Siemens SINUMERIK 808D Programming And Operating Manual page 86

Example of entering an argument:
Execution of macro programs in the Siemens and ISO modes
A called macro program can be called either in Siemens mode or in ISO mode. The language mode in which the program is
executed is defined in the first block of the macro program.
If a PROC <Program name> instruction exists in the first block of a macro program, then an automatic changeover to
Siemens mode is conducted. If this instruction is missing, the processing is done in ISO mode.
The transfer parameters can be saved in local variables by executing a program in Siemens mode. In ISO mode however, it
is not possible to store transfer parameters in local variables.
To read transfer parameters in a macro program executed in ISO mode, one must first change over to Siemens mode with
the G290 command.
Examples
Main program with macro call:
_N_M10_MPF:
N10 M3 S1000 F1000
N20 X100 Y50 Z33
N30 G65 P10 F55 X150 Y100 S2000
N40 X50
N50 ....
N200 M30
Macro program in Siemens mode:
_N_0010_SPF:
PROC 0010 ; Changeover to Siemens mode
N10 DEF REAL X_AXIS ,Y_AXIS, S_SPEED, FEED
N15 X_AXIS = $C_X Y_AXIS = $C_Y S_SPEED = $C_S FEED = $C_F
N20 G01 F=FEED G99 S=S_SPEED
...
N80 M17
Macro program in ISO mode:
_N_0010_SPF:
G290; Changeover to Siemens mode,
; to read the transfer parameters
N15 X_AXIS = $C_X Y_AXIS = $C_Y S_SPEED = $C_S FEED = $C_F
N20 G01 F=$C_F G99 S=$C_S
N10 G1 X=$C_X Y=$C_Y
G291; Changeover to ISO mode,
N15 M3 G54 T1
N20
Programming and Operating Manual (ISO Turning/Milling)
86
01/2017