Siemens SINUMERIK 808D ADVANCED - Circle of Holes - HOLES2

Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
157
N10 G90 F300 S500 M3 T10 D1
; Specification of the technological values
N20 G17 G0 X=R14 Y=R15 Z105
; Approach starting position
N30 MCALL CYCLE82(R11, R10, R12, R13,
0, 1)
; Modal call of drilling cycle
N40 LABEL1:
; Call of row of holes cycle
N41 HOLES1(R14, R15, R16, R17, R18,
R19)
N50 R15=R15+R22
; Calculate y value for the next line
N60 R21=R21+1
; Increment line counter
N70 IF R21<R20 GOTOB LABEL1
; Return to LABEL1 if the condition is fulfilled
N80 MCALL
; Deselect modal call
N90 G90 G0 X30 Y20 Z105
; Approach starting position
N100 M02
; End of program
9.5.3
Circle of holes - HOLES2
Programming
HOLES2 (CPA, CPO, RAD, STA1, INDA, NUM)
Parameters
Parameter
Data type
Description
CPA REAL Center point of circle of holes (absolute), first axis of the plane
CPO REAL Center point of circle of holes (absolute), second axis of the plane
RAD REAL Radius of circle of holes (enter without sign)
STA1 REAL Starting angle
Range of values: –180<STA1≤180 degrees
INDA REAL Incrementing angle
NUM INT Number of holes
Function
Use this cycle to machine a circle of holes. The machining plane must be defined before the cycle is called.
The type of hole is determined through the drilling cycle that has already been called modally.