)

3.2.14

Double slide or double turret processing G68/G69

Function

The G68/G69 function can be used to control the processing of rotating parts on both sides.

Both processing with a double slide in two channels and processing in one channel with two

tools which are permanently linked to one another at a distance x.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

MD10812 $MN_EXTERN_DOUBLE_TURRET_ON is used to define whether processing in the

two channels is synchronized (= FALSE) or whether the two permanently linked tools are used

in turn for processing (= TRUE).

When using permanently linked tools, G68 is used to activate distance x entered in setting data

42162 $SC_EXTERN_DOUBLE_TURRET_DIST as an additive work offset in the X axis.

Because the second tool processes the opposite side of the rotating part, G68 is also used to

activate mirroring around the Z axis (X axis direction change). The work offset and mirroring for

the 2nd tool are activated with the next block with axial motion.

G69 is used to reverse the work offset and processing continues with the 1st tool.

G68 and G69 must be programmed in a block on their own.

During tool length compensation in the X axis for the second tool, the correction sign must be

taken into account. The sign must be entered as if the X axis were not mirrored. Alternatively

the setting data 42900 $SC_MIRROR_TOOL_LENGTH (mirror tool length compensation) and

42190 $SC_MIRROR_TOOL_WEAR (mirror wear values of tool length compensation) must be

set.

MD10610 $MN_MIRROR_REF_AX must either be 0 or 1. The X or 1st axis is then always

mirrored.

If G68 is programmed and G68 is already active, the G function is skipped. The same applies

to G69.

Double turret head: $MN_EXTERN_DOUBLE_TURRET_ON = TRUE

The example below shows processing with two permanently linked tools. Machine data

$MN_EXTERN_DOUBLE_TURRET_ON = TRUE must be set for the function to be effective.

If the setting data 42162 $SC_EXTERN_DOUBLE_TURRET_DIST = 0, alarm 12728 "Distance

for double turret not set" is output.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

;

7RRO RIIVHW

7RRO 7

7RRO RIIVHW

7RRO 7

Figure 3-4

Processing with two permanently linked tools

Example:

N100 X40. Z180. G1 F1 G95 S1000 M3 T1

N110 G68

;Activate mirroring around Z and additive work offset

(220 mm)

N120 X80. Z120. T2

N130 G69

;Deactivate mirroring and additive work offset

N140 X120. Z60 T1

Double slide processing: $MN_EXTERN_DOUBLE_TURRET_ON = FALSE

If MD10812 $MN_EXTERN_DOUBLE_TURRET_ON = FALSE, G68 undertakes channel

synchronization. If G68 is programmed in a channel, processing is stopped until G68 is

detected in the second channel. This function can be used to synchronize the 1st and 2nd

channel. No more synchronization is undertaken. For the two tools to act in a synchronous

manner in subsequent processing, the programmed movements and feeds must be the same

in the two channels.

Wait mark 1 is used for G68 and wait mark 2 is used for G69 to synchronize the first two

channels. The first two M functions must not therefore be used at the same time for channel

synchronization in the same part program (see chap. "Program coordination between two

channels and M commands").

G68 only takes effect in the first two channels. If G68 is programmed in another channel and if

MD10812 $MN_EXTERN_DOUBLE_TURRET_ON = FALSE, G68 is skipped.

The function is used for producing thin rotating parts. The two tools should therefore perform

the same movement on the respective opposite side of the rotating part, mirrored around the

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Z axis. The same traversing and feeds must be programmed in the two channels for this to take

place.

Example of synchronous processing with two channels:

;

7RRO FKDQQHO

Figure 3-5

Synchronous processing with two channels

Example:

Channel 1:

N10 ...

- " -

N1000 G68

;Start synchronization

N1010 G01 X30 Z120 G95 F1.2 S1000 M3

N1020 X15 Z80

N1030 Z65

N1040 Z25 X40

N1050 G69

;Synchronization off

Channel 2:

N10 ...

- " -

N2000 G68

;Start synchronization

N2010 X30 Z120 G01 G95 F1.2 S1000 M3

N2020 X15 Z80

N2030 Z65

N2040 X40 Z25

N2050 G69

;Synchronization off

In ISO dialect original, channel synchronization is also undertaken when G68 is active.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.15

Polar coordinates G15/G16 (ISO dialect M)

Programming

When in ISO dialect mode, NC program parts in which polar programming is undertaken are

started using start command G16. Until the end command G15 is issued, the coordinates of the

end points are interpreted as radius and angle polar coordinate values in the current plane.

The first of the plane's axes is interpreted as a pole radius and the second axis as a pole angle,

i.e. for G17, X is the radius and Y the angle.

After G16, in each block up to G15 the pole is reset and the pole is reset at G17:

● G90 X: The pole lies at the workpiece zero

● G91 X: The pole lies at the current position

● No X in block: The pole lies at the workpiece zero

Example:

N5 G17 G90 X0 Y0 F5000

N10 G16 X50 Y90

;Polar coordinates ON

;the pole is the workpiece zero

;Position X=0 and Y=50 in the Cartesian coordinate system

N20 G90 Y0

;No X in the block

;Pole angle =0, radius= of the last programmed PolarRa-

dius=50

;Position X=50 and Y=0

N30 Y36.87

;The pole is at the workpiece zero

;Pole angle =36.87, radius=50

;Position X=40 and Y=30

G15

The pole radius is always taken as absolute value, while the pole angle can be interpreted as

absolute value as well as incremental value.

Programmed angle

When polar coordinates programming is active, the programmed angle can be read via system

variable $P_AP.

This variable is used in the shell cycle. Before the pole is reset, the angle must be saved during

incremental programming because the angle is deleted.

Pole programing is ended with G15. The pole radius is set to 0.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.16

Interpolation of polar coordinates G12.1/G13.1 (G112/G113)

Function

With G12.1 and G13.1 an interpolation is activated and deactivated in the machining plane

between a rotary axis and a linear axis. A further linear axis may be present perpendicular to

this plane. This function corresponds to the TRANSMIT function in the Siemens mode. In

Siemens mode, two TRANSMIT transformations may be parameterized. The 1st TRANSMIT

data block which must correspond to the 2nd transformation data block is always used for

G12.1.

Additional information on the TRANSMIT function is provided in the Transformations Function

Manual.

Example

5RWDU\ D[LV &

; D[LV

= D[LV

Figure 3-6

Example of the interpolation of polar coordinates

N010 T0101

N20 G94

N30 G90

N40 G291

N100 G00 X60. C0. Z50.

N200 G12.1

N201 G42 G01 X20. F1000.

N202 Y10.

N203 G03 X10. Y20. R14.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

N204 G01 X-20.

N205 Y-10.

N206 G03 X-10.0 Y-20.0 R14.

N207 G01 X20.

N208 Y0

N209 G40 X60.

N210 G13.1

N300 G00 Z50

N180 M30

Note

No geo axis interchange (parallel axes with G17 (G18, G19)) should be active.

3.2.17

Cylindrical interpolation G07.1 (G107)

Function

Randomly running grooves can be cut on cylindrical workpieces with function G07.1 (cylindrical

interpolation). The path of the grooves is programmed with reference to the unwrapped, level

surface of the cylinder. The cylindrical interpolation is started with G07.1 with the specification

of the cylinder radius (G07.1 C<cylinder radius>) and ended with G07.1 C0 (radius = 0).

Note

The function is mapped internally on the TRACYL Siemens functionality. In ISO dialect mode,

the 1st TRACYL transformation and the 1st transformation data block are always activated with

G07.1. The 2nd TRACYL function cannot be activated in ISO dialect mode. A detailed

description and parameterization of the 1st TRACYL function can be found in the following

documentation:

Description of functions for extended functions, chapter M1 and

Programming Manual for preparing for work, chapter 7 "Transformations".

Constraints

For Siemens the rotary axis must be defined for cylindrical interpolation in machine data.

With ISO dialect, the rotary axis is defined for cylindrical interpolation with G07.1 programming

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

N120 G01 C360.0

N130 G40 Z100.0

N140 G07.1 C0

;deselect cylindrical interpolation

N150 M30 ;

Example of programming in Siemens mode: The Y axis is assigned to the rotary axis as a linear

axis.

%0001

N05 G00 G90 Z100 C0

N10 G01 G91 G18 Z0 C0;

N20 TRACYL(114.598)

;select cylindrical interpolation with radius

57.299 mm

N30 G90 G01 G42 Z120 D01 F250

N40 Y30

N50 G02 Z90 Y60 RND=30

N60 G01 Z70

N70 G03 Z60.0 Y70 RND=10

N80 G01 Y150

N90 G03 Z70 Y190 RND=75

N100 G01 Z110 Y230

N110 G02 Z120 Y270 RND=75

N120 G01 Y360

N130 G40 Z100

N140 TRAFOOF

;deselect cylindrical interpolation

N150 M30 ;

3.2.18

Interrupt program with M96/M97 (ASUB)

M96

A subprogram can be defined as an interrupt routine with the M96 P<Program No.>.

The start of this program is triggered by an external signal. To start the interrupt routine, the 1st

rapid NC input is used from among the eight inputs available in the Siemens mode. Another

rapid input (1 to 8) can also be selected with MD10818

$MN_EXTERN_INTERRUPT_NUM_ASUP.

The function is mapped on the Siemens syntax SETINT(x) <CYCLE396> [PRIO=1].

The interrupt program programmed with Pxxxx is called in shell cycle CYCLE396 in ISO mode.

The program number can be found in $C_PI. At the end of the shell cycle, MD10808

$MN_EXTERN_INTERRUPT_BITS_M96, bit 1 is evaluated and either positioned on the

interruption point with REPOS or continued with the next block. The value programmed with "P"

can be found in the new cycle variable $C_PI without a leading zero. This must be increased

to four digits in the shell cycle before the subprogram is called.

Example:

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

N0020 M96 P5

Call in shell cycle

progName = "000" << $C_PI

ISOCALLprogName

See also how to handle 8-digit program numbers if MD20734

$MC_EXTERN_FUNCTION_MASK, bit 6 is set.

End of interruption (M97)

The interrupt program is deactivated with M97. Only after the next activation with M96 can the

interrupt routine be started with the external signal.

This corresponds to the Siemens syntax ENABLE(x).

x = Content of MD10818 $MN_EXTERN_INTERRUPT_NUM_ASUP

If the interrupt program programmed with M96 Pxx is to be called directly with the interrupt

signal (without intermediate step with CYCLE396), then machine data 20734

$MC_EXTERN_FUNCTION_MASK, bit 10 must be set. The subprogram programmed with

Pxx is then called in Siemens mode during a signal change from 0 -> 1.

The M function numbers for the interrupt function are set through machine data. MD10804

$MN_EXTERN_M_NO_SET_INT is used to determine the M number for activating an interrupt

routine, MD10806 $MN_EXTERN_M_NO_DISABLE_INT is used to determine the M number

for suppressing an interrupt routine.

Only M functions which are not standard M functions may be set. The default of the M functions

is M96 and M97. To activate the function, bit 0 must be set in MD10808

$MN_EXTERN_INTERRUPT_BITS_M96. The M functions are not output to the PLC. The M

functions are interpreted as normal auxiliary functions if bit 0 is not set.

At the end of the "interrupt" program, one normally traverses to the end position of the part

program block following the interruption block. If the part program is to be processed further

from the interruption point, there must be a REPOS instruction at the end of the "interrupt"

program, e.g. REPOSA. For this, the interrupt program must be written in the Siemens mode.

The M functions for activating and deactivating an interrupt program must be present alone in

the block. The system issues alarm 12080 "Channel %1 block %2 syntax error for text %3" if

addresses other than "M" and "P" are programmed in the block.

Information about machining cycles

In ISO dialect original you can set whether a machining cycle is to be interrupted immediately

or only at the end using an interrupt routine. To do this, the shell cycles must evaluate MD10808

$MN_INTERRUPT_BITS_M96 bit 3. If bit=1, the interrupt must be locked at the start of the

cycle with DISABLE(1) and activated again at the end of the cycle with ENABLE(1) so that the

machining cycle is not interrupted.

Because the interrupt program is only started during edge change 0/1, the interrupt input must

be monitored in the event of a locked interrupt during the cycle runtime with a synchronized

action in the shell cycle. If the interrupt signal in the cycle is changed from 0 to 1, the interrupt

signal must be set again following ENABLE(1) at the end of the shell cycle so that the interrupt

program is then started. To be able to write the interrupt input in the shell cycle, MD10361

$MN_FASTIO_DIG_SHORT_CIRCUIT[1] must be parameterized.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Machine data

The response of the interrupt program function can be determined from the following machine

data:

MD10808 $MN_EXTERN_INTERRUPT_BITS_M96:

Bit 0 = 0

Interrupt program is not possible as M96/M97 are normal M functions.

Bit 0 = 1

Activation of an interrupt program with M96/M97 is allowed.

Bit 1= 0

The part program is further processed with the end position of the next block following the

interrupt block (REPOSL RMEBL).

Bit 1= 1

Continue processing part program from interrupt position.

(Evaluation in interrupt program (ASUB), return with/without REPOSL)

Bit 2 = 0

The interrupt signal interrupts the current block immediately and starts the interrupt routine.

Bit 2 = 1: The interrupt routine is started only at the end of the block.

Bit 3 = 0

The machining cycle is interrupted immediately after an interrupt signal arrives.

Bit 3 = 1

The interrupt program is started only at the end of the machining cycle

(evaluation in the shell cycles)

Bit 3 must be evaluated in the shell cycles and the cycle process must be adapted accordingly.

Bit 1 must be evaluated in the interrupt program.

If Bit 1 = TRUE, REPOSL RMIBL must be used for positioning on the interruption point at the

end of the program, otherwise REPOSL RMEBL must be used for positioning on the block end

position.

Example:

N1000 M96 P1234

;Activate ASUB 1234.spf. In the case of a rising edge of

;the first high-speed input,

;the 1234.spf program is started.

N3000 M97

;Deactivation of ASUB

Before the call of the interrupt program no rapid lift (LIFTFAST) is performed. With the

increasing edge of the interrupt signal, depending on MD10808

$MN_EXTERN_INTERRUPT_BITS_M96, the interrupt program is started immediately.

Siemens constraints

The interrupt routine is treated as a normal subprogram. In other words, to be able to execute

interrupt routines, at least one subprogram level must be free. (For Siemens there are 12

program levels, for ISO dialect there are 5.)

The interrupt routine is started only during an edge change of the interrupt signal from 0 to 1.

If the interrupt signal remains permanently on 1, then the interrupt program is not restarted any

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

ISO dialect constraints

A program level is reserved for the interrupt routine such that all permissible program levels

may be filled before the interrupt program is called.

Depending on the machine data, the interrupt program is also started when there is a static

signal.

3.2.19

Comments

In ISO dialect mode, round brackets are interpreted as comment signs. In Siemens mode, ";"

is interpreted as a comment. To simplify matters, a ";" is also understood as a comment in ISO

dialect mode.

If the comment start sign '(' is used inside a comment again, the comment is ended only if all the

open brackets are closed again.

Example:

N5 (comment) X100 Y100

N10 (comment(comment)) X100 Y100

N15 (comment(comment) X100) Y100

In blocks N5 and N10, X100 Y100 is executed, in block N15 only Y100 because the first

bracket is closed only after X100. Everything up to that point is interpreted as a comment.

3.2.20

Skip block

The sign for skipping or suppression of blocks "/" can be used at any convenient position in a

block, i.e. even in the middle of the block. If the programmed block skip plane is active on the

date of the compilation, the block is not compiled from this point up to the end of the block. An

active block skip plane has the same effect as a block end.

Example:

N5 G00 X100. /3 YY100 --> Alarm 12080,

N5 G00 X100. /3 YY100 --> no alarm, if block skip plane 3 is active

Block skip signs within a comment are not interpreted as block skip signs

Example:

N5 G00 X100. ( /3 Part1 ) Y100

;the Y axis is traversed even when the

block skip plane 3 is active

The block skip planes /1 to /9 can be active. Block skip values <1 >9 lead to alarm 14060

"Channel %1 block %2 Impermissible skip plane for differential block skip".

The function is mapped to the existing Siemens skip planes. Unlike ISO Dialect original, / and /

1 are separate skip planes that must also be activated separately.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.21

Auxiliary function output

M functions

ISO dialect mode

M functions are output to the PLC as auxiliary functions. The only exceptions are M98 and M99.

Predefined M functions are:

M17, M40, M41, M42, M43, M44, M45, M70, M96, M97, M98, M99.

Spindle axis switchover with M29

In ISO dialect mode, the spindle is switched to axis mode with M29. The M function number may

however also be set differently using machine datum.

MD20095 $MC_EXTERN_RIGID_TAPPING_M_NR is used to pre-set the M function number.

The machine datum is only effective in external language mode and is preset with M29. Only

the M function numbers that are not used as standard M functions can be assigned. For

example, the M function numbers M0-M5, M30, M98, M99 are not allowed.

The same function is executed in Siemens mode with M70.

MD20094 $MC_SPIND_RIGID_TAPPING_M_NR) is used to pre-set the M function number.

The machine datum is only effective in Siemens mode and is preset with M70. An M function

other than M70 can therefore also be set in Siemens mode for the spindle changeover. The

machine datum may only be assigned M function numbers that are not used as standard M

functions. M0 to M5, M17, M19, M30, M40 to M45 are not permitted.

H functions

All H functions are output to the PLC in ISO dialect M as auxiliary functions. With ISO dialect T

G Code System A, H is the incremental path of the 4th axis - only if a 4th axis is present.

T functions

T functions are output to the PLC as auxiliary functions. T also means tool selection.

D functions

The D function is output to the PLC as an auxiliary function. With ISO dialect M, the tool length

compensation is activated under address D.

B functions

If B is not an axis, the B function is output to the PLC as auxiliary function H with address

extension H1=.

Example: B1234 is output as H1 = 1234.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.22

Approach 1st home position with intermediate point (G28)

The CYCLE328 cycle is called automatically when reading the ISO dialect command "G28

<axis>". The intermediate position (incremental or absolute) via which the home position is to

be approached is stated under <Axis>. The intermediate position and reference position are

approached in positioning mode.

The cycle only applies for the axes available with ISO dialect:

● ISO dialect M: X, Y, Z (A, B, C, U, V, W)

● ISO dialect T: X, Z, Y (C)

The cycle is always run with radius programming (DIAMOF). Active G commands become

effective again once the cycle is complete and before the cycle is called.

Various machine data must be set before the 1st home position is approached, see

"Commissioning" chap.

3.2.23

Switching precontrol on/off with G08 P..

Function

The feedforward control reduces the velocity-dependent overtravel when contouring towards

zero. Traversing with feedforward control permits higher path accuracy and thus improved

machining results.

Note

The type of feedforward control and which path axes are to be traversed with feedforward

control is specified via machine data.

Default: Velocity-dependent feedforward control

Option: Acceleration-dependent feedforward control

Example

N0010 G08 P1

; Switch on feedforward control

N0020 G1 X10 Y50 F900

N0030 G1 X20 Y70

N1000 G08 P0

; Switch off feedforward control

If G08 is programmed without "P", alarm 12470 "Channel %1 block %2 G function %3 is

unknown" is output.

In order to use G08 P1 to flexibly activate other functions such as SOFT, BRISK etc., G08 P..

is used to call cycle CYCLE308.spf.

G08 P1 alone must remain in the block.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

3.2.24

Compressor in ISO dialect mode

The commands COMPON, COMPCURV, COMPCAD are commands of the Siemens

language and they activate a compressor function that combines several linear blocks into one

machining section. If this function is activated in Siemens mode, even linear blocks can then be

compressed in ISO mode with this function.

The blocks can at the most consist of the following commands:

● Block number

● G01, modal or in block

● Axis assignments

● Feedrate

● Comments

If a block contains other commands (e.g., auxiliary functions, other G codes, etc.), then

compression does not take place.

Value assignments with $x for G, axes and feedrate are possible, as is the skip function.

Example: These blocks are compressed:

N5 G290

N10 COMPON

N15 G291

N20 G01 X100. Y100. F1000

N25 X100 Y100 F$3

N30 X$3 /1 Y100

N35 X100 (Axis 1)

These blocks are not compressed:

N5 G290

N10 COMPON

N20 G291

N25 G01 X100 G17

;G17

N30 X100 M22

; Auxiliary function in block

N35 X100 S200

;Spindle speed in block

3.2.25

Automatic corner override G62

An inner corner with active tool radius compensation is often meaningful to reduce the feedrate.

G62 operates only on inner corners with active tool radius compensation and active continuous-

path mode. Only the corners whose inner angle is smaller than SD42526

$SC_CORNER_SLOWDOWN_CRIT are taken into account. The inner angle is defined from

the bend in the contour.

The feedrate is reduced by the factor SD42524 $SC_CORNER_SLOWDOWN_OVR:

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

Traversed feedrate =

F * $SC_CORNER_SLOWDOWN_OVR * feedrate override.

The feedrate override is made up of the feedrate override of the Machine Control Panel

multiplied by the override from synchronized actions.

The reduction in feedrate is begun at a distance of SD42520

$SC_CORNER_SLOWDOWN_START before the corner. It ends at distance SD42522

$SC_CORNER_SLOWDOWN_END after the corner (see following figure). An appropriate

path is used for curved contours.

;

:RUNSLHFH

&RDWLQJ WR EH PLOOHG RII

7RRO FHQWHU SRLQW SDWK

6&B&251(5B6/2:'2:1B67$57

6&B&251(5B6/2:'2:1B(1'

,QWHUQDO DQJOH ื

6&B&251(5B6/2:'2:1B&5,7

)HHGUDWH VORZGRZQ DW FRUQHU

3DWK YHORFLW\ Y

)

6&B&251(5B6/2:'2:1B295

6&B&251(5B6/2:'2:1B67$57

3DWK V

6&B&251(5B6/2:'2:1B(1'

Figure 3-8

Parameter assignment of feedrate reduction G62 with the example of a 90 degree corner

Parameter assignment

The override value is set using the following setting data:

SD42520 $SC_CORNER_SLOWDOWN_START

SD42522 $SC_CORNER_SLOWDOWN_END

SD42524 $SC_CORNER_SLOWDOWN_OVR

SD42526 $SC_CORNER_SLOWDOWN_CRIT

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.2 G commands

The setting data is preassigned with the value 0.

● If $SC_CORNER_SLOWDOWN_CRIT = 0, the corner deceleration is effective only at the

reversal points.

● If $SC_CORNER_SLOWDOWN_START and $SC_CORNER_SLOWDOWN_END are

equal to 0, then the feedrate reduction is approached with the permissible dynamic

response.

● If $SC_CORNER_SLOWDOWN_OVR = 0, then a transient stop is inserted.

● $SC_CORNER_SLOWDOWN_CRIT is related to the geometry axes in G62. It defines the

maximum inner angle in the current machining plane up to which the corner deceleration is

used. G62 is not effective in rapid traverse.

Activating

The function is activated via G62 and/or G621. The G code is active either via the

corresponding part program command or through MD 20150

$MC_GCODE_RESET_VALUES[56].

Examples

$TC_DP1[1,1]=120

$TC_DP3[1,1]=0.

;Tool length compensation

$TC_DP4[1,1]=0.

$TC_DP5[1,1]=0.

N1000 G0 X0 Y0 Z0 F5000 G64 SOFT

N1010 STOPRE

N1020 $SC_CORNER_SLOWDOWN_START = 5.

N1030 $SC_CORNER_SLOWDOWN_END = 8.

N1040 $SC_CORNER_SLOWDOWN_OVR = 20.

N1050 $SC_CORNER_SLOWDOWN_CRIT = 100.

N2010 X00 Y30 G90 T1 D1 G64

N2020 X40 Y0 G62 G41

;Inner corner of N2030,

;but TRC still selected

N2030 X80 Y30

;Inner corner of N2040 127 degrees

N2040 Y70

;Inner corner of N2050 53 degrees

N2050 X40 Y40

;Outer corner of N2060

N2060 X20 Y70

; Inner corner of N2070 97 degrees

N2070 Y60

; Inner corner of N2080 90 degrees

N2080 X20 Y20

; Outer corner of N2090,

;irrelevant due to TRC deselection

N2090 X00 Y00 G40 FENDNORM

M30

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.3 Substitution by a substitution cycle with a tool selection block

3.3

Substitution by a substitution cycle with a tool selection block

3.3.1

Milling

Note

The following generally applies to all substitution cycles in which the programmed values are

transferred in $C_ variables:

The $C_ system variables must be copied at the start of the cycle into R parameters, local and

global user data. The cycle then only works with the copies.

Substitution by an M macro

MD10814: $MN_EXTERN_M_NO_MAC_CYCLE[0] = 6

MD10815: $MN_EXTERN_M_NO_MAC_CYCLE_NAME[0] = "L6"

Nothing from this block is executed, all programmed parameters are copied into $C_ system

variables.

In the cycle, T, H, D and M must be programmed and all other addresses programmed in the

block written indirectly.

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

N5 T10 H22 M6 or N5 T10 D33 M6 ; M6 calls L6

N100 PROC L6( )

N105

N110 $C_MACPAR[1]=$C_T

N115 $C_MACPAR[2]=$C_H

N120 $C_MACPAR[3]=$C_D

N125 G291

N130 T$1 H$2 M206 or N130 T$1 D$2 M206

N135 G290

N140 RET

T can also be programmed in Siemens mode with T=$C_T.

Substitution by an M function

MD10715: $MN_M_FCT_CYCLE[0] = 6

MD10716: $MN_M_FCT_CYCLE_NAME[0] = "L6"

MD10718: $MN_M_NO_FCT_CYCLE_PAR = 0

MD10719: $MN_T_NO_FCT_CYCLE_MODE

MD10718 is used to parameterize whether the cycle call takes place when the parameters are

transferred. MD10719 is used to set the call time at the start or end of the block.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.3 Substitution by a substitution cycle with a tool selection block

If just N5 T M6 and not H D is programmed in the part program block, the cycle can be called

without the transfer of parameters. The block is executed and the cycle called without the

transfer of parameters at the end of the block.

Only the M function has to be programmed in the cycle to activate the tool.

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

MD10715: $MN_M_FCT_CYCLE[0] = 6

MD10716: $MN_M_FCT_CYCLE_NAME[0] = "L6"

MD10718: $MN_M_NO_FCT_CYCLE_PAR = -1

N5 T10 M6 ; M6 calls L6

N100 PROC L6( )

…

N110 m206

N115 RET

If N5 T H M6 or N5 T D M6 is programmed in the part program block, the cycle must be called

with the transfer of parameters. T H D and the M function then have to be programmed in the

cycle to activate the tool. H and D must be programmed after the T and M function to activate

the tool.

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

MD10715: $MN_M_FCT_CYCLE[0] = 6

MD10716: $MN_M_FCT_CYCLE_NAME[0] = "L6"

MD10718: $MN_M_NO_FCT_CYCLE_PAR = 0

N5 T10 H22 D23 M6 ; M6 calls L6

N100 PROC L6( )

N105 IF $C_T_PROG == 1

N110 $C_MACPAR[1]=$C_T

N115 G291

N120 T$1 M206

N125 G290

N110; programming of H and D

; indirectly via $C_MACPAR as in blocks N110 and N120

M115 M17

Substitution by T programming

MD10717: $MN_T_FCT_CYCLE_NAME="L6"

$MN_T_NO_FCT_MODE

MD10719: $MN_T_NO_FCT_CYCLE_MODE

Nothing from this block is executed, all programmed values are written into $C_ system

variables. The call time is determined with $MN_T_NO_FCT_MODE. T and M must be

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.3 Substitution by a substitution cycle with a tool selection block

programmed in the cycle. If H or D are programmed in addition to T in the call block, H and D

must be programmed in the cycle after the T and M function to activate the tool.

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

N5 T10; T calls L6.spf

N100 PROC L6( )

N105 T=$C_T M206

or in ISO mode indirectly via T$1

N110 $C_MACPAR[1]=$C_T

N120 G291

N125 T$1 M206

N125 G290

3.3.2

Turning

Substitution by an M macro

MD10814: $MN_EXTERN_M_NO_MAC_CYCLE[0] = 6

MD10815: $MN_EXTERN_M_NO_MAC_CYCLE_NAME[0] = "L6"

Nothing from this block is executed, all programmed parameters are written into $C_ system

variables.

T must be programmed in the cycle. The programmed T contains the tool number and the

correction number. The programmed value is transferred in $C_T. T1234 results in $C_T =

1234; $C_T_PROG = 1.

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

N5 T1022 M6 ; M6 calls L6

N100 PROC L6( )

N101 IF $C_T == TRUE

N110 $C_MACPAR[1]=$C_T

N120 G291

N125 T$1 M206

N130 G290

N135 ENDIF

N140 M17

Substitution by an M function

MD10715: $MN_M_FCT_CYCLE[0] = 6

MD10716: $MN_M_FCT_CYCLE_NAME[0] = "L6"

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.3 Substitution by a substitution cycle with a tool selection block

The block is executed and the cycle called without the transfer of parameters at the end of the

block.

The M function is programmed in the cycle at the end to activate the tool (if present).

Example:

MD22550: $MC_TOOL_CHANGE_MODE = 1

MD22560: $MC_TOOL_CHANGE_M_CODE = 206

N5 T1234 M6 ;M6 calls L6

PROC L6( )

…

M206

M17

Substitution by T programming

MD10717: $MN_T_FCT_CYCLE_NAME="L6"

Nothing from the block is executed, all programmed values are written into $C_ system

variables.

The call time is determined with $MN_T_NO_FCT_CYCLE_MODE. T and M must be

programmed in the cycle. The programmed T value contains the tool number and tool

compensation number.

The split T value and the tool number in $C_T and the programmed tool number in $C_H are

transferred to the cycle according to MN_EXTERN_DIGITS_TOOL_NO or

MN_EXTER_DIGITS_OFFSET_NO.

The unsplit programmed T value is also transferred in $C_T_VALUE.

Example:

Tool

Cutting edge

H number

T10

T31

MN_EXTER_DIGITS_OFFSET_NO = 2

N5 T3104 ; tool 31 $C_T == 31

; H number 4$C_H == 4

; $C_T_VALUE == 3104

T is programmed indirectly in the cycle with $C_T_WORD.

Example:

N5 T3104 ; T calls L6.spf

PROC L6( ) ; T indirectly in ISO mode

N100

N102 $C_MACPAR[1] = $C_T_VALUE

N105 G291

N110 T$1

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N115 G290

N120 M17

3.3.3

Indirect programming in ISO mode using $ variables

What are known as $ variables exist in order to perform indirect programming in ISO mode.

Values are assigned in ISO mode via these $ variables, for example T$1. In total there are 30

$ variables, $1 to $30.

The $ variables are written in Siemens mode using $C_MACPAR[0] - [30]. When programming

in ISO mode, the value is read from the corresponding $C_MACPAR[ ] variable and assigned

to the address. The integer value following $ corresponds to the index for $C_MACPAR[ ].

Example:

N5 G290

N10 $C_MACPAR[5] = 12

N15 G291

N20 T$5

The value from $C_MACPAR[5] is assigned to address T. This corresponds to T12 in ISO

mode.

Several $ assignments can be located in the same block.

N5 G290

N10 $C_MACPAR[1] = 1000 $C_MACPAR[2] = 85 $C_MACPAR[3] = 93.2

N15 G29

N20 F$1 X$2 Y$3

This corresponds to F1000 X85 Y93.2

Numerous calculations can therefore be undertaken in Siemens mode and the results then

assigned to addresses in ISO mode.

Note

Pure calculations in ISO mode e.g.: N5 $1=$2+1200 are not possible.

3.4

Subprogram and macro technology

3.4.1

Subprogram technique: M98

Subprogram call

In ISO dialect, subprogram calls with M98 are programmed.

For the program syntax, see the figure below:

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

3 [[[[\\\\

3URJUDP QR PD[ GLJLWV

1R RI UHSHWLWLRQV PD[ GLJLWV

Figure 3-9

Description of permissible parameters

Program syntax M98 Pxxxxyyyy is used to call a subprogram with the number yyyy and repeat

it xxxx times. If xxxx is not programmed, the subprogram is only executed once. The

subprogram name always comprises four digits or is extended by adding 0s until there are four

digits.

For example, if M98 P21 is programmed, a search is undertaken for the 0021.spf program

name in the part program memory and the subprogram is run once. If the subprogram is to be

run three times, M98 P30021 should be programmed.

To date the number of program passes (number of repeats) in ISO dialect M/T has been

programmed with the subprogram number under address "P".

As an alternative to this programming syntax, the number of subprogram passes can now also

be programmed under address "L". The subprogram number is still programmed with Pxxxx. If

the number of passes is programmed with both addresses, the number of passes programmed

with address "L" applies. The number of subprogram passes may be between 1 and 9999.

Example:

N20 M98 P20123

;The 123.spf subprogram is executed twice

N40 M98 P55 L4

;The 55.spf subprogram has been executed four times

N60 M98 P30077 L2

;The 77.spf subprogram is executed twice

;The number of passes =3 programmed at address "P" is ignored.

End subprogram

The subprogram is ended with M99.

If M99 Pxxxx is programmed, a move is made to block number Nxxxx when returning to the

main program. The block number must always start with "N". The block number is first looked

for in a forward direction (from subprogram call working towards program end). If no suitable

block number is found, the part program is eventually searched in the reverse direction (in the

direction of the start of the part program).

If M99 has no block number (Pxxxx) in a subprogram, the subprogram is ended and a jump

made to the block after the subprogram call in the main program.

If M99 is without a block number (Pxxxx) in a main program, the control goes to the start of the

main program and the main program is processed afresh.

These M commands are not output to the PLC.

M99 does not reset the program runtime. An activated tool counter is not incremented.

Subprogram return with "RET"

Applies to ISO dialect T only.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

After scrubbing, in the Siemens shell cycles for stock removal (as in ISO dialect) the program

should continue in the main program following the contour description. To do this, the shell

cycle must return to the block after the end of the contour description in the subprogram. In

order to jump the blocks with the contour description during stock removal cycles after the

subprogram call (with G71-G73), two optional parameters are added to the RET command.

Program processing in the program being called (main program) with the block <block number/

label> is continued with the RET command (STRING <block number/label>).

If program processing is to be continued with the next block after <block number/label>, the 2nd

parameter in the RET command must be programmed > 0 RET (<block number/label>, 1). If a

value > 1 is programmed for the 2nd value, the subprogram also returns to the block after the

block with <block number/label>.

The contour to be processed is saved in the main program for cycles G70-G73. The extended

RET command is needed to start at the end of G70 (finishing cut above contour with stock

removal cycle) in the main program after the contour description. To jump to the next NC block

after the contour description at the end of the shell cycle for G70, this must end with the

following return syntax:

RET ("N" << $C_Q, 1)

Search direction:

The search direction for <block number/label> is always firstly forward direction (heading

towards program end) and then reverse direction (heading towards program start).

Example

N10 X10. Y20.

N20 G71 P30 Q60 U1 W1 F1000 S1500

N10 ...

;Shell cycle for stock removal cycle

N20 DEF STRING[6]BACK

N30 ...

N90

N100 RET ("N"<<$C_Q, 1)

;Jump back to block after

;contour definition -> N70

N30 X50. Z20.

N40 X60.

N50 Z55.

N60 X100. Z70.

N70 G70 P30 Q60

N80 G0 X150. Z200.

N90 M30

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

Note

In Siemens mode, M30 is interpreted in the subprogram as a program return jump.

In ISO dialect mode, M30 is also interpreted in the subprogram as part program / end of

program.

3.4.2

Siemens language commands in ISO dialect mode

Programming

Certain Siemens language commands are also needed in ISO dialect mode for ShopMill.

These are then run in ISO dialect mode. These language commands include subprogram calls

with and without the transfer of parameters (not calls with Lxx because address L already has

a different meaning with ISO dialect), program part repeat and control structures. All other

Siemens language commands are rejected with an alarm in ISO dialect mode.

When ISO dialect mode is active, the following Siemens language commands may be

programmed:

REPEAT:

REPEAT

Block number > [<block number>] [P..]

REPEAT

UNTIL

REPEATB

<block number> [P..]

Only block numbers and not labels are permitted as start and end delimiters.

IF - ELSE - ENDIF

FOR - ENDFOR

WHILE - ENDWHILE

IF<condition> - GOTO F<condition>

CASE

Modal and non-modal subprogram calls

N100 CALL "SHAFT" or

N100 MCALL SHAFT" or

N100 SHAFT

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

Modal and non-modal subprogram calls with transfer of parameters

N100 MCALL SHAFT ("ABC"; 33.5 ) or

N100 SHAFT ("ABC"; 33.5 ) subroutine calls with path name

N100 CALL"/_N_SPF_DIR/SHAFT or

N100 MCALL/_N_SPF_DIR/SHAFT or

N100 PCALL/_N_SPF_DIR/SHAFT

3.4.3

Expansion of subprogram call for contour preparation with CONTPRON

Expansion

With ISO dialect the contour description for the stock removal cycles G70-G73 is not saved

separately in a subprogram (as with SINUMERIK), but in the part program (main program).

When calling the cycles, the range of the contour description is defined with a start and end

block number. The cycles contain these block numbers as transfer parameters. The indirect

subprogram call is expanded for the Siemens adjustment cycles.

Until now a subprogram call has been called indirectly with CALL <program name>.

The indirect subprogram call is expanded as follows for accessing the contour description in the

main program:

CALL [<program name>] BLOCK <start label> TO <end label>

If there is no program name stated or if an empty string is stated as the program name, i.e. CALL

BLOCK <Start label> TO <End label>, the program part (start/end label) is sought in the

program currently selected. The labels are also sought in the selected program for MDA, ASUB

etc. (e.g. in the case of MDA, labels are not sought in the MDA buffer but in the program with

the selected program name). If this syntax is written directly in a main program, it acts like a

program part repeat with REPEAT <Start label> <End label> with a loop pass, i.e. start and end

label are sought in the same program, in which the CALL BLOCK ... command is also

programmed.

If a program name is stated, i.e. CALL <progName> BLOCK <Start label> TO <End label>, the

program part (start/end label) is sought in the "progName" subprogram.

Example

Nxx G71 Pxx Q1110 U.. W..

;ISO dialect G function calls shell cycle

;CYCLE395.spf

;_N_CYCLE395_SPF

N10

Nxxx CYCLE95(

, "N"<<$C_P, "N"<<$C_Q)

;Stock removal cycle with additional parame-

ters

;for start and end label

PROC CYCLE95(

, STRING[20] start lab, STRING[20]

end lab)

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N10

Nxxx CONTPRON(...)

CALL "" BLOCK start lab TO end lab

;Read contour definition or

CALL BLOCK start lab TO end lab

;Call contour program

EXECUTE(...)

Nxx M17

Nxxx

Nxxx RET ("N"<<$C_Q, 1)

;Return to next block after

;contour definition

N1120

Nxxx M30

Note

CONTPRON and EXECUTE calls themselves must not be changed.

Searching for start block number

The search for the start block number (start label) of the contour description always takes place

first working towards the program end (forwards) and then working towards the program start

(backwards).

If the same block number is programmed several times, the next block number (label) after the

current block in the program containing the contour description is recognized as the start of the

contour description (see example). The current block is usually the block in which the stock

removal cycle (shell cycle) was called in the main program.

Example:

In stock removal cycle CYCLE395, the contour description found in the main program between

blocks N10-N30 is to be used (with CALL BLOCK N10 TO N30 in CYCLE395). N40 is the

current program line in the main program.

The contour description block in our example is shown in bold.

N5 G1 F500

N10 X10. Y20.

N20 X30.

N30 Y10.

N40 G71 P10 Q30...

;Call shell cycle for stock removal cycle

;(In the stock removal cycle,

;"CALL BLOCK N10 TO N30" is programmed)

;The bold lines are found as the

;contour definition

N50 G90 G54

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N60 F1000 G94

N10 X50. Y10.

N20 X33. Y11.

N30 X10.

N50

N800 G71 P10 Q30

;Call shell cycle for stock removal cycle

;(In the stock removal cycle, "CALL BLOCK N10 TO

N30"

; is programmed)

;The lines printed in

;italics are found as the contour definition

N999

N10 X15.

N20 Y25.

N30 X33.

N1010 ...

N1020

3.4.4

Macro commands with G65, G66 and G67

ISO dialect

In ISO dialect mode, G65 Pxx and G66 Pxx are used to call macros in the part program. The

combination of several part program blocks which are terminated with M17 is known as a

macro.

When calling the subprogram, a switch is made from ISO mode to Siemens mode.

The following commands are used for selection and deselection:

● G65 macro call, non-modal effective

● G66 macro call, modal effective

● Deselect G67 modal macro call

Siemens

G commands G65 Pxx and G66 Pxx start macro xx. G65 calls the Pxx subprogram once, G66

makes subprogram call Pxx modal and it is executed in each block with axial motion (as MCALL

xx). G67 deselects the modal subprogram call again (corresponds to G80 for cycle calls).

In a part program block containing G65 or G66, the address Pxx is interpreted as the program

number of the subprogram in which the macro functionality is programmed. The number of

passes of the macro can be defined with the address Lxx. If the number of passes is not

programmed in the call block, the macro is run once. All other addresses in this part program

block are interpreted as transfer parameters and their programmed values are stored in the

system variables $C_A to $C_Z. These system variables can be read in the subprograms and

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

evaluated for the macro functionality. If other macros with parameter transfer are called in a

macro (subprogram), then the transfer parameters in the subprogram must be saved in internal

variables before the new macro call.

To enable internal variable definitions, one must switch automatically to the Siemens mode for

a macro call. If another macro call is programmed in the subprogram, then the ISO dialect mode

must be reselected in advance.

System variables for the addresses I, J, K

As the addresses I, J, and K can be programmed up to ten times in a block containing macro

call, the system variables of these addresses must be accessed with an array index. The syntax

of these three system variables thus is $C_I[..], $C_J[..], $C_K[..]. The values remain in the

programmed sequence in the array. The number of I, J, K addresses programmed in the block

is given in the variables $C_I_NUM, $C_J_NUM, $C_K_NUM.

The transfer parameters I, J, K for macro calls are treated in each case as one block even if the

individual addresses are not programmed. If a parameter is reprogrammed, or a following

parameter based on the I, J, K sequence has been programmed, it belongs to the next block.

The system variables $C_I_ORDER, $C_J_ORDER, $C_K_ORDER are set to detect the

programming sequence in ISO mode. These are identical arrays to $C_I, $C_K and they

contain the associated numbers of the parameters.

Note

The transfer parameters can only be read in the subprogram.

Example:

N5 I10 J10 K30 J22 K55 I44 K33

;

[ Block1 ] [Block2] [Block3]

$C_I[0]=10

$C_I[1]=44

$C_I_ORDER[0]=1 ; Block 1

$C_I_ORDER[1]=3 ; Block 3

$C_J[0]=10

$C_J[1]=22

$C_J_ORDER[0]=1 ; Block 1

$C_J_ORDER[1]=2 ; Block 2

$C_K[0]=30

$C_K[1]=55

$C_K[2]=33

$C_K_ORDER[0]=1 ; Block 1

$C_K_ORDER[1]=2 ; Block 2

$C_K_ORDER[2]=3 ; Block 3

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

Cycle parameter $C_x_PROG

In the ISO dialect 0 mode, the programmed values can be evaluated in different ways,

depending on the programming method (integer or actual value). The different evaluation is

activated using machine data.

If the MD is set, the control system responds as in the following example:

X100. ; X axis is traversed through 100 mm (100. with point => actual

value)

Y200 ; Y-axis is traversed through 200 mm (200 without point =>

integer value)

If the addresses programmed in the block are used as transfer parameters for cycles, then the

programmed values always exist as real values in the $C_x variables. For integer values, one

cannot take recourse to the programming method (real/integer) in the cycles any more, and

therefore there is no evaluation of the programmed values with the correct conversion factor.

To identify whether REAL or INTEGER has been programmed, refer to system variable

$C_TYP_PROG, which is structured just like $C_ALL_PROG and $C_INC_PROG. There is

one bit for each address (A-Z). If the value is programmed as INTEGER, bit 0 is set, for REAL

to 1. If the value is programmed using a variable $<Number>, then bit 2 is set = 1.

Examples

● P1234 A100. X100 ⇒ $C_TYP_PROG == 1

Only bit 0 == 1, as only A was programmed as REAL.

● P1234 A100. C20. X100 ⇒ $C_TYP_PROG == 5

Bit 1 == 1 and bit 3 == 1 (A and C).

Restrictions

A maximum of ten I, J, K parameters can be programmed in each block. Only one bit each is

provided for I, J, K in the variable $C_TYP_PROG. Hence in $C_TYP_PROG bits is always set

to 0 for I, J and K. Therefore it cannot be derived whether I, J or K is programmed as REAL or

as INTEGER.

Parameters P, L, O, N can only be programmed as integers. A real value results in an alarm.

The bit in $C_TYP_PROG is therefore always 0.

Modal macro calls

For modal macro calls, the programmed addresses are only written to the system variables in

the call block (block with G66). The macro is then executed in each block with axial motion until

deselected with G67 or until a new macro call is programmed with G66. Only macro parameters

are provided for modal macros in the call block (= block with G66). The macro is first run in the

next block with axial motion. (Process as with MCALL xx in Siemens mode.)

Example of macro call:

_N_M10_MPF:

N10 M3 S1000 F1000

N20 X100. Y50. Z33.

N30 G65 P10 F55 X150. Y100. S2000

N40 X50.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N50

N200 M30

Example of a subprogram as a macro in Siemens mode:

_N_10_SPF:

N10 DEF REAL X_AXIS Y_AXIS, SPEED, FEEDRATE

N15 X_AXIS = $C_X Y_AXIS = $C_Y SPEED = $C_S FEEDRATE = $C_F

N20 G01 F=FEEDRATE G95 S=SPEED

M17

3.4.5

Changing mode during macro calls with G65/G66

In the past during macro calls with G65/G66, a switch has been automatically made into

Siemens mode.

The user can now decide whether a switch is to be made to Siemens mode at the start of the

macro. If the first program line of the macro program contains the operation PROC<Program

name>, a switch is made into Siemens mode. If this operation isn't there, ISO mode is retained

in the macro program.

The user can then decide whether to create local variables (with DEF...) to save transfer

variables. To do this, the user must switch into Siemens mode with the PROC operation. But

he or she can also decide whether his or her macro program (e.g. an existing ISO dialect M/T

macro) can be processed in ISO mode.

Example of the macro call:

_N_M10_MPF:

N10 M3 S1000 F1000

N20 X100. Y50. Z33.

N30 G65 P10 F55 X150. Y100. S2000

N40 X50.

N50

N200 M30

Example of a subprogram as a macro in Siemens mode:

_N_0010_SPF:

PROC 0010

; Changeover to Siemens mode

N10 DEF REAL X_AXIS, Y_AXIS, SPEED, FEEDRATE

N15 X_AXIS= $C_X Y_AXIS= $C_Y SPEED= $C_S FEEDRATE= $C_F

N20 G01 F=FEEDRATE G95 S=SPEED

N80 M17

Example of a subprogram as a macro in ISO mode:

_N_0010_SPF:

G290

; Changeover to Siemens mode

;if transfer variables have to be read

N15 X_AXIS= $C_X Y_AXIS= $C_Y SPEED= $C_S

N20 G01 F= $C_F G95 S= $C_S

N10 G1 X= $C_X Y= $C_Y

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

G291; Changeover to ISO mode

N15 M3 G54 T1

N20

N80 M99

3.4.6

Macro call via M function

Function

A macro can be called using M numbers in the same way as G65 (see "Mode changeover

during macro calls with G65/G66" chap.).

10 M function replacements are configured using the following machine data:

● MD10814 $MN_EXTERN_M_NO_MAC_CYCLE and

● MD10815 $MN_EXTERN_M_NO_MAC_CYCLE_NAME.

Parameter transfer is identical to G65. Repetitions can be programmed with the L address.

Constraints

Only one M function replacement (or only one subprogram call) can be executed per part

program line. Conflicts with other subprogram calls are reported using alarm 12722 "Channel

%1 block %2 Several ISO_2/3 macro or cycle calls in the block". There is no further M function

replacement in the replaced subprogram.

Otherwise, the same constraints are valid as in G65.

Conflicts with pre-defined and other defined M numbers are rejected with an alarm.

Configuration examples

Call of subprogram M101_MACRO via the M101 M function

MD10814 $MN_EXTERN_M_NO_MAC_CYCLE[0] = 101

MD10815 $MN_EXTERN_M_NO_MAC_CYCLE_NAME[0] = "M101_MACRO"

Call of subprogram M6_MAKRO via the M6 M function.

MD10814 $MN_EXTERN_M_NO_MAC_CYCLE[1] = 6

MD10815 $MN_EXTERN_M_NO_MAC_CYCLE_NAME[1] = "M6_MACRO"

Programming example for tool change with M function:

PROC MAIN

N10

M6 X10 V20

N90

M30

PROC M6_MACRO

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N0010

R10 = R10 + 11.11

N0020

IF $C_X_PROG == 1 GOTOF N40

;($C_X_PROG)

N0030

SETAL(61000)

;programmed variable not

;transferred correctly

N0040

IF $C_V == 20 GTOF N60

;($C_V)

N0050

SETAL(61001)

N0060

M17

3.4.7

Macro call via G function

Function

A macro can be called using a G number in the same way as G65 (see "Mode changeover

during macro calls with G65/G66" chap.).

50 G function replacements can be configured using the following machine data:

MD10816 $MN_EXTERN_G_NO_MAC_CYCLE and

MD10817 $MN_EXTERN_G_NO_MAC_CYCLE_NAME

The parameters programmed in the block are stored in the $C_variables. The number of macro

repetitions is programmed with address L. The number of the programmed G_macros is stored

in the variable $C_G. All the other G functions programmed in the block are treated as normal

G functions. The programming sequence of the addresses and G functions in the block is

random, and it does not have any effect on the functionality.

All ISO G codes, including G codes with a decimal point (= real value), can be replaced by a

macro call.

G functions which are not replaced by a macro are still present in the control and can be

redefined using MD10882 $MN_NC_USER_EXTERN_GCODES_TAB[ ].

Constraints

Only one G/M function replacement (or only one subprogram call) can be executed per part

program line. Conflicts with other subprogram calls, e.g. if a modal subprogram call is active,

are reported using alarm 12722 "Channel %1 block %2 Several ISO_2/3 macro or cycle calls

in the block".

If a G macro is active, no other G/M macro or M subprogram is called. M macros/subprograms

are then executed as M functions and G macros as G functions, if there is an appropriate G

function. Otherwise, alarm 12470 is triggered.

Otherwise, the same constraints are valid as for G65

Configuration examples

Calling the subprogram G21_MACRO via G function G21

$MN_EXTERN_G_NO_MAC_CYCLE[0] = 21

$MN_EXTERN_G_NO_MAC_CYCLE_NAME[0] = "G21_MACRO"

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

$MN_EXTERN_G_NO_MAC_CYCLE[1] = 123

$MN_EXTERN_G_NO_MAC_CYCLE_NAME[1] = "G123_MACRO"

$MN_EXTERN_G_NO_MAC_CYCLE[2] = 421

$MN_EXTERN_G_NO_MAC_CYCLE_NAME[2] = "G123_MACRO"

Programming example

PROC MAIN

N0090 G291

;ISO mode

N0100 G1 G21 X10 Y20 F1000 G90

;Call of G21_MACRO.spf,

;G1 and G90 are activated

;before the call of

;G21_MACRO.spf

N0500 G90 X20 Y30 G123 G1 G54

;Call of G123_MACRO.spf,

;G1, G54 and G90 are activated

;before the call of

;G123_MACRO.spf

N0800 G90 X20 Y30 G421 G1 G54

;Call of G421_MACRO.spf,

;G1, G54 and G90 are activated

;before the call of

;G123_MACRO.spf

N0900 M30

PROC G21_MACRO

N0010 R10 = R10 + 11.11

N0020 IF $C_X_PROG == 0

N0030 SETAL(61000)

;programmed variable not

;transferred correctly

N0040 ENDIF

N0050 IF $C_V_PROG == 0

N0060 SETAL(61001)

N0070 ENDIF

N0080 IF $C_F_PROG == 0

N0090 SETAL(61002)

N0100 ENDIF

N0110 G90 X=$C_X V=$C_V

N0120 G291

N0130 G21 M6 X100

;G21->activate metric measuring system

; (no macro call)

N0140 G290

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

N0150 M17

PROC G123_MACRO

N0010 R10 = R10 + 11.11

N0020 IF $C_G == 421 GOTOF label_G421

;Macro functionality for G123

N0040 G91 X=$C_X Y=$C_Y F500

N1990 GOTOF label_end

N2000 label_G421:

;Macro functionality for G421

N2010 G90 X=$C_X

Y=$C_Y F100

N202

N3000 G291

N2010 G123

; Alarm 12470, because G123 is not a

;G function and a

;macro call is not possible for

; active macro.

;exception: The macro was called

;as subprogram with CALL

G123_MACRO.

N4000 label_end: G290

N4010 M17

3.4.8

High-speed cycle cutting G05 P..

G05 P.. high-speed cycle cutting is realized as a subprogram call.

Programming: G05 P.. L..

● Pxxxxx

Subprogram number, max. 10 characters

When calling, 0s are not filled as they are for M98.

● Lxxxx

Number of passes, L1 applies if L is not programmed.

Example:

G05 P10123 L3

10123.mpf is passed 3 times.

This call calls any subprogram. This subprogram may be a precompiled program, but doesn't

have to be. Only Siemens part programs can however be precompiled.

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

Programming

3.4 Subprogram and macro technology

Siemens mode has no equivalent for the G05 ISO dialect function. CYCLE305 gives the user

the opportunity to program their own functionality within the framework of the Siemens

functionality.

The CYCLE305.spf cycle is called when programming G05 in the following scenarios:

● G05 without P in block is skipped without alarm.

● G05.1 with and without P is skipped without alarm.

● G05 P0 or P01 are reserved for high-speed remote buffer B. This function is not supported.

All addresses programmed in the block are written into the cycle parameters $C_xx in the

scenarios stated. When calling CYCLE305, the mode does not automatically switch from ISO

to Siemens. If CYCLE305.spf is to be processed in Siemens mode, there must be a PROC

operation in the first program line as for macro calls with G65/G66.

As when programming G05, all functions programmed in the block are executed, i.e.

programmed axes are traversed, auxiliary functions output etc. The programmed addresses

are only written into the cycle parameters as additional information.

If G05 is programmed with a subprogram call (M98 P..) in the same block, alarm 12722

"Channel %1 block %2 Several ISO_2/3 macro or cycle calls in a block" is output.

3.4.9

Switchover modes for DryRun and skip planes

Changeover of the skip levels (DB21.DBB2) always represents an intervention in the program

run which has led to a short-term drop in velocity on the path. The same is true for the

changeover of the DryRun mode (DryRun = dry run feedrate DB21.DBB0.BIT6) from

DryRunOff to DryRunOn or vice-versa.

Drops in velocity can now be avoided by a new changeover mode that is limited in its function.

A drop in velocity is no longer required with a machine data assignment of 10706

$MN_SLASH_MASK==2 while changing the skip levels (i.e. a new value in the PLC->NCK-

Chan interface DB21.DBB2).

Note

The NCK processes blocks in two steps, the premachining and main runs (also pre-travel and

main run). The result of the premachining migrates to the preprocessing memory. Main

machining takes the oldest block in each case out of the preprocessing memory and traverses

its geometry.

Note

Changing the skip levels

Premachining is changed over with the machine data assignment $MN_SLASH_MASK==2

during a change in skip level! All blocks located in the preprocessing memory are traversed with

the old skip level. The user normally does not have any control over the fill level of the

preprocessing memory. The following effect is seen:

This will also be active "sometime" after the changeover of the DryRun mode!

ISO dialects

Function Manual, 12/2019, 6FC5397-7BP40-3BA1

SINUMERIK 840D sl. Service - Functions. Manual (2018-2020) - page 1