Thread Cutting - Siemens SINUMERIK 840D Programming Manual

Turning Cycles
4
4.7 Thread cutting – CYCLE97
Programming example

Thread cutting

With this program you can cut a metric outside
thread M42x2 with flank infeed. The infeed is
performed with a constant cross-section of cut.
5 roughing cuts are made to a thread depth of
1.23 mm without final machining allowance. After
machining has been completed, 2 noncuts are
performed.
DEF REAL MPIT=42, SPL=0, FPL=-35,
DM1=42, DM2=42, APP=10, ROP=3,
TDEP=1.23, FAL=0, IANG=30, NSP=0
DEF INT NRC=5, NID=2, VARI=3, NUMT=1
N10 G0 G90 Z100 X60
N20 G95 D1 T1 S1000 M4
N30 CYCLE97 ( , MPIT, SPL, FPL, DM1, ->
-> DM2, APP, ROP, TDEP, FAL, IANG, ->
-> NSP, NRC, NID, VARI, NUMT)
N40 G90 G0 X100 Z100
N50 M30
-> Must be programmed in a single block
4-250
X
Definition of parameters with value
assignments
Selection of starting position
Specification of technology values
Cycle call
Approach next position
End of program
SINUMERIK 840D/840Di/810D/FM-NC Programming Guide, Cycles (PGZ) - 04.00 Edition
03.96
4
M42x2
Z
35
 Siemens AG 2000 All rights reserved.