Siemens SINUMERIK 840D Programming Manual page 89

2
03.96
09.01
Further notes
Depending on the setting in machine data
NUM_ENCS, the cycle selects whether tapping is to
performed with or without encoder.
The direction of rotation for the spindle must be
programmed with M3 or M4 before the cycle is
called.
In thread blocks with G63, the values of the feedrate
override switch and spindle speed override switch
are frozen at 100 percent.
A longer compensating chuck is usually required for
tapping without encoder.
Programming example
Thread without encoder
In this program a thread is tapped without encoder at
position X35 Y35 in the XY plane, the drilling axis is
the Z axis. Parameters SDR and SDAC for the
direction of rotation must be assigned, parameter
ENC is assigned the value 1, the value for the depth
is absolute. Pitch parameter PIT can be omitted. A
compensating chuck is used in machining.
N10 G90 G0 D2 T2 S500 M3
N20 G17 X35 Y35 Z60
N30 G1 F200
N40 CYCLE840 (59, 56, , 15, , 1, 4, 3, 1) Cycle call, dwell time 1 sec, SDR=4,
N50 M30
© Siemens AG, 2002. All rights reserved
SINUMERIK 840D/840Di/810D Programming Guide Cycles (PGZ) – 11.02 Edition
Drilling Cycles and Drilling Patterns
2.1 Drilling cycles
Y
A
B
X
35
Specification of technology values
Traverse to drilling position
Specification of path feedrate
SDAC=3, no safety clearance, parameters
MPIT, PIT are not programmed, i.e. the lead
results from the correlation between the
freely programmable values F and S.
End of program
2
Y
A - B
Z
15
56
2-89