Tapping G36—Single Path - HEIDENHAIN MANUALPLUS 620 User Manual

Tapping G36—Single path
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.
Parameters
X Final point of axial hole (diameter value)
Z Final point of radial hole
F Feed per revolution (thread pitch)
B Slop. length (run-in length) for synchronizing spindle and feed
drive
S Return speed (default: Tapping speed)
Type of taps:
Stationary tap: Main spindle and feed drive are synchronized.
Driven tap: Driven tool and feed drive are synchronized.
Cycle stop interrupts the tapping operation.
Cycle start resumes the tapping operation.
Use the feed rate override function for speed changes.
Spindle override is not effective.
Use a floating tap holder if the driven tool is not
controlled, e.g. by a ROD encoder.
298
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 [tapping]
. . .
ISO Programming