Thread Milling Axial G799 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Drilling cycles

Thread milling axial G799

G799 mills a thread in existing holes.
Place the tool on the center of the hole before calling G799. The
cycle positions the tool to the end point of the thread within the
hole. Then the tool approaches at Apprch angle R and mills the
thread. With each rotation the tool moves by the Thread pitch F.
Following that, the cycle retracts the tool and returns it to the Start
pt. Z. With parameter V, you can program whether the thread is
to be milled in one rotation or, with single-point tools, in several
rotations.
Parameters:
I: Thread diameter
Z: Start pt. Z
K: Thread depth
R: Approach radius
F: Thread pitch
J: Direction of thread:
0: Right-hand thread
1: Left-hand thread
H: Mill cutting direction
0: Up-cut
1: Climb
V: Milling method
0: One revolution – the thread is milled in a 360-degree
helix
1: Two or more revolutions – the thread is milled in several
helix paths (single-point tool)
Use thread-milling tools for cycle G799.
Example: G799
%799.nc
N1 T9 G195 F0.2 G197 S800
N2 G0 X100 Z2
N3 M14
N4 G110 Z2 C45 X100
N5 G799 I12 Z0 K-20 F2 J0 H0
N6 M15
END
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
391