HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 320)

320
DIN programming
4.22 Dr
illing cy
cles
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.
Type of taps:
 Stationary tap: Main spindle and feed drive are synchronized.
 Driven tap: Driven tool and feed drive are synchronized.
Example: G36
. . .
N1 T5 G97 S1000 G95 F0.2 M3
N2 G0 X0 Z5
N3 G71 Z-30
N4 G14 Q0
N5 T6 G97 S60 0 M3
N6 G0 X0 Z8
N7 G36 Z-25 F1.5 B3 [tapping]
. . .
Parameters
X End point radial hole (diameter value)
Z End point of axial hole
F Feed per revolution (thread pitch)
B Run-in length for synchronizing spindle and feed drive
S Retraction speed (default: Shaft speed for tapping)
P Chip breaking depth
I Retraction distance
 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.