Siemens SINUMERIK 840D Programming Manual page 99

03.96
2
Programming example
Hole circle
The program uses CYCLE82 4 to produce holes with
a depth of 30 mm. The final drilling depth is defined
as a value relative to the reference plane. The circle
is defined by the center point X70 Y60 and the
radius 42 mm in the XY plane. The initial angle is 33
degrees.
The safety clearance in the drilling axis Z is 2 mm.
DEF REAL CPA=70,CPO=60,RAD=42,STA1=33
DEF INT NUM=4
N10 G90 F140 S710 M3 D4 T40
N20 G17 G0 X50 Y45 Z2
N30 MCALL CYCLE82 (2, 0,2, , 30)
N40 HOLES2 (CPA, CPO, RAD, STA1, , NUM)
N50 MCALL
N60 M30
 Siemens AG 2000 All rights reserved.
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
Drilling Cycles and Drilling Patterns
2.3 Drill pattern cycles
Y
A
33°
42
B
70
Definition of parameters with value
assignments
Specification of technology values
Approach starting position
Modal call of drilling cycle, without dwell
time, DP is not programmed
Call of circle of holes cycle, the indexing
angle is calculated internally by the cycle
as parameter INDA has been omitted
Deselect modal call
End of program
2
Y
X
Z
30
2-99