Siemens SINUMERIK 840D Programming Manual page 128

3
Milling Cycles
3.3 Thread cutting – CYCLE90
Further notes
The milling cutter radius is taken into account by the
cycle. A tool offset must therefore be programmed
before the cycle is called. Otherwise alarm
61000 "No tool offset active" is output and the cycle
is aborted.
When the tool radius equals zero or a negative
value, the cycle is also aborted with this alarm.
With inside threads, the tool radius is monitored and
alarm 61105 "Cutter radius too large" is output and
the cycle is aborted.
Programming example
Inside thread
With this program you can machine an inside thread
at position X60 Y50 on the G17 plane.
DEF REAL RTP=48, RFP=40, SDIS=5, ->
-> DPR=40, DIATH=60, KDIAM=50
DEF REAL PIT=2, FFR=500, CPA=60,CPO=50
DEF INT CDIR=2, TYPTH=0
N10 G90 G0 G17 X0 Y0 Z80 S200 M3
N20 T5 D1
N30 CYCLE90 (RTP, RFP, SDIS, ->
-> DPR, DIATH, KDIAM, PIT, FFR, CDIR,
TYPTH, CPA, CPO)
N40 G0 G90 Z100
N50 M02
-> Must be programmed in a single block
3-128
Y
60
Definition of variables with value assignment
Approach starting position
Specification of technology values
Cycle call
Approach position after cycle
End of program
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
3
12.97
08.97
Y
A - B
A
B
X
40 Z
© Siemens AG, 2002. All rights reserved