Siemens SINUMERIK 828D Programming Manual page 120

Flexible NC programming
1.14 Interrupt routine (ASUB)
Example
A broken tool should be automatically replaced by a daughter tool. Machining is then
continued with the new tool.
Main program:
Main program
N10 SETINT(1) PRIO=1 W_WECHS 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
Subprogram:
Subprogram
PROC W_CHANGE SAVE
N10 G0 Z100 M5
N20 T11 M6 D1 G41
N30 REPOSL RMB M3
120
Comments
; When input 1 is switched, the tool
is immediately retracted from the
contour with rapid lift (code No. 7
for tool radius compensation G41).
Then interrupt routine "W_WECHS" is
executed.
Comments
; Subprogram where the actual operating
state is saved
; Tool changing position, spindle stop
; Change tool
; Reposition at the contour and return
jump into the main program (this is
programmed in a block)
Programming Manual, 07/2010, 6FC5398-2BP40-0BA0
Job planning