Siemens SINUMERIK 828D Programming Manual page 164

Flexible NC programming
1.25 Subprogram technique
Example 2: A cycle is to act like a command for a user
Main program:
Program code
N10 G1 X10 G90 F200
N20 X-4 Y6
N30 CYCLE1
N40 G1 X0
N50 M30
Cycle CYCLE1:
Program code
N100 PROC CYCLE1 DISPLOF SBLOF
N110 R10=3*SIN(R20)+5
N120 IF (R11 <= 0)
N130 SETAL(61000)
N140 ENDIF
N150 G1 G91 Z=R10 F=R11
N160 M17
CYCLE1 is processed for active single block execution, i.e., the Start key must be pressed
once to process CYCLE1.
Example 3:
An ASUB, which is started by the PLC in order to activate a modified zero offset and tool
offsets, is to be executed invisibly.
Program code
N100 PROC ZO SBLOF DISPLOF
N110 CASE $P_UIFRNUM OF
N120 _G54: G54 D=$P_TOOL T=$P_TOOLNO
N130 RET
N140 _G54: G55 D=$P_TOOL T=$P_TOOLNO
N150 RET
N160 _G56: G56 D=$P_TOOL T=$P_TOOLNO
N170 RET
N180 _G57: G57 D=$P_TOOL T=$P_TOOLNO
N190 RET
N200 END: D=$P_TOOL T=$P_TOOLNO
N210 RET
164
Comments
; Suppress single block
0 GOTOF _G500
1 GOTOF _G54
2 GOTOF _G55
3 GOTOF _G56
4 GOTOF _G57
DEFAULT GOTOF END
Programming Manual, 07/2010, 6FC5398-2BP40-0BA0
Job planning