Tapping G36 - Single Path - HEIDENHAIN CNC PILOT 640 User Manual

4
Tapping G36 – single path
G36 cuts axial and radial threads using driven or stationary tools.
Depending on X/Z, G36 decides whether a radial or axial hole will
be machined.
Move to the starting point before G36. G36 returns to the starting
position after having cut the thread.
Parameters:
X: Diameter – end point of radial hole
Z: Target point
F: Feed per rot. (thread pitch)
B: Run-in lgth for synchronizing spindle and feed drive
S: Return speed (default: tapping speed)
P: Chip breaking depth
I: Return distance
Types of taps:
Stationary tap: Main spindle and feed drive are synchronized
Driven tap: Driven tool and feed drive are synchronized
NC STOP interrupts the tapping operation
NC 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
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
. . .
372
DIN/ISO programming | Drilling cycles
Tapping
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017