Hobbing G808 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO Programming for the Y axis | Milling cycles for the Y axis

Hobbing G808

G808 mills a gear profile from the Start point Z to the Final point
K. In W you enter the angular position of the tool.
If an oversize has been programmed, hobbing is split up in rough-
machining and subsequent finishing.
In parameters O, R and V you define the tool shift. Shifting by R
ensures a uniform wear of the hob cutter.
Parameters:
Z: Start point
K: Final point
C: Angle – offset angle of the C axis
A: Root circle diameter
B: Tip circle diameter
J: Number of workpiece teeth
W: Angle position
S: Cutting speed in m/min
I: Allowance
D: Turn. direct. of the workpiece
3: M3
4: M4
F: Feed per revolution
E: Finishing feed
P: Maximum infeed
O: Shift starting position
R: Shift value
V: Shift quantity
H: Infeed axis
0: Tool infeed is performed in the X axis
1: Tool infeed is performed in the Y axis
Q: Spindle with workpiece
0: Spindle 0 (main spindle) holds the workpiece
3: Spindle 3 (opposing spindle) holds the workpiece
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
6
609