HEIDENHAIN SW 548328-05 DIN Programming - Manual (Page 328)

328
DIN programming
4.22 Dr
illing cy
cles
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 on the end point of the thread within the hole. Then
the tool approaches on "approaching radius R" and mills the thread.
During this, the tool advances by the thread pitch F. Following that, the
cycle retracts the tool and returns it to the starting point. With
parameter V, you can program whether the thread is to be milled in
one rotation or, with single-point tools, in several rotations.
Example: G799
%799.nc
[G799]
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
Parameters
I Thread diameter
Z Starting point Z
K Thread depth
R Approach radius
F Thread pitch
J Direction of thread—(default: 0)
 0: Right-hand thread
 1: Left-hand thread
H Cutting direction (default: 0)
 0: Up-cut milling
 1: Climb milling
V Milling method
 0: The thread is milled in a 360-degree helix
 1: The thread is milled in several helical paths (single-point
tool)
Use thread-milling tools for cycle G799.
Danger of collision!
Be sure to consider the hole diameter and the diameter of
the milling cutter when programming "approach radius R."