Macro Call Via M Function; M Functions (M08, M09) - Siemens SINUMERIK 808D Programming And Operating Manual

4.3.5.6

Macro call via M function

Via M numbers, one can call a subroutine (macro) similar to G65.
The configuration of a maximum of 10 M functions replacements is undertaken via machine data 10814
$MN_EXTERN_M_NO_MAC_CYCLE and machine data 10815 $MN_EXTERN_M_NO_MAC_CYCLE_NAME.
Programming takes place identical to G65. Repetitions can be programmed with the L address.
Restrictions
Only one M function replacement (or only one subroutine call) can be executed per part program line. Conflicts with other
subroutine calls are signaled by alarm 12722. There is no further M function replacement in the replaced subroutine.
Otherwise, the same restrictions are valid as in G65.
Conflicts with pre-defined and other defined M numbers are rejected with an alarm.
Configuration example
Call of subroutine M101_MAKRO via the M101 M function:
$MN_EXTERN_M_NO_MAC_CYCLE[0] = 101
$MN_EXTERN_M_NO_MAC_CYCLE_NAME[0] = "M101_MAKRO"
Call of subroutine M6_MAKRO via the M6 M function:
$MN_EXTERN_M_NO_MAC_CYCLE[1] = 6
$MN_EXTERN_M_NO_MAC_CYCLE_NAME[1] = "M6_MAKRO"
Programming example for tool change with M function:
PROC MAIN
...
N10
...
N90
PROC M6_MAKRO
...
N0010
N0020
N0030
N0040
N0050
N0060
4.3.5.7

M functions (M08, M09)

General M functions
The non-specific M functions are defined by the machine manufacturer. A representative example of the use of general M
functions is available under. Details are available in the documentation of your machine manufacturer. If an M command is
programmed with an axis motion in the same block, whether the M function is to be executed at the start or end of the block
on reaching the axis position depends on the machine data setting of the machine manufacturer. Details are available in the
documentation of your machine manufacturer.
M function Function
M08 Coolant ON
M09 Coolant OFF
Specification of several M functions in one block
A maximum of five M functions can be programmed in on block. Possible combinations of M functions and possible
restrictions are specified in the documentation of your machine manufacturer.
Programming and Operating Manual (ISO Turning/Milling)
01/2017
M6 X10 V20
M30
R10 = R10 + 11.11
IF $C_X_PROG == 1 GOTOF N40
SETAL(61000)
IF $C_V == 20 GTOF N60
SETAL(61001)
M17
Remarks
These M functions are defined by the machine manufacturer.
;Call of M6_MAKRO program
;($C_X_PROG)
;programmed variable not
;transferred correctly
;($C_V)
121