Siemens SINUMERIK 840D sl Programming Manual page 61

Example
In this example, a broken tool is to be replaced automatically by an alternate tool. Machining
is continued with the new tool. Machining is then continued with the new tool.
Main program
N10 SETINT(1) PRIO=1 W_CHANGE ->
-> LIFTFAST
N20 G0 Z100 G17 T1 ALF=7 D1
N30 G0 X-5 Y-22 Z2 M3 S300
N40 Z-7
N50 G41 G1 X16 Y16 F200
N60 Y35
N70 X53 Y65
N90 X71.5 Y16
N100 X16
N110 G40 G0 Z100 M30
Subroutine
PROC W_CHANGE SAVE
N10 G0 Z100 M5
N20 T11 M6 D1 G41
N30 REPOSL RMB M3
-> programmed in a single block.
Caution
If you do not program any of the REPOS commands in the subroutine, the axis is moved to
the end of the block that follows the interrupted block.
Create interrupt routine as subroutine
The interrupt routine is identified as a subroutine in the definition.
Example:
PROC LIFT_Z
N10
N50 M17
Program name LIFT_Z, followed by the NC blocks, finally end-of-program M17 and return
to main program.
Job planning
Programming Manual, 03/2006 Edition, 6FC5398-2BP10-1BA0
1.14 Interrupt routine (SETINT, DISABLE, ENABLE, CLRINT)
When input 1 is enabled, the tool is
automatically retracted from the contour
with liftfast (code no. 7 for tool radius
compensation G41). Interrupt routine
W_CHANGE is subsequently executed.
Subroutine with storage of current
operating state
;Tool changing position, spindle stop
;Change tool
;Repositioning and return
;to main program
Flexible NC programming
1-47