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

Programming

3.4 Subprogram and macro technology

Note

The part program command STOPRE vacates the preprocessing memory. If the skip level is

changed before STOPRE, then all the blocks after STOPRE are changed over securely. The

same is valid for an implicit STOPRE.

Changing the DryRun mode has the same constraints.

No drop in velocity is required when changing the DryRun mode with the machine data

assignment 10704 $MN_DRYRUN_MASK==2. Here too, only the premachining that leads to

the above-mentioned restrictions, is changed.

3.4.10

Eight-digit program number

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 6=1 activates an eight-digit program

number selection. This function impacts on M98 (see "Subprogram technique M98" chapter),

G65/66 (see "Mode changeover during macro calls with G65/G66" chapter) and M96 (see

"Interrupt program with M96/M97 (ASUB)" chapter).

y: Number of program passes

x: Program number

Subprogram call

$MC_EXTERN_FUNCTION_MASK, bit 6 = 0

M98 Pyyyyxxxx or

M98 Pxxxx Lyyyy

Program number max. 4 digits

Addition of program number always to 4 digits with 0

Example:

M98 P20012: calls 0012.mpf 2 passes

M98 P123 L2: calls 0123.mpf 2 passes

$MC_EXTERN_FUNCTION_MASK, bit 6 = 1

M98 Pxxxxxxxx Lyyyy

There is no extension with 0, even if the program number has less than 4 digits.

The number of passes and program number in P(Pyyyyxxxxx) cannot be programmed,

the number of passes must always be programmed with L!

Example:

M98 P123: calls 123.mpf 1 pass

M98 P20012: calls 20012.mpf 1 pass,

Caution: This is no longer compatible with ISO dialect original!

M98 P12345 L2: calls 12345.mpf 2 passes

ISO dialects

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

Programming

3.4 Subprogram and macro technology

Modal and blockwise macro G65/G66

$MC_EXTERN_FUNCTION_MASK, bit 6 = 0

G65 Pxxxx Lyyyy

Program number is always expanded to 4 digits using 0s. Program numbers with more than 4

digits result in an alarm.

$MC_EXTERN_FUNCTION_MASK, bit 6 = 1

G65 Pxxxx Lyyyy

0s are not added, even if the program number is less than 4 digits long. A program number with

more than 8 digits leads to an alarm.

Interrupt M96

Does not function in SINUMERIK 802D sl.

$MC_EXTERN_FUNCTION_MASK, bit 6 = 0

M96 Pxxxx

Program number is always expanded to 4 digits with 0s

$MC_EXTERN_FUNCTION_MASK, bit 6 = 1

M96 Pxxxx

0s are not added, even if the program number is less than 4 digits long. A program number with

more than 8 digits leads to an alarm.

3.4.11

System variable for level stack in ISO mode

In standard mode, the current program level is displayed in the $P_STACK system variable.

This variable is affected by all subprogram calls and returns. There are however subprogram

calls in ISO mode for which the current user variable level is not changed. You must know the

current program level in ISO mode in order to realize level-specific variables using GUDs.

System variable $P_IPO_STACK provides the current program level in ISO dialect mode.

The table below shows all the possible subprogram and macro calls in ISO mode and how they

impact on the current program level.

The calls in ISO mode are mapped on calls in standard mode such that the $P_STACK variable

contains the same information as before even in ISO mode.

The number of maximum possible subprogram calls remains unchanged.

System variable $P_IPO_STACK is incremented whenever a subprogram is started which is

programmed as a macro call with G65, G66, G code or M macro in ISO mode. $P_IPO_STACK

is decremented again when returning from such an ISO macro. If there are no ISO macros

active, $P_IPO_STACK = 0. $P_IPO_STACK therefore provides the number of currently active

ISO macros.

When calling an interrupt program defined with M96 Pxx, variable $P_IPO_STACK is also

incremented depending on MD $MC_EXTERN_FUNCTION_MASK, bit 11.

$MC_EXTERN_FUNCTION_MASK

Bit 12 = 0, $P_IPO_STACK is not changed by the interrupt program.

Bit 12 = 1, $P_IPO_STACK is incremented by the interrupt program.

ISO dialects

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

Programming

3.4 Subprogram and macro technology

Cycle calls with e.g. G81, G77 etc. or functions realized internally with cycles, e.g. G05, G72.1

etc. and subprogram calls with M98 Pxx do not affect $P_IPO_STACK.

Example:

Subprogram calls in ISO and standard mode.

M98 stands for subprogram calls without an increase in level

G65 P stands for a macro calls with an increase in level

Table 3-4

Subprogram and macro calls

$P_STACK

$P_IPO_STACK

Level 1

Level 2

Level 3

O111.mpf

N5 M98 P2222

O2222.mpf

G65 P3333

O3333.mpf

M99

M98 does not forward the levels. O1111.mpf and O2222.mpf work with the same $P_ISO_STACK content, G65 forwards the

levels such that O3333.mpf sees different content. $P_STACK continues to display the levels in standard mode.

$P_STACK

$P_IPO_STACK

Level 1

Level 2

Level 3

O1111.mpf

N5 G65 P2222

O2222.mpf

M98 P3333

O3333.mpf

M99

Switching from ISO to standard mode

$P_STACK

$P_IPO_STACK

Level 1

Level 2

Level 3

O1111.mpf

G291

N5 M98 P2222

O2222.mpf

G290

3333( )

3333.mpf

M30

G291

M99

N10 M30

Switching from standard to ISO mode

1111.mpf

N5 G290

N10 2222( )

2222.mpf

ISO dialects

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

Programming

3.4 Subprogram and macro technology

$P_STACK

$P_IPO_STACK

Level 1

Level 2

Level 3

G291

M98 P3333

O3333.mpf

M99

G290

M17

N15 M30

List of possible subprogram and macro calls in ISO mode

M98 Pxxxx

Subprogram call

Level is not changed

M98 Pxxxx Lyyyy

Up call with iteration

Level is not changed

G65 P

Non-modal macro

Level is increased

G66 P

Modal macro

Level is increased

G05

UP call CYCLE305

Level is not changed

M macro subst

10814: EXTERN_M_NO_MAC_CYCLE

Level is increased

M up subst.

10715: M_NO_FCT_CYCLE

Level is not changed

T subst

10717: T_NO_FCT_CYCLE_NAME

Level is not changed

G subst

10816: EXTERN_G_NO_MAC_CYCLE

Level is increased

M96

Interrupt ASUB

Level is changed depending on

$MC_EXTERN_FUNC-

TION_MASK, bit 12

Shell cycles:

Level is not increased

G code cycles:

G22 G23 G27 G28 G30 G30.1 G72.1 G50

Level is not increased

G code cycles, shell cycles:

$P_ISO_STACK has no meaning for the user because these cycles do not offer access for

writing.

Depending on machine datum $MC_EXTERN_FUNCTION_MASK, bit 12, variable

$P_ISO_STACK is incremented when calling an interrupt program (ASUB).

● Bit 12 = 0

Variable $P_ISO_STACK is not changed when calling an interrupt program defined with

M96 Pxx

● Bit 12 = 1

Variable $P_ISO_STACK is incremented when calling an interrupt program defined with

M96 Pxx

ISO dialects

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

Tool changes and tool offsets

4.1

Shared tool offset memory

4.1.1

Tool offsets: T, D (ISO dialect M)

Tool data, T/D number H number

As the Siemens and ISO dialect programs are intended to run alternately in the control, they

must be implemented using the Siemens tool data memory.

Each offset data set is assigned to a tool. This offset data set contains the length, geometry and

wear.

In Siemens mode the offset memory is addressed with T (tool number) and D (cutting edge

number), or T/D number for short.

In ISO dialect M programs the offset memory is addressed with D (radius) or H (length), referred

to below as the H number.

In order to be able to assign this H number unambiguously to a T/D number, an element

$TC_DPH[t,d] has been added to the offset data set. The H number of the ISO dialect is entered

in this element.

Table 4-1

Example: Tool offset data set

D/cutting edge

H number

Radius

Length

$TC_DPH

100,00

250,00

Example:

Siemens program

ISO dialect program

N10

G41 D3

N10

G41 H12 or G41 D12

When programming the H value in the ISO dialect M program, the corresponding $TC_DPH is

used to search for the offset data set in the active T and the tool is selected.

If an offset data set does not include an H number, this offset cannot be activated in ISO dialect

mode.

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

If an H is programmed but no offset data set with the corresponding H number is found or the

associated tool T is not selected, an alarm is output.

4.1.2

Possible H numbers

H = 0

H0 is an offset with the offset value 0. If H0 is programmed during G43/G44, G43/G44 remains

active but with the tool length 0. H0 cannot be programmed while G41/G42 is active,

however.

H = unique

Each H number can only occur once in any TO unit, otherwise unambiguous addressing of the

offset data set is not possible. If you try to assign an H number for a second time, an alarm

"17183 Channel %1 Set %2 H number already exists in T= %3 with D=%4" is sent from the

program on attempting to write the values. This alarm is offset data set-capable and NC start

clear.

Example:

N5 $TC_DPH[1,1] = 5

N10 $TC_DPH[2,1] = 5

If you try to assign an H number twice via BTSS (HMI, PLC), a negative acknowledgement is

output for this write attempt.

Changing the offset memory

Existing tool offsets can be overwritten with G10. New tool offsets are not created with G10.

Tool length geometry offset: G10 L10 Pxx Ryy

Tool length wear offset: G10 L11 Pxx Ryy

Radius geometry offset: G10 L12 Pxx Ryy

Radius wear offset: G10 L13 Pxx Ryy

P indicates the H number of the offset memory and R the value.

L1 can be programmed in place of L11.

Active plane

To ensure that the assignment of tool length offsets to the geometry axes is independent of the

plane selection, the setting data 42940 $SC_TOOL_LENGTH_CONST must contain the value

17. In this way length 1 is always assigned to the Z-axis.

Tool length selection

The tool length and tool radius are always programmed with D or H.

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

Example:

D/cutting edge

H number

Radius

Length

$TC_DPH

ISO dialect M:

G43 H4 or D4 ;Length selection

G42 D4 or H4 ;Radius selection

In ISO dialect M programs which are programmed with different D and H numbers, the offset

value must be entered twice.

Example:

D/cutting edge

H number

Radius

Length

$TC_DPH

ISO dialect M:

G43 H4 ;Length offset from T2 D3

G42 D5 ;Radius and length offset from T2 D4

Flat D number

If flat D numbers are active, the T is programmed independently of the H number. The system

no longer checks whether the H number matches the selected tool.

Even with flat D numbers an H number must be assigned to each offset memory.

Tool management

If tool management is active, sister tools have the same H number. They are differentiated by

means of duplo numbers.

With H99 the offset D1 for the currently selected tool is activated if tool management is active.

In ISO dialect M only numerical expressions are permissible as tool identifiers. Strings are not

permissible as identifiers.

Example: T = "2", selection with T2.

Tool length offset in multiple axes

Tool length offsets can be activated in multiple axes. The resulting tool length offset cannot be

displayed, however.

If T and D numbers are active, the Siemens T and D numbers are displayed.

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

For the active ISO dialect H and D numbers there are new BTSS variables that can be

displayed.

The machine data 22220 $MC_AUXFU_T_SYNC_TYPE defines whether output to the PLC

takes place during or after the movement.

The machine data 20110 $MC_RESET_MODE_MASK, bit6 can be used to specify that the tool

length offset remains active after a reset.

MD 20156 $MC_EXTERN_RESET_GCODE_MODE[7] is used to define whether the G code of

group 8 (G43, G44, G49) is retained after a reset or whether the setting from MD 20254

$MC_EXTERN_RESET_GCODE[7] takes effect after a reset.

The default settings for both machine data should be set such that after a reset G49 is active

and the tool length offset is deselected.

Example: Tool selection in ISO dialect M:

;(Fanuc 0 M tool offset with T, cutting edge number

;(the offsets are)

;(with G10)

G290

;Tool offset memory T2 cutting edge1:

N5000 $TC_DP1[2,1]=10

;Type

N5000 $ TC_DP1[2,1]=7

;ISO H number

;Tool offset memory T3 cutting edge2:

N5000 $TC_DP1[3,2]=10

;Type

N5000 $TC_DP1[3,2]=3

;ISO H number

;Tool offset memory T4 cutting edge3:

N5000 $TC_DP1[4,3]=10

;Type

N5000 $TC_DP1[4,3]=8

;ISO H number

G291

;Write tool offsets

;------------------------

;T2 cutting edge1

G10 L12 P7 R5

;T3 cutting edge2

G10 L10 P3 R15

G10 L12 P3 R10

N8 G01 G40 F5000 X0 Y0 Z0

N10 X50.

N15 Y50

N17 Z10.

N20 X0

N25 Y0

N30 X-10 Y-10

N30 T2

;Tool 2

N33 G43 H7 Z0

;H number 7

N35 G41 X0 Y0 Z0 D7

N40 X50.

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

N45 Y50.

N48 Z10.

N50 X0

N55 Y0

N60 G40 X-10 Y-10

N65 T3

N68 G43 H3 Z0

N70 G42 X0 Y0 Z0 D3

N75 X50.

N77 Y50.

N78 Z10.

N80 X0

N85 Y0

N90 G40 X-10 Y-10

N95 T4

N98 G43 H8 Z0

N100 G41 X0 Y0 Z0 D8

N105 X50.

N110 Y50.

N112 Z10.

N115 X0

N120 Y0

N125 G40 X-10 Y-10

M30

Whether the offset takes effect in the selection set or the next time the axis is programmed is

defined by machine data 20382 $MC_TOOL_CORR_MOVE_MODE.

4.1.3

Tool offset T (ISO dialect T)

The tool data is located in the Siemens tool data memory and corresponds to the offset data for

a Siemens cutting edge.

The meaning corresponds to the cutting edge position for Siemens turning tools.

In ISO dialect T, the tool number and correction number are both programmed in the T word.

During interpretation, the T word is split according to the tool number and correction number.

The following possibilities now exist:

10889 $MN_EXTERN_DIGITS_OFFSET_NO, number of digits for correction number.

Range of values 0-8, default value 0

The function is deactivated with 0.

The number of digits is counted from the T word from the right, the rest is the tool number.

Example: $MN_EXTERN_DIGITS_OFFSET_NO = 3

T1234 is split into T1 H234

10888 $MN_EXTERN_DIGITS_TOOL_NO, number of digits for tool number.

Range of values 0-8, default value 2

The function is deactivated with 0.

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

The number of digits is counted from the T word from the left, the rest is the correction number.

Example: $MN_EXTERN_DIGITS_TOOL_NO = 3

T1234 is split into T123 H4

Only one of the two functions may be active to split the T word. If both machine data have a

value of 0, splitting is not possible. Programming T results in NC alarm 12550.

If both machine data have a value of < > 0, splitting is not possible. Programming T results in

NC alarm 12550.

The function is compatible with the standard values of previous statuses.

Examples

$MN_EXTERN_DIGITS_OFFSET_NO = 0

$MN_EXTERN_DIGITS_TOOL_NO = 2

Splitting according to tool numbers, 2 digits

T123 becomes T12 H3

T0123 becomes T1 H23

$MN_EXTERN_DIGITS_OFFSET_NO = 3

$MN_EXTERN_DIGITS_TOOL_NO = 0

Splitting according to tool numbers, 3 digits

T1234 becomes T12 H234

T01234 becomes T1 H234

$MN_EXTERN_DIGITS_OFFSET_NO = 3

$MN_EXTERN_DIGITS_TOOL_NO = 2

Splitting not possible because both functions are activated. T programming results in alarm

12550.

$MN_EXTERN_DIGITS_OFFSET_NO = 0

$MN_EXTERN_DIGITS_TOOL_NO = 0

Splitting not possible because both functions are deactivated. T programming results in alarm

12550.

Changing the offset memory

Existing tool offsets can be overwritten with G10. New tool offsets are not created with G10.

G10 P<100 / 10000 X Y R Q Geometry

G10 P>100 / 10000 X Y R Q Wear

P100/10000

;With MD 20734: EXTERN_FUNCTION_MASK, bit 1 is selected,

;when P<100 or 10000, whether differentiation is by geometry

;or wear.

X Y Z

;Offset values absolute or incremental, depending on G90/91

U V W

;Offset values incremental

;Radius

;Cutting edge position

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

Tool offset selection with $TC_DPH

In ISO dialect T the "flat D numbers" function has previously always been active. The D

numbers are unique; with the command Txxyy or G10 Pyy the Siemens cutting edge number

is addressed with yy. In order to use tool management in ISO dialect T, structured D numbers

must be addressed. Just as in ISO dialect M, each cutting edge is therefore given a parameter

$TC_DPH[°], which allows a cutting edge to be addressed unambiguously within a TO unit.

The function is switched on with MD 10890 $MN_EXTERN_TOOLPROG_MODE bit 2=1.

If the function is active, the tool offset must always be addressed with the H number in ISO

dialect T. Programs which address the cutting edge number no longer run. The parameter

$TC_DPH[ ] is only created if $MN_EXTERN_TOOLPROG_MODE bit 2=1. The H numbers

must be allocated unambiguously within a TO unit, otherwise alarm 17183 is output.

There are three options:

$MN_MM_TYPE_OF_CUTTING_EDGE=1 flat D number

1. Flat D number + $MN_EXTERN_TOOLPROG_MODE bit 2=0

The offset is always addressed with cutting edge D.

G290

N605 $TC_DP1[1]= 500

N615 $TC_DP1[2]= 500

N625 $TC_DP1[3]= 500

N635 $TC_DP1[4]= 500

G291

N650 G10 P2 X10

;Write cutting edge 2 geometry

N655 G10 P102 X1

;Write cutting edge 2 wear

N670 T0102

;Select cutting edge 2

N675 T0105

;Alarm because cutting edge 5 does not ex-

ist

2. Flat D number + $MN_EXTERN_TOOLPROG_MODE bit 2=1

The offset is always addressed with the H number.

G290

N705 $TC_DP1[1]= 500

N708 $TC_DPH[1]=11

N710 $TC_DP1[2]= 500

N715 $TC_DPH[2]=22

N720 $TC_DP1[3]= 500

N725 $TC_DPH[3]=33

N730 $TC_DP1[4]= 500

N735 $TC_DPH[4]=44

G291

N740 G10 P22 X10.

;Write cutting edge 2 geometry

N745 G10 P122 X1.

;Write cutting edge 2 wear

N747 G10 P55 X10.

;Alarm 12550 because cutting edge does

;not exist with H55

ISO dialects

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

Tool changes and tool offsets

4.1 Shared tool offset memory

N750 T0122

;Cutting edge 2 is selected

N752 T0155

;Alarm 12550 because cutting edge does

;not exist with H55

$MN_MM_TYPE_OF_CUTTING_EDGE=0

Structured D number

3. Structured D number + $MN_EXTERN_TOOLPROG_MODE bit 2=1

The offset is always addressed with the H number.

G290

N805 $TC_DP1[1,1]= 500

N808 $TC_DPH[1,1]=11

N810 $TC_DP1[1,2]= 500

N815 $TC_DPH[1.2]=22

N820 $TC_DP1[2,1]= 500

N825 $TC_DPH[2,1]=33

N830 $TC_DP1[2,2]= 500

N835 $TC_DPH[2,2]=44

G291

N840 G10 P22 X10

;Write T1 cutting edge 2 geometry

N845 G10 P122 X1

;Write T1 cutting edge 2 wear

N847 G10 P55 X1

;Alarm 12550 because cutting edge does

;not exist with H55

N850 T0122

;Select T1 cutting edge 2.

N855 T0244

;Select T2 cutting edge 2

;Alarm because cutting edge

;does not exist in T2 with H22.

4.1.4

Tool change cycle

ISO dialect mode

A subprogram is assigned to the T command using MD 10717 T_NO_FCT_CYCLE_NAME.

Each set containing a T command is executed and then the subprogram is called. The T value

is not output; the T word has to be programmed again in the cycle.

In the subprogram the system variable $C_T_PROG or $C_D_PROG can be used to query

whether T or D has been programmed. The values can be read with the system variables $C_T

and $C_D respectively. If another T command is programmed in the subprogram, no

replacement is made but the T word is output to the PLC.

A subprogram can be assigned to an M function (e.g., M06) using MD 10715

M_NO_FCT_CYCLE and 10716 M_NO_FCT_CYCLE_NAME.

The mapping of M, T programming to cycle calls is the same in ISO dialect mode as in Siemens

mode.

If T and M6 are programmed in a set, the programmed T number can be queried in the cycle

called with M6 using GETSELT(). GETSELT() gets the T number of the preselected tool. In the

ISO dialects

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

Cycles and contour definition

5.1

Sequence of cycle calls in the external CNC system using G

commands

General description

The functionality of the ISO dialect cycles is realized in the Siemens standard cycles:

A shell cycle is called from the ISO dialect program. All addresses programmed in the block are

transferred to this shell cycle in the form of system variables. The shell cycle customizes this

data to the standard Siemens cycle and calls its name.

The machine manufacturer can replace the shell cycles with its own ones.

Cycle parameters

During machining cycles, various cycle parameters should be preset in channel-specific GUDs

(Global User Data). The names and meanings of the GUDs are listed in the "Global user data

(GUD)" chapter.

Sequence for calling cycles using G command

3DUW SURJUDP

H[WHUQDO &1& V\VWHP

H J ,62 GLDOHFW

6KHOO F\FOH

;

6LHPHQV VWDQGDUG F\FOH

Figure 5-1

General cycle sequence in ISO dialect mode

Shell cycle

The customizations, required due to the ISO dialect programming syntax, are undertaken in the

shell cycle. The existing SINUMERIK cycles do not need to be changed for this. The shell cycle

name is permanently assigned.

ISO dialects

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

Cycles and contour definition

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

Sequence:

1. The cycle (e.g. G81) is programmed in ISO dialect mode

2. A switch is made automatically to Siemens mode and the associated shell cycle called (see

previous figure)

3. The shell cycle calls the associated standard Siemens cycle

Programming with G290 is not needed. A switch is automatically made to the external CNC

system when returning.

Note

The cycles may only be called with the G commands.

This ensures that the shell cycle is provided with the appropriate cycle parameters.

The shell cycle must not be called directly with CALL CYCLE3xx!

Modally effective cycles

If a modal cycle is active, the shell cycle is called in each NC block. If there are no axis positions

(X, Y or Z) programmed in the NC block, the standard Siemens cycle is not called.

Addresses programmed in the block (F etc.) are activated by the shell cycle. For example, if a

feedrate has not been programmed, the current feedrate is used as the path feedrate.

Cycle parameters can be programmed in the following blocks while a modal cycle is active.

These parameters are written to the system variables so that the shell cycle works with the

modified parameters.

Unlike modal macros, modal cycles are executed in the call block (e.g. block with G81 etc.).

Cycle deselection:

G80 or a G function of the 1st G group is used for deselection.

Example:

N10 G81 X10. Y20. Z-15. R5 F1000

Drilling position X10 mm, Y20 mm

Drilling depth Z-15 mm

Reference plane 5 mm

Drilling feedrate F.. (mm/min or mm/rev.)

N20 X50. Y30. R10

Drilling position X50 mm, Y30 mm,

New reference plane 10 mm

N30 G80

Delete cycle G81

Writing cycle variable, depending on programmed addresses in block

During active modal cycles, to date all programmed addresses in the block have always been

written into the cycle variables. The variables are evaluated in the cycle where a decision is

made on the basis of the cycle logic as to how the variables have to be used.

ISO dialects

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

Cycles and contour definition

5.2 Global user data (GUD)

In many cases this results in the cycle parameters being described even if they cannot be

interpreted as cycle parameters because of their programming syntax.

None, or no longer all of the programmed addresses are therefore written in the cycle

parameters for the following functions:

M98 P3 L2 X10 Y20

Addresses Pxx and Lxx are not written in the cycle parameters.

G05 P5 L2 X10 Y20

Addresses Pxx and Lxx are not written in the cycle parameters.

G05 P1 L2 X10 Y20

During an active modal cycle, alarm 12722 is output because

CYCLE305, for which the programmed values are actually in-

tended, is called here after the modal cycle.

G54 P10 X10 Y20 M44

Address Pxx is not written in the cycle parameters.

G31 P98 X30 F100

Addresses Pxx, Fxx and axis values are not written in the cycle

parameters.

G31 P1 X30 Y20 F100

None of the programmed addresses are written in the cycle

parameters.

G51 P1000 I2 J3 K2 X30 Y40

None of the programmed addresses are written in the cycle

parameters.

G50 P10000 X10 Y30

All parameters are written in the cycle parameters.

5.2

Global user data (GUD)

Table 5-1

SGUD for programmed cycle values (ISO dialect program data)

GUD

Description/use

CYCLE

Real values

_ZFPR[0]

Basis (current position for 1st call with G..), retraction position for G98

381M, 383M,

active

384M, 387M

_ZFPR[1]

Reference plane, retraction position for G99 active (only retraction to

381M, 383M,

starting position possible for G87)

384M, 387M

_ZFPR[2]

Final drilling depth, absolute

381M, 383M,

384M, 387M

_ZFPR[3]

Retraction position, depending on G98/G99 (basis/R plane)

381M, 383M,

384M, 387M

_ZFPR[4]

Drilling feedrate

381M, 383M,

384M, 387M

_ZFPR[5]

Dwell time (s) at final depth (G82/G89/G76/G87) [ms]

381M, 384M,

387M

_ZFPR[6]

1st drilling depth (individual drilling depth) incr. (G73/G83)

383M

_ZFPR[7]

1st absolute drilling depth (G73/G83)

383M

_ZFPR[8]

Lifting/feed in distance (G76)

387M

_ZFPR[9]

Speed for tapping (G74/G84)

384M

_ZFPR[10]

Programmable holding distance when dipping back into hole G83

383M

Values:

> > 0 programmable value applies

= 0 automatic calculation

ISO dialects

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

Cycles and contour definition

5.2 Global user data (GUD)

GUD

Description/use

CYCLE

_ZFPR[20]

Basis (current position for 1st call)

383T, 384T,

385T

_ZFPR[21]

R plane

383T, 384T,

385T

_ZFPR[22]

Final drilling depth, absolute

383T, 384T,

385T

_ZFPR[23]

Retraction position (1=G98, 2=G99)

383T, 384T,

385T

_ZFPR[24]

Thread lead/drilling feedrate

376T, 383T,

384T, 385T

_ZFPR[25]

Dwell time at final depth

383T, 384T,

385T

_ZFPR[26]

Speed for tapping

384T

_ZFPR[27]

End point X

371T, 372T,

373T, 376T

_ZFPR[28]

End point Z

371T, 372T,

373T, 376T

_ZFPR[29]

Start point offset X (taper thread)

371T, 372T,

376T

_ZFPR[30]

Thread start point X

376T

_ZFPR[31]

Thread start point Z

376T

_ZFPR[32]

First drilling depth

383T

Integer values

_ZFPI[0]

Current G code of ISO dialect drilling cycle

381M, 383M,

384M

_ZFPI[1]

M function for spindle start (M3, M4) after spindle stop

381M, 384M

_ZFPI[20]

Current G code of thread cycle/drilling cycle

383T, 384T,

385T

_ZFPI[21]

Spindle direction (3=M3, 4=M4)

383T, 384T,

385T

_ZFPI[22]

Roughing stock removal type

370T, 371T,

372T, 373T

_ZFPI[23]

Deep-hole / drilling machining type

383T

Assignment list of GUD parameters to the machine data for ISO cycles

GUD up to SW Version 1.5

MD/SD name

_ZSFI[0]

$SCS_ISO_M_DRILLING:AXIS_IS_Z

_ZSFI[1]

$SCS_ISO_M_DRILLING_TYPE

_ZSFI[2]

$SCS_ISO_M_RETRACTION_FACTOR

_ZSFI[3]

$SCS_ISO_M_ENABLE_POLAR_COORD

_ZSFI[4]

$SCS_ISO_ENABLE_INTERRUPTS

_ZSFI[5]

$SCS_ISO_M_RETRACTION_DIR

_ZSFI[6]

$SCS_ISO_ENABLE_DRYRUN

_ZSFI[7]

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

GUD up to SW Version 1.5

MD/SD name

_ZSFI[8]

$SCS_ISO_SIMULTAN_AXES_START

_ZSFI[9] ... _ZSFI[19]

_ZSFI[20]

$SCS_ISO_T_DEEPHOLE_DRILL_MODE

_ZSFI[21]

_ZSFI[22]

$SCS_ISO_T_RETRACTION_FACTOR

_ZSFI[23]

$SCS_ISO_T_DWELL_TIME_UNIT

_ZSFI[24] ... _ZSFI[38]

_ZSFI[39]

5.3

Drilling cycles (ISO dialect M)

5.3.1

Overview and parameter description

The drilling cycles are modal. When a drilling mode is active, only the new parameters have to

be programmed if a parameter is changed.

No traversing is executed if:

● no value is programmed for X, Y and Z in the NC block

● the number of repeats K=0 has been programmed

The retraction position applies to all drilling cycles

● G98 retraction at basis

● G98 retraction at datum plane

Overview

Table 5-2

Overview of drilling cycles

External cycle call

Description

G73 X.. Y.. Z.. R.. F.. Q..

Deep hole drilling cycle with chip breakage

G74 X.. Y.. Z.. R.. F.. P..

Left tapping cycle

G76 X.. Y.. Z.. R.. F.. Q.. P..

Fine drill cycle

G80

Cycle off; cycle is also deselected by programming a G function

from the 1st G group.

G81 X.. Y.. Z.. R.. F..

Drilling cycle; drilling, retraction with G00

G82 X.. Y.. Z.. R.. F.. P..

Drilling cycle; drilling, dwell time, retraction with G00

G83 X.. Y.. Z.. R.. F.. Q..

Deep hole drilling cycle with chip removal

G84 X.. Y.. Z.. R.. F.. P..

Right tapping cycle

G85 X.. Y.. Z.. R.. F..

Drilling cycle; drilling, retraction with drilling feedrate

G86 X.. Y.. Z.. F.. R.. K..

Drilling cycle, retraction with G00

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

External cycle call

Description

G87 X.. Y.. Z.. F.. R.. P.. Q.. K..

Reverse countersinking

G89 X.. Y.. Z.. F.. R.. P.. K..

Drilling cycle, retraction with machining feedrate

&\FOH FDOO IURP ,62

6LHPHQV

6KHOO F\FOH

GLDOHFW 0 PRGH

VWDQGDUG F\FOH

&<&/(

6ZLWFK LQWR

6LHPHQV PRGH

Figure 5-2

Assignment of cycle call to standard Siemens cycle in ISO dialect M mode using shell cycle

Example: ISO dialect M

N10 G81 X100. Z-50. R20 F100

G81 is used to automatically call the CYCLE381M shell cycle.

The calculations are carried out in the shell cycle and the standard drilling cycle CYCLE81 then

called.

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

Parameter description

* 9 RU

* 9 ;

)

1XPEHU RI UHSHWLWLRQV

LI QR . LV SURJUDPPHG

WKH F\FOH LV SHUIRUPHG RQFH

0DFKLQLQJ IHHGUDWH

'ULOOHG KROH

SRVLWLRQ

&RQWLQXRXV LQGLYLGXDO GULOOLQJ GHSWK ZLWK *

* OLIWLQJ SDWK ZLWK *

'ZHOO WLPH DW GULOOLQJ KROH GHSWK

IRU *

5HIHUHQFH SODQH

'ULOOLQJ KROH GHSWK

Figure 5-3

Description of permissible parameters for G17 (X/Y plane)

Plane

In drilling cycles, one generally assumes that the current coordinate system in which the

operation is to be executed, is defined through the selection of plane G17, G18 or G19 and

activation of a programmed work offset.

The drilling axis is then always the application of this coordinate system.

Table 5-3

Plane definition

Defined plane

Position of hole

Depth

G17

X, Y

G18

Z, X

G19

Y, Z

'ULOOLQJ WRRO

2XWSXW SODQH *

5 LQFU

5 DEV

'DWXP SODQH *

:RUNSLHFH VXUIDFH

= LQFU

= DEV

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

Figure 5-4

Example of deep hole drilling cycle G83 with defined plane G17. Representation of output

and datum plane and parameters

5.3.2

Description of shell cycle CYCLE381M

NOTE

It is called in ISO dialect M mode using the G commands G81, G82, G85, G86, G89.

The drilling axis should be defined via GUD _ZSFI[0] (see "Global user data (GUD)" chapter).

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth.

GUD _ZSFR[0] can be used to enter a safety clearance. If the safety clearance has already

been taken into account when programming the datum plane, 0 must be entered for _ZSFR[0].

If no datum plane has been programmed, drilling is undertaken from the basis (current position).

The final drilling depth must be programmed. Otherwise, an alarm is displayed.

If a feedrate is not programmed, the current feedrate is used as the drilling feedrate.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

5.3.3

Description of shell cycle CYCLE383M

Call

It is called in ISO dialect M mode using the G commands G73, G83.

NOTE

The drilling axis should be defined via GUD _ZSFI[0] (see "Global user data (GUD)" chapter).

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth.

GUD _ZSFR[0] can be used to enter a safety clearance. If the safety clearance has already

been taken into account when programming the datum plane, 0 must be entered for _ZSFR[0].

If no datum plane has been programmed, drilling is undertaken in stages from the basis (current

position).

The final drilling depth and the individual drilling depth Q must be programmed. Otherwise, an

alarm is displayed.

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

If a feedrate is not programmed, the current feedrate is used as the drilling feedrate.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

Deep hole drilling with chip removal (G83)

In the standard Siemens cycle, a formula is used to determine the holding distance, i.e. it cannot

be freely selected.

The system moves back to the datum plane for chip removal.

Individual drilling depth "Q":

● If there is no "Q" or if Q ≤ 0, an alarm is displayed.

● If Q > total depth, drilling is performed to the final depth.

● If Q > total depth/2, the first drilling process uses the Q value. The rest is then drilled in one

drilling process.

● If Q < total depth/2, the individual drilling depth is drilled until the residual depth is < Q/2. The

rest is then split into 2 infeeds of the same size.

Deep hole drilling with chip breakage

The retraction amount from chip breaking is defined with GUD _ZSFR[1].

● _ZSFR[1] > 0 Retraction amount as input

● _ZSFR[1] ≤ 0 Retraction amount is always 1 mm

Individual drilling depth "Q":

● If there is no "Q" or if Q ≤ 0, an alarm is displayed.

● If Q > total depth, drilling is performed to the final depth.

● If Q < total depth, the individual drilling depth is drilled until the residual depth is ≤ Q. The rest

is then drilled in one drilling process.

5.3.4

Description of shell cycle CYCLE384M

NOTE

It is called in ISO dialect M mode using the G commands G74, G84.

The drilling axis should be defined via GUD _ZSFI[0] (see "Global user data (GUD)" chapter).

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth.

GUD _ZSFR[0] can be used to enter a safety clearance. If the safety clearance has already

been taken into account when programming the datum plane, 0 must be entered for _ZSFR[0].

ISO dialects

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

Cycles and contour definition

5.3 Drilling cycles (ISO dialect M)

GUD _ZSFI[2] can be used to influence the speed when retracting.

Example: _ZSFI[2]=80, the retraction takes place at 80% of the drilling speed.

If no datum plane has been programmed, drilling is undertaken from the basis (current position).

The final drilling depth must be programmed. Otherwise, an alarm is displayed.

If a feedrate is not programmed, the current feedrate is used as the drilling feedrate.

If the drilling feedrate has been stated in mm/min (inch/min), the programmed feedrate value is

converted into the appropriate revolution feedrate depending on the last speed programmed

and transferred to the standard tapping cycle CYCLE84 as an incline value.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

5.3.5

Description of shell cycle CYCLE387M

NOTE

It is called in ISO dialect M mode using the G commands G76 and G87.

The drilling axis should be defined via GUD _ZSFI[0] (see "Global user data (GUD)" chapter)

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth.

GUD _ZSFR[0] can be used to enter a safety clearance. If the safety clearance has already

been taken into account when programming the datum plane, 0 must be entered for _ZSFR[0].

The lifting path always relates to the negative direction of the first geometry axis:

For plane G17: Lifting path in -X

For plane G18: Lifting path in -Z

For plane G19: Lifting path in -Y

The angle must therefore be entered such that the tool tip points to the spindle stop in the

positive direction (+) at the defined plane.

Example: Plane G17 active, then tool tip must be facing +X.

If no datum plane has been programmed, drilling is undertaken from the basis (current position).

The final drilling depth must be programmed. Otherwise, an alarm is displayed.

If a feedrate is not programmed, the current feedrate is used as the drilling feedrate.

In the absence of a programmed lifting amount, Q = 0 is set. The cycle is executed without lifting.

ISO dialects

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

After retraction to the retraction plane, the tool is again moved to the center of the hole and the

spindle started in the direction of rotation for processing.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

5.4

Turning and drilling cycles (ISO dialect T)

5.4.1

Turning cycles G70 to G76

Overview

Table 5-4

Overview of turning cycles

G command

Description

G70

Finishing cycle

G71

Stock removal cycle, longitudinal axis

G72

Stock removal cycle transverse axis

G73

Contour repetition

G74

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

G75

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

G76

Multiple thread cutting cycle

The cycle supply for G71 to G76 can consist of two G commands. Depending on the addresses

programmed in the block, only the values of the addresses programmed in the NC block are

saved so they can be used for a later cycle call or additionally to start cycle processing.

Evaluation is undertaken in the shell cycle in both cases.

ISO dialects

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

&\FOH FDOO RII

6LHPHQV

,62 GLDOHFW 7 PRGH

6KHOO F\FOH

VWDQGDUG F\FOH

5XQV ZLWKRXW

&<&/(

VWDQGDUG F\FOH

&<&/(

&KDQJHRYHU WR WKH 6LHPHQV PRGH

Figure 5-5

Assignment of cycle call to standard Siemens cycle in ISO dialect T mode using shell cycle

Finishing cycle G70

%ORFN QXPEHU LQ PDLQ SURJUDP DW ZKLFK WKH FRQWRXU GHILQLWLRQ HQGV

%ORFN QXPEHU LQ PDLQ SURJUDP DW ZKLFK WKH FRQWRXU GHILQLWLRQ VWDUWV

Figure 5-6

Description of permissible parameters

In ISO dialect mode, the contour is not skipped in the main program with G70. The program is

always processed in the next part program block after the cycle call.

Example:

When the cycle is called, the contour N20-N50 is traversed. After the end of the cycle, the part

program is processed from N20. Logically, G70 is always called after the contour description.

N10 G70 P20 Q50

N20 X100. Z50.

N30 X200.

N40 Z100.

N50 X250. Z111.

N60 M30

The blocks N20-N50 are processed once by the finishing cycle and then once again by the

normal program sequence.

ISO dialects

100

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

Stock removal cycle, longitudinal axis G71

8 5

5HWUDFWLRQ SDWK

,QIHHG GHSWK IRU VFUXEELQJ

Figure 5-7

Description of permissible parameters; save values in GUDs

4 8 :

)

7RRO VHOHFWLRQ

6SLQGOH VSHHG

0DFKLQLQJ IHHGUDWH

)LQLVKLQJ DOORZDQFH LQ WKH = D[LV

)LQLVKLQJ DOORZDQFH LQ WKH ; D[LV

%ORFN QXPEHU DW ZKLFK WKH FRQWRXU GHILQLWLRQ HQGV

%ORFN QXPEHU DW ZKLFK WKH FRQWRXU GHILQLWLRQ VWDUWV

Figure 5-8

Description of permissible parameters; start cycle processing

In ISO dialect T mode with G71 the contour is traversed to the finishing allowance in the main

program after scrubbing (residual corner stock removal). The program is always processed

with the part program block after the last block of the contour description. Part program blocks

which can be found between the cycle call and the first contour description block are not

executed.

N10 G71 P50 Q80 U4 W3 F1000 ...

N20 G1 F0.5 G95 S1000

N30 X30. Z10.

N40 M30

N50 X100. Z50.

N60 X200.

N70 Z100.

N80 X250. Z111.

N90 M30

The blocks N20-N40 are skipped and not executed. If G71 is called in the part program after

the contour description, the program runs in an infinite loop. The different ways in which the part

program is further processed must be taken into account in the shell cycles.

Example: G71 U6 R5 Save values in GUDs

In the example, the programmed values in the shell cycle are read from the system variables

($C_xx) and saved in channel-specific GUDs. There are separate GUDs for each cycle (G71-

G76), which ensures that the programmed values remain valid until they are programmed the

next time (in an NC block with G71-G76). Scenario 1 does not have to be programmed, so it

makes sense to precompile the assigned GUDs.

Example: G71 P30 Q50 U3 Start cycle processing

In the example, the programmed values are only saved in system variables ($C_xx). The

system variables are overwritten in each NC block in which a G function is programmed for the

cycle call. For G71-G73 the processing of cycles always starts with the G command after which

the "P" and "Q" addresses are programmed. Cycle processing G74-G76 is started with the G

command after which addresses X/U or Z/W are programmed. F, S and T commands in the

ISO dialects

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

101

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

cycle's call line are also stored in system variables. The addresses do not therefore have to

differ for specific cycles. The shell cycle assigns meaning to the parameters (e.g. for G76

address F = thread lead and not feedrate). For G70, feedrate, speed and tool selection

commands (F, S, T) from the program part of the contour description are relevant.

The same shell cycle is always called in both scenarios.

Stock removal cycle, transverse axis G72

: 5

5HWUDFWLRQ SDWK

,QIHHG GHSWK IRU VFUXEELQJ

Figure 5-9

Description of permissible parameters; save values in GUDs

Contour repetition G73

8 : 5

1XPEHU RI FXWV SDUDOOHO WR FRQWRXU

0RYHPHQW RI VWDUW SRLQW IURP FXUUHQW

WRRO SRVLWLRQ LQ WKH = D[LV

0RYHPHQW RI VWDUW SRLQW IURP FXUUHQW

WRRO SRVLWLRQ LQ WKH ; D[LV

Figure 5-10

Description of permissible parameters; save values in GUDs

4 8 : ) 6 7

7RRO VHOHFWLRQ

6SLQGOH VSHHG

0DFKLQLQJ IHHGUDWH

)LQLVKLQJ DOORZDQFH LQ WKH = D[LV

)LQLVKLQJ DOORZDQFH LQ WKH ; D[LV

%ORFN QXPEHU DW ZKLFK WKH FRQWRXU GHILQLWLRQ HQGV

%ORFN QXPEHU DW ZKLFK WKH FRQWRXU GHILQLWLRQ VWDUWV

Figure 5-11

Description of permissible parameters; start cycle processing

Deep-hole drilling and grooving in the longitudinal axis G74

5HWUDFWLRQ SDWK WR FKLS EUHDNLQJ

Figure 5-12

Description of permissible parameters; save values in GUDs

ISO dialects

102

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

;8 =: 3 4 5 )

0DFKLQLQJ IHHGUDWH

5HWUDFWLRQ SDWK DW HQWU\ EDVH

)HHG LQ LQ WKH ORQJLWXGLQDO D[LV = D[LV WR

FKLS EUHDNLQJ

)HHG LQ LQ WUDQVYHUVH D[LV ; D[LV IRU WKH QH[W FXW

ZKHQ LQVHUWLQJ

6WDUW SRVLWLRQ LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

6WDUW SRVLWLRQ LQ ; D[LV

; 3RVLWLRQ DEVROXWH RU

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-13

Description of permissible parameters; start cycle processing

Note

The cycle can be used as a drilling or cut-in cycle. If the cycle is used for drilling, the addresses

X/U and P cannot be used.

Deep-hole drilling and grooving in the transverse axis G75

5HWUDFWLRQ SDWK WR FKLS EUHDNLQJ

Figure 5-14

Description of permissible parameters; save values in GUDs

;8 =: 3 4 5 )

0DFKLQLQJ IHHGUDWH

5HWUDFWLRQ SDWK DW UHFHVV EDVH

)HHG LQ LQ WKH ORQJLWXGLQDO D[LV = D[LV WR FKLS EUHDNLQJ

)HHG LQ DPRXQW LQ WKH WUDQVYHUVH D[LV ; D[LV WR FKLS

EUHDNLQJ

6WDUW SRVLWLRQ LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

6WDUW SRVLWLRQ LQ ; D[LV

; 3RVLWLRQ DEVROXWH RU

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-15

Description of permissible parameters; start cycle processing

Note

The cycle can be used as a drilling or cut-in cycle. If the cycle is used for drilling, the addresses

Z/W and Q cannot be used.

ISO dialects

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

103

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

Multiple thread cutting cycle G76

3[[[[[[[ 4

)LQLVKLQJ DOORZDQFH

0LQLPXP LQIHHG GHSWK WKLV YDOXH PXVW QRW EH H[FHHGHG ZKHQ

IHHGLQJ LQ

$QJOH RI WRRO EODGH

6L]H RI FKDPIHU RQ WKUHDG HQG LQ

[ WKUHDG OHDG

1XPEHU RI ILQLVKLQJ FXWV

Figure 5-16

Description of permissible parameters; save values in GUDs

;8 =: 5 3 4 )

7KUHDG OHDG

6L]H RI ILUVW IHHG LQ

7KUHDG GHSWK WRWDO IHHG LQ LQ WKH ; D[LV

5DGLXV GLIIHUHQFH IRU WDSHU WKUHDG

7KUHDG HQG SRLQW LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

7KUHDG HQG SRLQW LQ WKH ; D[LV

; 3RVLWLRQ DEVROXWH RU

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-17

Description of permissible parameters; start cycle processing

Example for address P:

G76 P012055 Q4 R0.5

$QJOH RI ZRUNSLHFH EODGH

GHJUHHV

&KDPIHU RQ WKUHDG HQG

[ WKUHDG OHDG

ILQLVKLQJ FXW

ISO dialects

104

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

5.4.2

Turning cycles G77 to G79

Overview

Table 5-5

Overview of turning cycles G77 to G79

G command

Description

G77

Lengthwise stock removal

G78

Thread cutting

G79

Transverse stock removal

These cycle calls are modally effective and are called in each NC block with axial motion. The

processing movements are defined in the call parameters after the G function. The following

parameters are permitted in NC blocks with cycle calls using G77 to G79:

;

8 (QG SRVLWLRQ RI FRQWRXU LQ ; LQFU

= (QG SRVLWLRQ RI FRQWRXU LQ = DEV RU

: (QG SRVLWLRQ RI FRQWRXU LQ = LQFU

5 ,QFUHPHQWDO UDGLXV GLIIHUHQFH IRU

HQG SRVLWLRQ LQ ; IRU WDSHU WXUQLQJ

5 )RU *

* PDFKLQLQJ IHHGUDWH

)RU * WKUHDG OHDG

Figure 5-18

Parameters for cycle calls using G77 to G79

ISO dialects

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

105

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

Lengthwise stock removal G77

5 )

0DFKLQLQJ IHHGUDWH

LQFUHPHQWDO PRYHPHQW RI HQG SRVLWLRQ LQ ; D[LV IRU WDSHU

WXUQLQJ

&\OLQGHU WXUQLQJ 5 QRW SURJUDPPHG RU 5

3RVLWLRQ LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

3RVLWLRQ LQ WKH ; D[LV

; 3RVLWLRQ DEVROXWH

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-19

Description of permissible parameters; start cycle processing

Thread cutting G78

5 )

6WDUW SRLQW IRU DQJOH RIIVHW

7KUHDG OHDG

LQFUHPHQWDO PRYHPHQW RI HQG SRVLWLRQ

LQ WKH ; D[LV IRU WDSHU WXUQLQJ

&\OLQGHU WXUQLQJ 5 QRW SURJUDPPHG RU 5

3RVLWLRQ LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

3RVLWLRQ LQ WKH ; D[LV

; 3RVLWLRQ DEVROXWH

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-20

Description of permissible parameters; start cycle processing

ISO dialects

106

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

Transverse stock removal G79

5 )

0DFKLQLQJ IHHGUDWH

LQFUHPHQWDO PRYHPHQW RI HQG SRVLWLRQ

LQ WKH = D[LV IRU WDSHU WXUQLQJ

&\OLQGHU WXUQLQJ 5 QRW SURJUDPPHG RU 5

3RVLWLRQ LQ WKH = D[LV

= 3RVLWLRQ DEVROXWH

: 3RVLWLRQ LQFUHPHQWDO

3RVLWLRQ LQ WKH ; D[LV

; 3RVLWLRQ DEVROXWH

8 3RVLWLRQ LQFUHPHQWDO

Figure 5-21

Description of permissible parameters; start cycle processing

5.4.3

Drilling cycles G80 to G89

Overview

With fixed cycles for hole-machining specific movements can be programmed for machining

the drill holes, which normally require several command frames made of several single-block

commands. The program called with the fixed cycle can be deselected again with G80.

The G functions used for calling the fixed cycles G80 to G89 are the same for all G code

systems.

Table 5-6

Overview of drilling cycles

G command

Description

G80

Drilling cycle off

G83

Front face deep hole drilling

G84

Front face tapping

G85

Front face drilling

G87

Side surface deep hole drilling

G88

Side surface tapping

G89

Side surface drilling

ISO dialects

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

107

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

&\FOH FDOO IURP ,62

6LHPHQV

6KHOO F\FOH

GLDOHFW 7 PRGH

VWDQGDUG F\FOH

&<&/(

&KDQJHRYHU WR WKH

6LHPHQV PRGH

Figure 5-22

Assignment of drilling cycles to standard Siemens cycle in ISO dialect T mode using shell

cycle

5 3 4 ) . 0

$VFHUWDLQ 0 FRGH IRU & D[LV

1XPEHU RI UHSHWLWLRQV

LI QR . LV SURJUDPPHG

WKH F\FOH LV SHUIRUPHG RQFH

'ULOOHG KROH SRVLWLRQ

. F\FOH LV QRW SHUIRUPHG

0DFKLQLQJ IHHGUDWH

,QIHHG

'ZHOO WLPH DW GULOOLQJ KROH GHSWK

'LVWDQFH EHWZHHQ UHWUDFWLRQ SODQH DQG GULOOLQJ SODQH

'ULOOLQJ KROH GHSWK

Figure 5-23

Description of permissible parameters; start cycle processing

=: &+

5 3 4 ) . 0

$VFHUWDLQ 0 FRGH IRU & D[LV

1XPEHU RI UHSHWLWLRQV

LI QR . LV SURJUDPPHG

WKH F\FOH LV SHUIRUPHG RQFH

'ULOOHG KROH SRVLWLRQ

. F\FOH LV QRW SHUIRUPHG

0DFKLQLQJ IHHGUDWH

,QIHHG

'ZHOO WLPH DW GULOOLQJ KROH GHSWK

'LVWDQFH EHWZHHQ UHWUDFWLRQ SODQH DQG GULOOLQJ

SODQH

'ULOOLQJ KROH GHSWK

Figure 5-24

Description of permissible parameters; start cycle processing

ISO dialects

108

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

The drilling cycles are modally effective and are executed in every NC block in which axial

movements of axes X, C, Z are programmed. When a drilling mode is active, only the new

parameters have to be programmed if a parameter is changed. The parameters are stored in

the system variables $C_xx (xx = NC address) which are read by the cycles.

If there is a G function of the 1st G group in the same NC block after the cycle G function, the

cycle is not executed. Only the axes programmed in the NC block are traversed. Addresses R,

Q, P, K are not written to the system variables. The feedrate programmed in this block is

activated.

;

= ;

Figure 5-25

Drilling cycle

Modal cycles

All modal cycles are deselected in ISO dialect mode with G80 or with a G function of the 1st

group (G00-G03, G33, G34, apart from G77-G79).

Cycle parameters can be programmed in the following blocks while a modal cycle is active.

These parameters are written to the system variables so that the shell cycle works with the

modified parameters.

Example:

N10 G81 X10. Z15. R5 Q4 P10 F1000

N20 X50. ;drilling cycle at position X50

ISO dialects

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

109

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

5.4.4

Description of shell cycle CYCLE383T

It is called in ISO dialect T mode using the G commands G83 and G87.

Note

The direction of the basis in relation to the reference plane must be identical to the direction of

the reference plane in relation to the final depth. Otherwise the Siemens drilling cycle results in

an error message.

In ISO dialect T, the programmer must take into account the safety clearance when defining the

reference plane. For Siemens the safety clearance from the R plane can be stated separately.

This option has also been realized in ISO cycles. GUD_ZSFR[20] can be used to enter a safety

clearance if necessary. If the safety clearance has already been taken into account when

programming the R plane, "ZERO" must be entered for GUD_ZSFR[20].

GUD_ZSFR[23] is used to determine whether the dwell time (for deep-hole drilling only) is to be

undertaken in seconds or revolutions for G95.

A shell cycle may only be called by an external G code (G83/G87). Calling in Siemens mode

(after switching over with G290 and CYCLE383T call) is not permitted.

If the G83/G87 block contains axis names other than X/Z (U/W), alarm (61811) "ISO axis name

not permitted" occurs.

GUD_ZSFR[2] is used to determine whether the cycle is to be executed with chip breaking or

chip removal.

With ISO dialect, the constant individual depth is retained until the remainder at the base of the

hole is removed with an infeed. With Siemens the remainder (less than 2*individual depth) at

the base of the hole is split into two infeeds of the same size if necessary.

Note

Alarms are listed in the "Alarms" section along with alarm number and description.

ISO dialects

110

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

Cycles and contour definition

5.4 Turning and drilling cycles (ISO dialect T)

5.4.5

Description of shell cycle CYCLE384T

It is called in ISO dialect T mode using the G commands G84 and G88.

Note

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth. Otherwise the Siemens drilling cycle results in an error

message. ISO dialect has no monitoring here.

In ISO dialect T, the programmer must take into account the safety clearance when defining the

datum plane. For Siemens the safety clearance from the R plane can be stated separately.

This option has also been realized in ISO cycles. GUD_ZSFR[20] can be used to enter a safety

clearance if necessary. If the safety clearance has already been taken into account when

programming the R plane, "ZERO" must be entered for GUD_ZSFR[20].

A shell cycle may only be called by an external G code (G84/G88). Calling in Siemens mode

(after switching over with G290 and CYCLE384T call) is not permitted.

If the G84/G88 block contains axis names other than X/Z (U/W), alarm (61811) "ISO axis name

not permitted" occurs.

GUD_ZSFI[22] (value as %) can be used to influence the speed of drilling when retracting.

Example: ZSFI[22]=95 Retraction takes place at 95% of the hole depth.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

ISO dialects

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

111

Cycles and contour definition

5.5 System variables

5.4.6

Description of shell cycle CYCLE385T

It is called in ISO dialect T mode using the G commands G85 and G89.

Note

The direction of the basis in relation to the datum plane must be identical to the direction of the

datum plane in relation to the final depth. Otherwise the Siemens drilling cycle results in an error

message. ISO dialect has no monitoring here.

In ISO dialect T, the programmer must take into account the safety clearance when defining the

datum plane. For Siemens the safety clearance from the R plane can be stated separately.

This option has also been realized in ISO cycles. GUD_ZSFR[20] can be used to enter a safety

clearance if necessary. If the safety clearance has already been taken into account when

programming the R plane, "ZERO" must be entered for GUD_ZSFR[20].

A shell cycle may only be called by an external G code (G85/G89). Calling in Siemens mode

(after switching over with G290 and CYCLE385T call) is not permitted.

If the G85/89 block contains axis names other than X/Z (U/W), alarm (61811) "ISO axis name

not permitted" occurs.

If the G84 block contains axis names other than X/Z (U/W), alarm (61811) "ISO axis name not

permitted" occurs.

Note

Alarms are listed in the "Alarms" chap. along with alarm number and description.

5.5

System variables

The names of the system variables all start with $C_ xx. The NC address, the value of which is

stored in the system variables, can be found in the name extension xx. Variable $C_G always

contains the G number with which a cycle has been called.

Bit 0 is set in the $C_x_PROG system variables for all programmed addresses if the address

is programmed.

Bit 1 is also set in the $C_x_PROG variables for axis addresses programmed incrementally.

For end of subprogram with RET, $C_x_PROG is set to FALSE, for end of subprogram with

M17, the values in $C_x_PROG are retained.

Example 1:

N10 G01 G81 X100. Z-50. R20 F100

Shell cycle CYCLE381M for G81 is called automatically. The calculations are carried out in the

shell cycle and the standard Siemens cycle CYCLE82 then called. The G01 command is not

needed.

The values of the programmed addresses are written to the system variables:

ISO dialects

112

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

Cycles and contour definition

5.5 System variables

Address X is written to system variable $C_X;

Address Z is written to system variable $C_Z;

Address R is written to system variable $C_R;

Address F is written to system variable $C_F;

Example 2:

Axis Z is programmed in an incremental manner (G91) → $C_Z_PROG =3

Axis Z is programmed in an absolute manner (G90) → $C_Z_PROG =1

Example 3: Siemens shell cycle for Gxy

N10 PROC CYCLE377 DISPLOF

;Block display remains G77 block,

;Freeze G code display

N20 DEF REAL DELTA_X, pos_X, pos_Z, FEEDRATE

N30 DEF BOOL R_prog, X_prog, Z_prog

N50 DELTA_X = 0

N60 IF $C_R_PROG

;Only load DELTA_X if

N70 DELTA_X = $C_R

;address R has been programmed

N75 ENDIF

N110 CYCLE...(DELTA_X, $C_X, $C_Z,

;Call Siemens cycle

$C_R_PROG, $C_X_PROG, $C_Z_PROG, $C_F)

N230 RET

;Shell cycle end

Table 5-7

List and description of system variables

Identifier

Type

Description

$C_A

REAL

Value of programmed address A in ISO dialect mode for cycle pro-

gramming

$C_B

REAL

Value of programmed address B in ISO-dialect-mode for cycle pro-

gramming

$C_G

INT

G number for cycle calls in external mode

$C_H

REAL

Value of programmed address H in ISO dialect mode for cycle pro-

gramming

$C_I[ ]

REAL

Value of the programmed Address I in ISO dialect mode for cycle pro-

gramming and macro technology with G65/G66. A max. of 10 entries is

possible in the block for the macro programming. The values remain in

the programmed sequence in the array.

$C_I_ORDER[ ]

REAL

For description, refer to $C_I[ ], defines the programming sequence

$C_J[ ]

REAL

For description refer to $C_I[ ]

$C_J_ORDER[ ]

REAL

For description, refer to $C_I[ ], defines the programming sequence

$C_K[ ]

REAL

For description refer to $C_I[ ]

$C_K_ORDER[ ]

REAL

For description, refer to $C_I[ ], defines the programming sequence

$C_L

REAL

Value of programmed address L in ISO dialect mode for cycle pro-

gramming

$C_Z

REAL

Value of programmed address Z in ISO dialect mode for cycle pro-

gramming

ISO dialects

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

113

Cycles and contour definition

5.5 System variables

Identifier

Type

Description

$C_TS

STRING

String of tool identifier programmed under the address T

$C_A_PROG

INT

Address A is programmed in a block with cycle call.

0 = Not programmed

1 = Programmed (absolute)

3 = Programmed (incremental)

$C_B_PROG

INT

Address B is programmed in a block with cycle call.

0 = Not programmed

1 = Programmed (absolute)

3 = Programmed (incremental)

$C_G_PROG

INT

The shell cycle is programmed over a G function

$C_Z_PROG

INT

Address Z is programmed in a block with cycle call.

0 = Not programmed

1 = Programmed (absolute)

3 = Programmed (incremental)

$C_TS_PROG

INT

A tool identifier was programmed under address T

TRUE = programmed; FALSE = not programmed

$C_ALL_PROG

INT

Bit pattern of all programmed addresses in a block with cycle call

Bit 0 = Address A

Bit 25 = Address Z

Bit = 1 address is programmed

Bit = 0 address is not programmed

$P_EXTGG[n]

INT

Active G code of the external language

$C_INC_PROG

INT

Bit pattern of all incrementally programmed addresses in a block with

cycle call

Bit 0 = Address A

Bit 25 = Address Z

Bit = 1 address is programmed incrementally

Bit = 0 address is not programmed as absolute

$C_I_NUM

INT

Cycle programming: Value is always 1 if bit 0 is set in $C_I_PROG.

Macro programming: Number of address I programmed in the block

(max. 10).

$C_J_NUM

INT

For description refer to $C_I_NUM

$C_K_NUM

INT

For description refer to $C_I_NUM

$P_AP

INT

Polar coordinates 0=OFF 1=ON

$C_TYP_PROG

INT

Bit pattern of all programmed addresses in a block with cycle call

Bit 0 = A

Bit 25 = Z

Bit = 0 Axis is programmed as INT

Bit = 1 Axis is programmed as REAL

$C_PI

INT

Program number of the interrupt routine that was programmed with

M96

ISO dialects

114

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

Cycles and contour definition

5.6 Programming contour definitions

5.6

Programming contour definitions

Overview

Contour definitions can be programmed in both ISO dialect mode and Siemens mode.

There are three basic forms of contour definitions:

● One straight line

End point is programmed with a Cartesian coordinate and an angle

● Two straight lines

Transition with a curve or chamfer

● Three straight lines

Transitions with a curve or chamfer

In the descriptions that follow, the address letters X, Z, A, R and C sometimes have indices to

allow for clear assignment between NC block and the associated drawing. These indices do not

appear in the NC program. The assignment always clearly results from the block containing an

address letter. Address letter Q is a filler at places where either R or C may occur. Q may also

not be used. In such cases, no chamfer or curve is inserted at the transition of the two straight

lines.

Any other NC addresses can be used, e.g. address letters for other axes (single axes or axis

perpendicular to the machining plane), auxiliary function specifications, G codes, velocities,

etc. in the blocks that describe contour definitions.

It is assumed that G18 is active in the following examples. However, the programming of

contour definitions is also possible without restrictions with G17 or G19.

ISO dialect mode

Address A is used in ISO dialect mode as both an axis identifier and as an identifier for an angle

in the contour definition. To distinguish between the possibilities, a "," must be set before the

address when programming the contour definition.

Address C is used in ISO dialect mode as both an axis identifier and as an identifier for a

chamfer in the contour definition.

Address R can either be a cycle parameter or an identifier for the radius in a contour definition.

To distinguish between the two possibilities, a "," must be set before address C or R when

programming the contour definition. If an angle is programmed before C or R, a comma does

not have to be programmed before it. If radius and chamfer are programmed together in a block,

e.g. N333 X100 A10 C20 R15, regardless of the programming sequence a radius is always

inserted in the contour. The chamfer is ignored.

ISO dialects

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

115

Cycles and contour definition

5.6 Programming contour definitions

Siemens mode

In Siemens mode, the identifiers for angle, radius and chamfer are defined via machine data.

This avoids name conflicts. A comma must not be programmed before the identifier for radius

or chamfer.

Note

MD10652 for angle: $MN_CONTOUR_DEF_ANGLE_NAME

MD10654 for radius: $MN_RADIUS_NAME

MD10656 for chamfer: $MN_CHAMFER_NAME

5.6.1

End point programming with angles

If the address letter A appears in an NC block, either none, one or both of the axes in the active

plane may also be programmed.

If no axis of the active plane has been programmed, then this is either the first or second block

of a contour definition consisting of two blocks. If this is the second block of such a contour

definition, the start and end point in the active plane are identical. The contour definition then

consists only of a motion perpendicular to the active plane.

If exactly one axis of the active plane has been programmed, then this is either a single straight

line whose end point can be clearly defined via the angle and programmed Cartesian

coordinate or the second block of a contour definition consisting of two blocks. In the second

case, the missing coordinate is set to the same as the last (modal) position reached.

If two axes of the active plane have been programmed, then this is the second block of a

contour definition consisting of two blocks. If the current block has not been preceded by a block

with angle programming without programmed axes of the active plane, then this block is not

permitted.

Angle A may only be programmed for linear or spline interpolation. (Spline interpolation in

Siemens mode only.)

Alarms are generated in the following cases:

● With a contour definition consisting of two blocks, at the transition to the second block, the

active plane is changed.

● With the angles programmed, a valid intermediate point cannot be formed for a contour

definition consisting of two straight lines.

● In a block with address A, neither linear nor spline interpolation is active.

● A block with address A without a programmed axis in the active plane is not followed by a

block which can be used to determine the end point of the contour definition. This is the case

if this block is the last in a program or if the following block contains a preprocessing stop.

● No angle has been programmed in the second block of a contour definition consisting of two

straight lines.

● Both axes of the active plane are programmed in a block with address A, which is not the

second block of a contour definition consisting of two straight lines.

● Programmed Cartesian coordinates and programmed angles are incompatible.

ISO dialects

116

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

Cycles and contour definition

5.6 Programming contour definitions

5.6.2

Straight line with angle

The end point is defined by stating angle A and one of the two coordinates X₂ or Z₂.

Programming syntax:

X₂.. ,A.. or

Z₂.. ,A..

;

Figure 5-26

Straight line with angle

;

GHJUHHV

;

Figure 5-27

Straight line with angle

Example (previous figure):

Programming in ISO dialect T mode:

N10 G1 X5. Z70. F1000 G18

N20 X88.8 ,A110 or (Z39.5 ,A110)

Programming in Siemens mode:

ISO dialects

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

117

Cycles and contour definition

5.6 Programming contour definitions

N10 X5. Z70. F1000 G18

N20 X88.8 ANG=110 or (Z39.5 ANG=110)

5.6.3

Two straight lines

The end point of the first straight line can be programmed by specifying the Cartesian

coordinates or by specifying the angle of the two straight lines relative to the x coordinate.

Programming syntax:

N10 ,A1.. (Q..)

N20 X3.. Z3.. ,A2..

N10 X1.. Z1.. (Q..)

N20 X3.. Z3..

;

Figure 5-28

Two straight lines

ISO dialects

118

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

Cycles and contour definition

5.6 Programming contour definitions

;

GHJUHHV

&KDPIHU

;

GHJUHHV

;

Figure 5-29

Two straight lines

Example (previous figure):

Programming in the ISO dialect mode:

N10 G1 X10. Z80. F1000 G18

N20 ,A148.64 C55

N30 X85. Z40. ,A100

Programming in Siemens mode:

N10 X10. Z80. F1000 G18

N20 ANG=148.65 CHR=5.5

N30 X85. Z40. ANG=100

5.6.4

Three straight lines

The end point of the third straight line must always be programmed with Cartesian coordinates.

The transition from the second to the third coordinate can either take the form of a chamfer or

radius.

This type of programming can be continued for any number of blocks, i.e. a distinction does not

have to be made between contour definitions with two or more blocks.

Programming syntax:

N10 X2.. Z2.. (Q1..)

N20 X3.. Z3.. (Q2..)

N30 X4.. Z4..

ISO dialects

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

119

Cycles and contour definition

5.6 Programming contour definitions

Programming in the ISO dialect mode:

N10 G1 X10. Z100. F1000 G18

N20 ,A140 C7.5

N30 X80. Z70. ,A95.824, R10

Programming in Siemens mode:

N10 X10. Z100. F1000 G18

N20 ANG=140 CHR=7,5

N30 X80. Z70. ANG=95.824 RND=10

N40 X70 Z50

5.6.5

Multi-edge turning with G51.2

Function

Does not function in SINUMERIK 802D sl.

With the G51.2 function, workpieces with multiple edges can be produced by coupling two

spindles. This corresponds to the synchronous spindle function in Siemens mode with a

transformation ratio other than 1 : 1.

With the programming syntax G51.2 Q.. P.. R.. the synchronous spindle coupling is activated.

The transformation ratio from leading spindle to the following spindle is defined with the

parameters "Q" and "P". If the coupling is to be activated with an angular offset from following

spindle and leading axis, the angular difference is programmed with the address "R".

When mapping the function to Siemens language, in order to activate the synchronous spindle

function, two part program commands must always be issued - these must not occur in the

same block.

The assignment of leading and following spindle and the transformation ratio (and type of

coupling) are defined with a part program command (COUPDEF(..)). The second part program

command activates the coupling with the angle offset programmed (COUPON(..)). To execute

the two program commands, a cycle is called with G51.2 (CYCLE3512). The programmed

values are transferred to cycle parameters $C_P, $C_Q and $C_R. G50.2 is used to deactivate

the coupling again (also with CYCLE3512).

With the programming of G51.2, the 1st spindle in the channel is always defined as the leading

spindle and the 2nd spindle as the following spindle. Setpoint linkage is selected as the type of

coupling.

Example

N10 T1234

N20 G0 X10 Z100 M3 S1000

N30 G51.2 P1 Q3

;start synchronous spindle with transforma-

tion ratio 1 : 3

;and angle offset of 0 degrees

Nxx

ISO dialects

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

121

Cycles and contour definition

5.6 Programming contour definitions

N1000 G51.2 R180

;angle offset between leading and

;following spindle of 180 degrees

N1200 G50.2

;switch off synchronous spindle operation

N2000 M30

For a detailed description of the synchronous spindle function, see

Function Manual for extended functions, chapter M1 and

Programming Manual for preparing for work, chapter "Synchronous spindle".

5.6.6

Contour repetition G72.1/G72.2

Function

G72.x is used to call a subprogram programmed under address P... The number of subprogram

repetitions is defined with address L. If address L is not programmed, the subprogram is

executed once. Depending on the G code, a coordinate rotation is executed (G72.1) or an

incremental distance traversed, relative to the contour's start point, before every subprogram

call (G72.2).

G72.1

G72.1 is used to call a subprogram (in which the contour to be repeated is programmed) several

times. The coordinate system is rotated by a certain angle before each subprogram call.

This function is realized by calling a cycle (CYCLE3721). The programmed values in cycle

parameters $C_.. are transferred to the cycle. The G function number can be found in $C_G,

a value of 721 is entered for G72.1 and 722 for G72.2 in $C_G. The cycle carries out the

coordinate rotation n times and calls the subprogram n times. The coordinate rotation is

executed around a vertical axis on the selected plane.

X.. Y.. (Z..)

Reference point for coordinate rotation

P..

Subprogram number

L..

Number of subprogram repeats

R..

Angle of rotation

Example:

ISO dialects

122

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

Cycles and contour definition

5.6 Programming contour definitions

6WDUW SRLQW

;

Figure 5-32

Contour repetition with G72.1

Main program

N10 G92 X40.0 Y50.0 ;

N20 G01 G90 G17 G41 20 Y20 D01 F1000

N30 G72.1 P1234 L4 X0 Y0 R90.0

N40 G40 G01 X100 Y50 Z0

N50 G00 X40.0 Y50.0 ;

N60 M30 ;

Subprogram 1234.spf

N100 G01 X10

N200 Y50

N300 X-10

N400 Y10

N500 X-20

N600 M99

G72.2

G72.2 is used to call a subprogram (in which the contour to be repeated is programmed) several

times. The axes programmed with I, J and K are traversed incrementally before each

subprogram call. In CYCLE3721 the programmed G function recognizes whether the contour

subprogram is repeated after a rotation or a linear movement.

This function is realized by calling a cycle. The programmed values in cycle parameters $C_..

are transferred to the cycle. The cycle calls the subprogram n times. A distance programmed

ISO dialects

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

123

Cycles and contour definition

5.6 Programming contour definitions

under I, J, K is traversed incrementally (calculated from the start point) before each subprogram

call.

I.. J.. K..

Position to which the X, Y Z axes are traversed before calling the

subprogram. The position relates to the start point of the subprogram.

P..

Subprogram number

L..

Number of subprogram repeats

Example:

6WDUW SRLQW

;

Figure 5-33

Contour repetition with G72.2

N10 G00 G90 X0 Y0

N20 G01 G17 G41 X30. Y0 D01 F1000

N30 Y10.

N40 X30.

N50 G72.2 P2000 L3 I80. J0

O2000 G90 G01 X40.

N100 Y30.

N200 G01 X80.

N300 G01 Y10.

N400 X90.

N500 M99

5.6.7

Output on an external device / an external file

Function

With the "Process DataShare" function, it is possible to write data from a part program to an

external device or an external file; for instance, e.g. to log production data or to control

additional equipment on a control system.

ISO dialects

124

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

Cycles and contour definition

5.6 Programming contour definitions

The part program commands ISOOPEN, ISOPRINT and ISOCLOSE are provided for output on

an external device in the ISO language mode. These commands are parameterized via the

NCK machine data 10830 $MN_EXTERN_PRINT_DEVICE and 10831

$MN_EXTERN_PRINT_MODE.

The ISOOPEN, ISOPRINT and ISOCLOSE commands listed here may only be on their own in

a program block - apart from the block number, skip identifier and comment.

In ISO mode, precisely one device can be used for the output across all channels.

ISOPEN (open output device)

The output device referenced with MD $MN_EXTERN_PRINT_DEVICE is opened. MD

$MN_EXTERN_PRINT_MODE bit 0 can be used to set whether the output is to be synchronous

(FALSE) or asynchronous (TRUE), and $MN_EXTERN_PRINT_MODE bit 1 (FALSE) used to

set whether the output device is to be assigned exclusively.

If MD $MN_EXTERN_PRINT_MODE bit 2 is set, the control character DC2 (H12) is output with

ISOOPEN.

MD $MN_EXTERN_PRINT_MODE bits 4 and 5 can be used to determine whether the output

is to be terminated with LF or CR+LF.

Alarm 14066 "Error during output on an external device" is issued when an error occurs and the

part program execution is aborted. The error cause is specified in the alarm parameter "error

code".

ISOPRINT (output on an external device)

Syntax:

ISOPRINT[<Format string>, <Value list>]

<Format string> Character string that contains fixed and variable parts. The variable parts

are specified by the format statement %P.

Each %P is assigned a value from the <Value list>

●

%.nP: Output of a binary value with n decimal places

Example: ISOPRINT("X%.3P", 123.456)

● %m.nP: Output of a decimal number with m places before the decimal

point and n decimal places.

Example: ISOPRINT("X%5.3P", 123.456)

The <Format string> must only include format operations of one type (%.nP

or %m.nP). The "*" character is converted to a blank.

The start and end of the format string is identified by a ".

Example: "Measured value part 1: %3.2P"

List of the values to be output in the form of REAL constants. The individual

values are separated by commas. The value list can contain a maximum of

ten values.

The prepared string is output on the output device previously opened with ISOOPEN. The

output is terminated with LF or CR+LF depending on the setting of MD

$MN_EXTERN_PRINT_MODE, bits 4 and 5.

ISO dialects

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

125

Cycles and contour definition

5.6 Programming contour definitions

Alarm 14066 "Error during output on an external device" is issued when an error occurs during

the output and the part program execution is aborted. The error cause is specified in the alarm

parameter "error code".

ISOCLOSE (close output device)

The output device opened with ISOOPEN is closed. If MD $MN_EXTERN_PRINT_MODE bit

3 is set, the control character DC4 (H14) is output with ISOCLOSE.

5.6.8

Convex thread with G35 and G36

In ISO dialect T, convex threads are programmed with G codes G35 in the clockwise direction

and G36 in the counter-clockwise direction.

These G codes are available for the G code systems A, B and C. The arc can be programmed

with specification of the circle center point via the circle parameters I, J, K or via specification

of the radius R. Optionally, a thread starting point offset can be specified with Q. If R is

programmed together with I, J, K, only R is effective.

Programming:

X.. Y.. Z.. I.. J.. K.. R.. F.. Q..

X Y Z

End point of the arc

I J K

Coordinates for circle center point programming

Radius for radius programming

Lead in the direction of the main axis

Thread starting point offset (optional)

Convex threads are described in detail in SINUMERIK 840D sl / 828D Fundamentals

Programming Manual, Section 9 "Motion commands".

ISO dialects

126

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

Commissioning

6.1

Machine data

Activating ISO dialect mode

MD18800 $MN_MM_EXTERN_LANGUAGE

Selection of ISO dialect M or T

MD 10880 $MN_MM_EXTERN_CNC_SYSTEM=1: ISO dialect M

MD 10880 $MN_MM_EXTERN_CNC_SYSTEM=2: ISO dialect T

ISO dialect T axis names

The maximum number of axes is eight. The axis identifiers of the first two axes are fixed X, Z.

Possible axis identifiers for the other axes are Y, A, B, C, U, V, W.

If G code system A is active (there is then no G91), incremental values are programmed for X,

Z, Y with U, V, W. U, V, W cannot then be used as axis identifiers, a maximum of six axes are

possible. H is used to incrementally traverse the C axis.

If B is not used as an axis identifier, B can be used as an extended auxiliary function. B is then

output as auxiliary function H with address extension 1 (H1=).

Contour definition:

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 0 is used to define the programming for the

contour definition.

0: Contour definition is programmed with ,C ,R ,A (with commas). C and A can be axis

identifiers.

1: Contour definition is programmed with C R A (without commas). C and A cannot be axis

identifiers.

ISO dialect M axis names

The maximum number of axes is eight. The axis identifiers of the first three axes are fixed X, Y,

Z. Possible axis names for the other axes are A, B, C, U, V, W.

If B is not an auxiliary function, B can be used as an axis identifier.

Axis interpolation

All programmable axes interpolate with one another as standard with ISO dialect.

This corresponds to FGROUP with ISO dialect M: X, Y, Z (A, B, C, U, V, W).

This corresponds to FGROUP with ISO dialect T: X, Z, Y (C).

ISO dialects

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

127

Commissioning

6.1 Machine data

MD22420 $MC_FGROUP_DEFAULT_AXES[0] is used to achieve this behavior if the machine

has four axes:

$MC_FGROUP_DEFAULT_AXES[0] = 1

$MC_FGROUP_DEFAULT_AXES[1] = 2

$MC_FGROUP_DEFAULT_AXES[2] = 3

$MC_FGROUP_DEFAULT_AXES[3] = 4

Work offset (ISO dialect M only)

If only NVs G54 to G59 are used, MD28080 $MC_MM_NUM_USER_FRAMES or with global

frames MD18601 $MC_MM_NUM_GLOBAL_USER_FRAMES >= 7 must be set.

If G54 is to be active after a reset, the following MD must be set to 1:

MD20154 $MC_EXTERN_GCODE_RESET_VALUES[13]

MD20150 $MC_GCODE_RESET_VALUES[7]

If the extended work offsets G54 P1 to P48 are used, MD28080

$MC_MM_NUM_USER_FRAMES or with global frames MD18601

$MC_MM_NUM_GLOBAL_USER_FRAMES >= 55 must be set.

If the following MD is set to 7, after a reset, G54 P1 is active:

MD 20154 $MC_EXTERN_GCODE_RESET_VALUES[13]

MD 20150 $MC_GCODE_RESET_VALUES[7]

G54 P1 is mapped to Siemens G507.

If an activated work offset is not to be retracted with G91, the following setting data should be

set to 0:

SD 42440 $SC_FRAME_OFFSET_INCR_PROG

Suppress tool lengths and radius compensation with G53:

MD 10760 $MN_G53_TOOLCORR = 1

Metric/Inch switchover

The handwheel evaluation and increment evaluation are not switched over with G20 and G21.

This switchover must be performed from the PLC: See MD31090 $MA_JOG_INCR_WEIGHT.

In ISO dialect mode, the work offsets are converted during the switchover. With ISO dialect

original, the comma is simply moved.

Programming diameter or radius

When MD20150 $MC_GCODE_RESET_VALUES[28] = 2, diameter programming is activated

for the transverse axis.

Decimal point programming

MD10884 $MN_EXTERN_FLOATINGPOINT_PROG is used to chose between Standard

Notation and PocketcalculatorNotation.

Input resolution IS-B and IS-C is selected with MD10886

$MN_EXTERN_INCREMENT_SYSTEM.

ISO dialects

128

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

Commissioning

6.1 Machine data

Note that MD10200 $MN_INT_INCR_PER_MM and 10210 $MN_INT_INCR_PER_DEG are at

least set such that input resolution IS-B or IS-C can be allocated.

If this is not the case, the programmed values are rounded.

Example: IS-C mm $MN_INT_INCR_PER_MM = 10000.

Scaling

MD22910 $MC_WEIGHTING_FACTOR_FOR_SCALE=0: 0,001

MD22910 $MC_WEIGHTING_FACTOR_FOR_SCALE=1: 0,00001

Axial scaling factor: MD43120 $MA_DEFAULT_SCALE_FACTOR_AXIS

Scaling factor P: MD42140 $MC_DEFAULT_SCALE_FACTOR_P

Enable axial scaling: MD22914 $MC_AXES_SCALE_ENABLE = 1 (when = 0, axial scaling is

not possible)

Position in machine coordinate system G53

The axial speed for positioning with G53 and with G00 without interpolation is defined in

MD32060 $MA_POS_AX_VELO.

With G53 X.. Y... , a position in the machine coordinate system is approached. The axes don't

interpolate with one another, instead each axis moves to the programmed position separately

at maximum speed.

Incremental positions are skipped in the G53 block. While tool radius compensation or tool

length compensation is active (G41/G42, G43/G44), the axes are not traversed independently

of one another, the axes are interpolated with one another.

Setting actual value G92

Delete the G92 movement at PowerOn:

MD24004 $MC_CHBFRAME_POWERON_MASK=1

G92 is retained during a reset (M30, channel reset):

MD20110 $MC_RESET_MODE_MASK bit 0 and bit 14=1

Resetting the tool coordinate system G92.1

With G92.1 X.. (G code system A: G50.3 P0), a moved coordinate system can be reset before

being moved. The tool coordinate system is reset to the coordinate system that is defined by

the active adjustable work offsets (G54-G59). The tool coordinate system is set to the reference

position if no adjustable work offset is active. G92.1 resets shifts carried out through G92 or

G52. However, only the axes that are programmed, are reset.

Example 1:

N10 G0 X100 Y100

;Display: WCS: X100 Y100 MCS: X100 Y100

N20 G92 X10 Y10

;Display: WCS: X10 Y10

MCS: X100 Y100

ISO dialects

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

129

Commissioning

6.1 Machine data

N30 G0 X50 Y50

;Display: WCS: X50 Y50

MCS: X140 Y140

N40 G92.1 X0 Y0

;Display: WCS: X140 Y140

MCS: X140 Y140

Example 2:

N10 G10 L2 P1 X10 Y10

N20 G0 X100 Y100

;Display: WCS: X100 Y100 MCS: X100 Y100

N30 G54 X100 Y100

;Display: WCS: X100 Y100 MCS: X110 Y110

N40 G92 X50 Y50

;Display: WCS: X50 Y50

MCS: X110 Y110

N50 G0 X100 Y100

;Display: WCS: X100 Y100

MCS: X160 Y160

N60 G92.1 X0 Y0

;Display: WCS: X150 Y150

MCS: X160 Y160

Delete distance-to-go

With ISO dialect original, G31 can be used to delete the distance-to-go. The distance-to-go is

only deleted in this block if the PLC signal is in place for the channel. Without G31, the signal

is not evaluated.

In ISO dialect mode, the PLC signals are evaluated in each block regardless of G31. G31 is

used to activate probe 1.

With ISO dialect, the deleted distance-to-go can be calculated using PLC Varselector.

The function G31 P1 (.. P4) is different from G31 in that different inputs for the measuring signal

can be selected with P1-P4. Several inputs can also be monitored on a rising edge of a

measuring signal simultaneously. The assignment of the inputs to the addresses P1 to P4 is

defined by the following machine data.

MD10810 $MN_EXTERN_MEAS_G31_P_SIGNAL[0 .. 3].

Note

Only two measuring inputs are available for the 840D sl.

Spindle position

The spindle position for M19 is set using setting data 43240 $SC_M19_SPOS.

Protection zone

If G commands G22 and G23 are used, there must be a protection zone:

MD18190 $MM_NUM_PROTECT_AREA_NCK = 1

MD28210 $MC_NUM_PROTECT_AREA_ACTIVE = 1

Auxiliary function output

If value H is to be output to the PLC as an integer value, MD22110 $MC_AUXFU_H_TYPE_INT

must be set to 1.

ISO dialects

130

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

Commissioning

6.1 Machine data

The time at which the auxiliary function is output (M, S, T, H) to the PLC can be set using

machine data:

0 = Auxiliary function output before motion

1 = Auxiliary function output during motion

2 = Auxiliary function output after motion

3 = Motion is not output to PLC

MD22200 $MC_AUXFU_M_SYNC_TYPE for M functions

MD22210 $MC_AUXFU_S_SYNC_TYPE for S functions

MD22220 $MC_AUXFU_T_SYNC_TYPE for T functions

MD22230 $MC_AUXFU_H_SYNC_TYPE for H functions

Approach 1st reference point G28

The following machine data must be set:

●

20050 $MC_AXCONF_GEOAX_ASSIGN_TAB[0-2]

Axis 1 to 3

●

20060 $MC_AXCONF_GEOAX_NAME_TAB[0-2]

Axis names for milling: X, Y, Z

Axis names for turning: X, Z, Y

●

200070 $MC_AXCONF_MACHAX_USED[0-3]

Axis 1 to 4

●

20080 $MC_AXCONF_CHANAX_NAME_TAB[0-3]

4th axis name for milling: X, Y, Z are permanently assigned; A, B, C, U, V or W can also be

selected.

4th axis name for turning: X, Z, Y are permanently assigned; C can also be selected

●

20100 $MC_DIAMETER_AX_DEF

Only when turning: X axis

●

20150 $MC_GCODE_RESET_VALUES[28]

Radius or diameter programming

1 = DIAMOF (radius for G90/G91)

2 = DIAMON (diameter for G90/G91)

3 = DIAM90 (diameter for G90, radius for G91)

Note: DIAM90 is treated like DIAMON within the cycle.

●

34100 $MA_REFP_SET_POS[0]

0 = 1st reference point

Enter a value for each axis

●

35000 $MA_SPIND_ASSIGN_TO_MACHAX

0 = Axis is not spindle

1 = Axis is a spindle

ISO dialects

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

131

Commissioning

6.1 Machine data

Approach 2nd/3rd/4th reference point G30

The following machine data must be set:

●

20050 $MC_AXCONF_GEOAX_ASSIGN_TAB[0-2]

Axis 1 to 3

●

20060 $MC_AXCONF_GEOAX_NAME_TAB[0-2]

Axis names for milling: X, Y, Z

Axis names for turning: X, Z, Y

●

20070 $MC_AXCONF_MACHAX_USED[0-3]

Axis 1 to 4

●

20080 $MC_AXCONF_CHANAX_NAME_TAB[0-3]

4th axis name for milling: X, Y, Z are permanently assigned; A, B, C, U, V or W can also be

selected.

4th axis name for turning: X, Z, Y are permanently assigned; C can also be selected

●

20100 $MC_DIAMETER_AX_DEF

Only when turning: X axis

●

20150 $MC_GCODE_RESET_VALUES[28]

Radius or diameter programming

1 = DIAMOF (radius for G90/G91)

2 = DIAMON (diameter for G90/G91)

3 = DIAM90 (diameter for G90, radius for G91)

Note: DIAM90 is treated like DIAMON within the cycle.

●

34100 $MA_REFP_SET_POS[1,2,3]

1,2,3 = 2nd, 3rd, 4th reference point

Enter a value for each axis

●

35000 $MA_SPIND_ASSIGN_TO_MACHAX

0 = Axis is not spindle

1 = Axis is a spindle

G30.1 reference point position

Reference point approach is realized in the CYCLE328 cycle. The reference point position is

written in setting data 43340 $SC_EXTERN_REF_POSITION_G30_1.

6.1.1

Active G command for PLC

The user can use MD22512 $MC_EXTERN_GCODE_GROUPS_TO_PLC to select the G

groups of an external language whose active G command is to be reported to the PLC.

$MC_EXTERN_GCODE_GROUPS_TO_PLC[0..7]=0

6.1.2

Tool change, tool data

No cutting edge is selected during a tool change.

MD20270 $MC_CUTTING_EDGE_DEFAULT = 0

ISO dialects

132

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

Commissioning

6.1 Machine data

Setting datum: During a tool change, with G91 the compensation is not retracted

SD42442 $SC_TOOL_OFFSET_INCR_PROG = 0

The assignment of tool length compensation to geometry axes is fixed:

Length 1: Z

Length 2: Y

Length 3: X

SD42940 $SC_TOOL_LENGTH_CONST =17

Effectiveness of tool length compensation beyond reset:

MD20110 $MC_RESET_MODE_MASK = 'B1000000'

Effectiveness of tool compensation with programming of T/H/D, not with M6

MD22550 $MC_TOOL_CHANGE_MODE = 0

6.1.3

G00 always with exact stop

At high speeds, collisions may occur during active continuous-path mode in G00 mode when

smoothing. MD20734 $MC_EXTERN_FUNCTION_MASK, bit 4 is used to determine the exact

stop behavior with G00.

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 4=0, G00 is traversed with the exact stop

function currently active. If G64 is active, the G00 blocks are also traversed with G64.

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 4=1, each G00 block with traversing is

traversed with G09 (non-modal exact stop). Even if G64 is active, the non-modal exact stop

takes effect in every G00 block.

6.1.4

Response to syntax faults

Response to faults occurring

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 3 is used to determine the response to faults

occurring in the first part of the ISO Translator. Here the entire ASCII block is examined.

If bit 3==0, an NC alarm is output and processing is stopped if unknown addresses are found.

If bit 3==1, no alarm is output, the ASCII block is forwarded to the Siemens Translator. The NC

block following this is first given back to the ISO Translator and an attempt is made in the

Siemens Translator to translate the ASCII block.

This allows unique Siemens blocks to be programmed without using G290 to switch to Siemens

mode while ISO mode is active.

The current ISO G code is displayed in the G code window, a switch is not made to Siemens

mode.

If a G function, which can be translated directly to an ISO G code, is activated in such a block

in the Siemens Translator, the G codes are updated here.

ISO dialects

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

133

Commissioning

6.1 Machine data

Example

20734 $MC_EXTERN_FUNCTION_MASK, bit 3==0

N5 G291

;ISO mode

N10 WAIT

;Alarm 12080 "WAIT unknown"

N15 G91 G500

;Alarm 12080 "G500 unknown"

20734 $MC_EXTERN_FUNCTION_MASK, bit 3==1

N5 G291

;ISO mode

N10 WAIT

;block is processed by the Siemens Translator

N15 G91 G500

;block is processed by the Siemens Translator

N20 X Y

;because of G291, block is processed by ISO Transla-

tor,

;G91 from N15 is active

Note

Unwanted responses may result from incorrect programming in ISO mode.

Example for ISO M:

To be programmed: G90 G76 ;modal cycle call

but the following is entered: G90 G75

G75 is not available in ISO M mode, the block goes to the Siemens Translator and results in

"Move to fixed point" without any query or alarm G75.

6.1.5

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

Function

In ISO dialect-T, a differentiation is made between G code system A, B and C. By default, the

G code system B is active.

Code system A, B or C is selected in MD10881 $MN_MM_EXTERN_GCODE_SYSTEM. The

"Rename G codes" function is not used by this function, the user can use this function without

any limitations.

As previously, switching over with a cycle is still possible.

$MN_MM_EXTERN_CNC_SYSTEM = 1: ISO dialect M

$MN_MM_EXTERN_CNC_SYSTEM = 2: ISO dialect T

$MN_MM_EXTERN_GCODE_SYSTEM = 0: G code system B

$MN_MM_EXTERN_GCODE_SYSTEM = 1: G code system A

$MN_MM_EXTERN_GCODE_SYSTEM = 2: G code system C

ISO dialects

134

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

Commissioning

6.1 Machine data

In order for the shell cycle to work in the correct G code system, the corresponding system must

be entered in the GUD variable _ZSFI[39]:

_ZSFI[39]: Setting datum for G code system with ISO T

0 = G code system B

1 = G code system A

2 = G code system B

3 = G code system C

Inch/metric changeover

With ISO dialect original there is a MD which is used to determine how the inch/metric

changeover is programmed, either with G20/21 or G70/71. This MD does not exist for ISO

dialect mode, it can also not be selected using $MN_MM_EXTERN_GCODE_SYSTEM.

G20/G21 is active by default. A switchover to G70/71 is realized using MD10712

$MN_USER_CODE_CONF_NAME_TAB.

$MN_USER_CODE_CONF_NAME_TAB[0]= G20

$MN_USER_CODE_CONF_NAME_TAB[1]= G70

$MN_USER_CODE_CONF_NAME_TAB[2]= G21

$MN_USER_CODE_CONF_NAME_TAB[3]= G71

Regardless of G20/21 G70/71, a 1 is read in system variable $P_GG[6] with G20/G70 and a 2

with G21/G71.

6.1.6

Fixed feedrates F0 - F9

Function

Ten different feedrate values pre-set via setting data can be activated with F0-F9.

To activate the rapid traverse rate with F0, the corresponding speed must be entered in the

setting datum 42160 $SC_EXTERN_FIXED_FEEDRATE_F1_9[0].

The feedrate values for F0-F9 are entered in the setting data as real values. An evaluation of

the input values is not undertaken.

The function is activated via MD22920 $MC_EXTERN_FIXED_FEEDRATE_F1_ON. If the

machine data is set to FALSE, F1-F9 is interpreted as normal feedrate programming, e.g. F2=2

mm/min, F0=0 mm/min.

If the machine data = TRUE, the feedrate values for F0-F9 are fetched from the setting data

42160 $SC_EXTERN_FIXED_FEEDRATE_F1_F9[ ]. If the value 0 exists in one of the setting

data, then the corresponding address extension of feedrate 0 is activated during the

programming.

ISO dialects

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

135

Commissioning

6.1 Machine data

Example

$SC_FIXED_FEEDRATE_F1_F9[0] = 5000

$SC_FIXED_FEEDRATE_F1_F9[1] = 1000

$SC_FIXED_FEEDRATE_F1_F9[2] = 500

N10 X10 Y10 Z10 F0 G94

;Approach position at 5000 mm/min

N20 G01 X150 Y30 F1

;Feedrate 1000 mm/min active

N30 Z0 F2

;Position approached at 500 mm/min

N40 Z10 F0

;Approach position at 5000 mm/min

If the function is activated with MD22920 $MC_FIXED_FEEDRATE_F1_F9_ON and if the

feedrate value from the setting datum is not to be active with F1-F9, then the feedrate value is

programmed as a real value. If, for instance, a feedrate value should be programmed at 1 mm/

min, the feedrate must be programmed with F1.0 instead of F1.

Note

While macroprogramming with G65/66, the programmed value for the address F is always

entered in the $C_F system variable. The address signifies a transfer variable here and has no

direct reference to the feedrate.

The same is true of the thread lead programming in G33-G34 with address F. No feedrate is

programmed with F here, instead the distance between 2 threads during a spindle revolution.

In cycle programming (e.g., G81 X.. Y.. Z.. R.. P.. Q.. F..), the feedrate is always programmed

under address F. In a part program block with a cycle call via a G function (G81-G87 etc.), the

corresponding feedrate value during the programming of F1-F9 is written from the

corresponding setting datum in the variable $C_F.

Restriction

In ISO dialect mode, the feedrate values are changed in the setting data with a handwheel. In

Siemens mode, the feedrates can be influenced only like a directly programmed feedrate, e.g.

using the override switch.

6.1.7

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

Function G17 (G18, G19)<Axis name>.. can be used to activate an axis parallel to the basic

axis in the coordinate system.

The basic axes are, e.g. X, Y and Z. The following programming is used to activate axis U in the

G17 plane in place of basic axis X:

G17 U0 Y0 ;Activation of parallel axis U

This function can be reproduced with the 840D sl function GEOAX (..,..). GEOAX() can be used

to replace a geometry axis with any channel axis. But all frames (apart from handwheel and

external movement), the working area limitation and the protection zones are then deleted. The

user can prevent the frames from being deleted with MD10602

$MN_FRAME_GEOAX_CHANGE_MODE, the protection zones from being deleted with

ISO dialects

136

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

Commissioning

6.1 Machine data

MD10618 $MC_PROTAREA_GEOAX_CHANGE_MODE and working area limitation from

being deactivated with MD10604 $MN_WALIM_GEOAX_CHANGE_MODE.

One parallel axis can be defined for each of the three geometry axes using MD22930

$MC_EXTERN_PARALLEL_GEOAX[ ]. By programming the G function for plane selection

(G17-G19) and the axis name of the parallel axis, a geometry axis interchange is then carried

out as with the GEOAX() function.

During the selection of planes (geometry axis interchange with parallel axis), the axes are

moved to their programmed position.

If a basic axis of the coordinate system is programmed along with its parallel axis in a plane

selection block, alarm 12726 "Impermissible plane selection with parallel axes" is output.

6.1.8

Inserting chamfers and radii

Chamfers and radii

The process of inserting chamfers and radii is mapped to the corresponding Siemens

functionality. The two blocks between which a radius or chamfer is to be inserted must always

be programmed. If there are several addresses programmed in a block, the last radius

programmed always takes effect.

In ISO dialect M mode, the name for the radius is always "R" and for the chamfer "C". As soon

as a comma is programmed in the block, addresses R and C to the right after the comma are

interpreted as radius and chamfer. If a circle is to be programmed with radius R or axis C, the

two addresses must be positioned to the left before the comma. A radius or chamfer can be

inserted between linear blocks, circle blocks or a mix of the two.

In ISO dialect T mode, the name for the radius is always "R", while addresses "C", "I" and "K"

can be used for the chamfer. Address C may only be used if it is not defined as an axis name.

Radii and chamfers can only be inserted between linear blocks. The linear blocks do not have

to be above one another vertically. Programming a sign before the chamfer and/or radius is of

no significance here because the direction of the chamfer and/or radius is defined with the 2nd

straight line block.

ISO dialect M programming

Chamfers and radii are always marked in the block with a comma. The address for a chamfer

is "C" and for a radius is "R". Chamfers and radii can be inserted between linear blocks and

circle blocks.

N10 X100. ,R10

;insert radius of 10 mm

N20 Y30. ,C5

;insert chamfer of 5 mm

N30 X150. Y40.

N40 G03 X180. Y65. R30, R8

N50 G01 X150. ,R8

ISO dialects

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

137

Commissioning

6.1 Machine data

ISO dialect T programming

Chamfers and radii are not marked in the block with a comma. The address for a radius is

always "R", address "I", "K" or "C" can be used for a chamfer. C may only be used if the address

is not defined as an axis name.

In ISO dialect T mode, chamfers and radii can only be inserted between 2 linear blocks.

N10 X100. R10

;insert radius of 10 mm

N20 Z30. C5

;insert chamfer of 5 mm

N30 X150. Z40.

N40 X180. Z65. I8

N50 G01 X150. K8

6.1.9

Rotary axis function

If an axis is defined as a rotary axis, this axis can be traversed as follows:

● Axis is traversed as linear axis

No modulo conversion is active.

Positive and negative values can be programmed

MD30300 $MA_IS_ROT_AX = TRUE

MD30310 $MA_ROT_IS_MODULO = FALSE

● Example:

N5 G90 B0

N10 B370

;axis moves to 370 degrees

N15 B-10

;axis moves to -10 degrees

N20 G91 B-20

;axis moves to -20 degrees

● Axis traverses at shortest distance

Modulo conversion is active

Values < 0 and > modulo value can be programmed

MD30300 $MA_IS_ROT_AX = TRUE

MD30310 $MA_ROT_IS_MODULO = TRUE

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 5 = 0

MD30455 $MA_MISC_FUNCTION_MASK, bit 0 = 1

Example:

N5 B0

;axis moves to 0 degrees

N10 B10

;axis moves to 10 degrees, positive

;Direction of rotation

N15 B350

;axis moves to 350 degrees, negative

;Direction of rotation

N20 B-5

;axis moves to 355 degrees, positive

;Direction of rotation

N25 G91 B-10

;axis moves to 345 degrees, negative

;Direction of rotation

ISO dialects

138

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

Commissioning

6.1 Machine data

● Axis traverses in positive or negative direction depending on sign programmed

Modulo conversion is active

Values < 0 and > modulo value can be programmed

MD30300 $MA_IS_ROT_AX = TRUE

MD30310 $MA_ROT_IS_MODULO = TRUE

MD20734 $MC_EXTERN_FUNCTION_MASK, bit 5 = 1

MD30455 $MA_MISC_FUNCTION_MASK, bit 0 = 1

Example:

N5 B0

;axis moves to 0 degrees

N10 B10

;axis moves to 10 degrees,

;positive direction of rotation

N15 B350

;axis moves to 350 degrees,

;positive direction of rotation

N20 B-5

;axis moves to 355 degrees,

;negative direction of rotation

N25 G91 B-10

;axis moves to 345 degrees,

;negative direction of rotation

In this case, the sign has two meanings, it is taken into account in the modulo conversion and

determines the direction of rotation.

The response is the same for all types of interpolation.

Incremental motion is always executed depending on the sign.

6.1.10

Program coordination between 2 channels and M commands

Overview

M functions which serve as WAIT marks can be programmed to synchronize the program

sequence between two channels. If one such M function is reached in the part program of one

channel, the program sequence is stopped until the other channel has also reached the same

M function. The part programs in the two channels are then processed further.

The M function numbers for the Wait marks are defined with two pieces of machine data. A

range of M numbers is defined and reserved for this function.

Machine data 10800 $MN_EXTERN_CHAN_SYNC_M_NO_MIN marks the smallest M number

and 10802 $MN_EXTERN_CHAN_SYNC_M_NO_MAX the largest M number in the range

reserved for program coordination. Machine data $MN_EXTERN_CHAN_SYNC_M_NO_MAX

must not exceed ($MN_EXTERN_CHAN_SYNC_M_NO_MIN + 10 * number of channels).

To avoid conflicts with standard M functions, the smallest M number (MD

$MN_EXTERN_CHAN_SYNC_M_NO_MIN) must not be less than 100. If the machine data is

predefined with -1, this means that program coordination in ISO dialect T/M mode is not

possible.

If a value <100 is entered in $MN_EXTERN_CHAN_SYNC_M_NO_MIN or a value <

$MN_ETERN_CHAN_SYNC_M_NO_MIN is entered in

$MN_EXTERN_CHAN_SYNC_M_NO_MAX, alarm 4170 "Impermissible number for channel

synchronization" is output.

ISO dialects

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

139

Commissioning

6.2 Standard machine data assignment for ISO dialect

The function is mapped to the WAITM command of the Siemens language (WAITM(<mark>,

<channel number>, <channel number>)). Channel synchronization in ISO dialect T/M mode is

always carried out for channels 1 and 2. All other channels can only be synchronized in

Siemens mode.

The M numbers are not output to the PLC.

The M functions for channel synchronization must be the only items in their block. The system

issues alarm 12080 "Channel %1 block %2 syntax error for text" if addresses other than "M" are

programmed in the block.

For a more detailed description, see

Job Planning; Section "Program coordination"

Constraint

Only 10 M functions (WAIT marks) can be set per channel. The difference between

$MN_EXTERN_CHAN_SYNC_M_NO_MAX and $MN_EXTERN_CHAN_SYNC_M_NO_MIN

must therefore not exceed 20 in a 2-channel system. With ISO dialect original 99999899 M

numbers can be defined as wait marks.

6.2

Standard machine data assignment for ISO dialect

ISO dialect M

Standard assignment of MD20154 $MC_EXTERN_GCODE_RESET_VALUES[ ]:

$MC_EXTERN_GCODE_RESET_VALUES[0] = 1

G00

$MC_EXTERN_GCODE_RESET_VALUES[1]=1

G17

$MC_EXTERN_GCODE_RESET_VALUES[2]=1

G90

$MC_EXTERN_GCODE_RESET_VALUES[3]=2

G23

$MC_EXTERN_GCODE_RESET_VALUES[4]=1

G94

$MC_EXTERN_GCODE_RESET_VALUES[5]=1

G20

$MC_EXTERN_GCODE_RESET_VALUES[6]=1

G40

$MC_EXTERN_GCODE_RESET_VALUES[7]=3

G49

$MC_EXTERN_GCODE_RESET_VALUES[8]=4

G80

$MC_EXTERN_GCODE_RESET_VALUES[9]=1

G98

$MC_EXTERN_GCODE_RESET_VALUES[10]=1

G50

$MC_EXTERN_GCODE_RESET_VALUES[11]=2

G67

$MC_EXTERN_GCODE_RESET_VALUES[12]=2

G97

$MC_EXTERN_GCODE_RESET_VALUES[13]=1

G54

$MC_EXTERN_GCODE_RESET_VALUES[14]=3

G64

$MC_EXTERN_GCODE_RESET_VALUES[15]=2

G69

$MC_EXTERN_GCODE_RESET_VALUES[16]=1

G15

$MC_EXTERN_GCODE_RESET_VALUES[17]=0

non-modal

$MC_EXTERN_GCODE_RESET_VALUES[21]=1

G50.1

ISO dialects

140

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

Commissioning

6.2 Standard machine data assignment for ISO dialect

$MC_EXTERN_GCODE_RESET_VALUES[24]=1

G12.1

$MC_EXTERN_GCODE_RESET_VALUES[30]=1

G290

ISO dialect T

Standard assignment of MD20154 $MC_EXTERN_GCODE_RESET_VALUES[ ]:

Several G code systems are available as options for ISO dialect T. The same function is called

using different G commands. G code system B is realized as standard. Machine datum 10881

$MN_ EXTERN_GCODE_SYSTEM is used to use another G code system.

$MC_EXTERN_GCODE_RESET_VALUES[0]=1

G00

$MC_EXTERN_GCODE_RESET_VALUES[1]=2

G97

$MC_EXTERN_GCODE_RESET_VALUES[2]=1

G90

$MC_EXTERN_GCODE_RESET_VALUES[3]=2

G69

$MC_EXTERN_GCODE_RESET_VALUES[4]=2

G95

$MC_EXTERN_GCODE_RESET_VALUES[5]=1

G21

$MC_EXTERN_GCODE_RESET_VALUES[6]=1

G40

$MC_EXTERN_GCODE_RESET_VALUES[8]=2

G23

$MC_EXTERN_GCODE_RESET_VALUES[9]=1

G80

$MC_EXTERN_GCODE_RESET_VALUES[10]=1

G98

$MC_EXTERN_GCODE_RESET_VALUES[11]=2

G67

$MC_EXTERN_GCODE_RESET_VALUES[15]=2

G18

$MC_EXTERN_GCODE_RESET_VALUES[17]=0

non-modal

$MC_EXTERN_GCODE_RESET_VALUES[19]=1

G50.2

$MC_EXTERN_GCODE_RESET_VALUES[20]=1

G12.1

$MC_EXTERN_GCODE_RESET_VALUES[30]=1

G290

ISO dialects

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

141

SINUMERIK 840D sl. Service - Functions. Manual (2018-2020) - page 2