Thread Milling In Xy Plane G800 - HEIDENHAIN CNC PILOT 640 User Manual

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

Thread milling in XY plane G800

G800 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 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 G800.
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
6
607