Calling Machining Cycles - Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual

Program repetition P...
If a subroutine is to be executed several times in succession, write the number of times it is to be executed in the block of
the call after the subroutine name under the address P. A maximum of 9,999 cycles are possible (P1 ... P9999).
Example:
N10 L785 P3
Nesting depth
Subroutines can also be called from a subroutine, not only from a main program. In total, up to 8 program levels are
available for this type of nested call, including the main program level.
See the following illustration for execution with 8 program levels:
Information
Modal G functions can be changed in the subroutine, e.g. G90 -> G91. When returning to the calling program, ensure that all
modal functions are set the way you need them to be.
Please make sure that the values of your arithmetic parameters used in upper program levels are not inadvertently changed
in lower program levels.
When working with SIEMENS cycles, up to 4 program levels are needed.
8.15.2

Calling machining cycles

Functionality
Cycles are technology subroutines realizing a certain machining process generally, for example, drilling or milling.
Adaptation to the particular problem is performed directly via supply parameters/values when calling the respective cycle.
Programming example
N10 DEF REAL RTP, RFP, SDIS, DP, DTB
N20 G18 X100 Z100 G0
N30 M3 S100 F100
N40 G17 X0
N50 CYCLE83(110, 90, 0, -80, 0, -10, 0, 0, 0, 0, 1, 0) ; Call of cycle 83, transfer values directly,
N60 G0 X100 Z100
N70 RTP=100 RFP= 95.5 SDIS=1, DP=-5, DTB=3
N80 CYCLE82(RTP, RFP, SDIS, DP, , DTB)
N90 M30
112
; Call subroutine L785, 3 cycles
separate block
; Set transfer parameters for cycle 82
; Call of cycle 82, separate block
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014