Calling Machining Cycles - Siemens SINUMERIK 808D User Manual

See the following illustration for execution with 8 program levels:
In formation
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.
11.15.2

Calling machining cycles

Fu n ctionality
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
11.15.3 Modal subroutine call
Fu n ctionality
The subroutine in the block containing MCALL is called automatically after each successive block containing a p a th motion.
The call acts until the next MCALL is called.
The modal call of the subroutine which contains MCALL or quitting of the call requires a separate block.
MCALL is advantageous, for example, when producing drill patterns.
Programming example
Application example: Drilling a row of holes
N10 MCALL CYCLE82(100, 0, 1, -10, 2)
N20 HOLES1(1, 2, 45, 2, 2, 1)
N30 MCALL
N40 M30
134
separate block
; Set transfer parameters for cycle 82
; Call of cycle 82, separate block
; Drilling cycle 82
; Cycle for row of holes; after each approach
of the hole position, CYCLE82(...) will be
called with the transfer parameters
; Modal call of CYCLE82(...) completed
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017