HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 250)

250
4.23 Dr
illing Cy
cles
Tapping G36
G36 cuts axial/radial threads using driven or stationary tools.
Depending on X/Z, G36 decides whether a radial or axial thread will be
machined.
Move to the starting point before G36. G36 returns to the starting
position after having cut the thread.
Cycle run
1 Moves at rapid traverse to the starting point:
„ K not programmed: Retracts directly to the starting point
„ K programmed: Moves to the position K and then to the
starting point
2 Moves along run-in length B feed rate (synchronization of spindle
and feed drives).
3 Cuts the thread.
4 Retracts with return speed S:
„ K not programmed: To the starting point
„ K programmed: To the position K
Example: G36
. . .
N1 T5 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-30
N4 G14 Q0
N5 T6 G97 S600 M3
N6 G0 X0 Z8
N7 G36 Z-25 F1.5 B3 Q0 [tapping]
. . .
Parameters
X End point of axial hole (diameter value)
Z End point of radial hole
F Feed per revolution: Thread pitch
Q Number of spindle (default: 0—main spindle)
B Run-in length for synchronizing spindle and feed drive
H Reference direction for thread pitch (default: 0)
„ H=0: Feed rate on the Z axis
„ H=1: Feed rate on the X axis
„ H=2: Feed rate on the Y axis
„ H=3: Contouring feed rate
S Retraction speed (default: Tapping speed)