HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 278)

278
4.27 Milling Cy
cles
Thread milling, axial G799
Starting with software version 625 952-05: G799 mills a thread in
existing holes.
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 revolution or, with single-point tools, in several revolutions.
Example: G799
%799.nc
[G799]
N1 T9 G195 F0.2 G197 S800
N2 G0 X100 Z2
N3 M14
N4 G799 XK100 C45 Z0 I12 K-20 F2 J0 H0 V0
N5 M15
END
Parameters
X Polar starting point
C Polar starting point
XK Cartesian starting point
YK Cartesian starting point
Z Milling top edge
I Thread diameter
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 One rotation / several rotations
„ 0: The thread is milled in a 360-degree rotation
„ 1: The thread is milled in several rotations (single-point tool)
Use thread-milling tools for cycle G799.
Danger of collision!
The hole depth must exceed the thread depth by at least
F/2.