Siemens SINUMERIK 808D User Manual page 181

drilling is carried out using CYCLE82, and then tapping is performed using CYCLE84 (tapping without compensating chuck).
The holes are 80 mm in depth (difference between reference plane and final drilling depth).
N10 G90 F30 S500 M3 T10 D1
N20 G17 G90 X20 Z105 Y30
N30 MCALL CYCLE82(105, 102, 2, 22, 0, 1)
N40 HOLES1(20, 30, 0, 10, 20, 5)
N50 MCALL
...
N60 G90 G0 X30 Z110 Y105
N70 MCALL CYCLE84(105, 102, 2, 22, 0, , 3, , 4.2, ,300, )
N80 HOLES1(20, 30, 0, 10, 20, 5)
N90 MCALL
N100 M02
Programming example: Grid of holes
Use this program to machine a grid of holes consisting of five rows with five holes each, which are arranged in the XY plane,
with a spacing of 10 mm between them. The starting point of the grid is at X30 Y20.
The example uses R parameters as transfer parameters for the cycle.
R10=102
R11=105
R12=2
R13=75
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017
; Reference plane
; Retraction plane
; Safety clearance
; Drilling depth
; Specification of the technological
values for the machining step
; Approach start position
; Modal call of drilling cycle
; Call of row-of-holes cycle; the cycle
starts with the first hole; only the
drill positions are approached in this
cycle
; Deselect modal call
; Change tool
; Approach position next to 5th hole
; Modal call of the tapping cycle
; Call of row of holes cycle starting
with the fifth hole in the row
; Deselect modal call
; End of program
181