Siemens SINUMERIK 840D Programming Manual page 95

03.96
2
Programming example
Row of holes
With this program you can machine a row of holes
of 5 tapped holes positioned in parallel to the Z axis
on the ZX plane, with a distance between each hole
of 20 mm. The row of holes starts at Z20 and X30,
the first hole in the row being 10 mm from this point.
The geometry of the row of holes is described by the
cycle HOLES1. First of all, drilling is performed with
cycle CYCLE81 and then with CYCLE84 tapping
(rigid). The holes are 80 mm deep. This is the
difference between the reference plane and the
final drilling depth.
DEF REAL RFP=102, DP=22, RTP=105
DEF REAL SDIS, FDIS
DEF REAL SPCA=30, SPCO=20, STA1=0,
FDIS=20, DBH=20
->
DEF INT NUM=5
N10 SDIS=3 FDIS=10
N20 G90 F30 S500 M3 D1 T1
N30 G18 G0 Z20 Y105 X30
N40 MCALL CYCLE81 (RTP, RFP, SDIS, DP)
N50 HOLES1 (SPCA, SPCO, STA1, FDIS,
-> DBH, NUM)
N60 MCALL
...
N70 G90 G0 Z30 Y75 X105
N80 MCALL CYCLE84 (RTP, RFPSDIS, DP, ,
, , 3, , 4.2)
->
N90 HOLES1 (SPCA, SPCO, STA, FDIS,
DBH, NUM)
->
N100 MCALL
N110 M30
-> Must be programmed in a single block
 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
Z
A
B
30
Definition of parameters with value
assignments
->
Value for safety clearance and distance
of the first hole to the reference point
Specification of technology values for the
machining section
Approach starting position
Modal call of drilling cycle
Call of row of holes cycle, the cycle starts
->
with the first hole. Only the drilling
positions are approached in this cycle
Deselect modal call
Tool change
Traverse to position next to 5th hole
Modal call of tapping cycle
->
Call of row of holes cycle started with
->
the 5th hole in the row
Deselect modal call
End of program
2
Z
A - B
X
22
102
2-95
Y