Enhanced Level Commands
4.10 Macroprograms
04.07
4-160
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
Siemens mode/ISO mode macro program execution
The called macro program can either be executed in Siemens mode or ISO mode.
The execution mode is decided in the first block of the macro program.
If
a
PROC
<program
name>
instruction
is
included
in
the
first
block
of
the
macro
program, it is automatically switched to Siemens mode. If no such instruction is
included, ISO mode is retained.
By executing a macro program in Siemens mode, transfer parameters can be
stored into local variables using the DEF instruction. In ISO mode, however, trans-
fer parameters cannot be stored into local variables.
In order to read transfer parameters within the macroprogram executed in ISO
mode, switch to Siemens mode by G290 command.
Examples
Main program containing the macro call:
_N_M10_MPF:
N10 M3 S1000 F1000
N20 X100 Y50 Z33
N30 G65 P10 F55 X150 Y100 S2000
N40 X50
N50 ....
N200 M30
Macro program in Siemens mode:
_N_0010_SPF:
PROC 0010 ; Switching into 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 G95 S=S_SPEED
...
N80 M17
Macro program in ISO mode:
_N_0010_SPF:
G290 ; Switching into Siemens mode,
; if transfer parameters need to be read
N15 X_AXIS = $C_X Y_AXIS = $C_Y S_SPEED = $C_S FEED = $C_F
N20 G01 F=$C_F G95 S=$C_S
N10 G1 X=$C_X Y=$C_Y
G291 ; Switching into ISO mode
N15 M3 G54 T1
N20
...
N80 M99
To Next Page
Loading...
Need help?
General
