HEIDENHAIN CNC Pilot 4290 V7.1 Description of B and Y axes - Manual (Page 66)

66
1
.1
1
DIN PLUS (Y Axis): Milling Cy
cles
Thread milling in YZ plane G806
Starting with software version 625 952-05: G806 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.
Parameters
I
Thread diameter
X Starting point in X
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)
O Spindle brake (O is evaluated if the brake is entered in
machine parameter 1019, ..)—default: 0
„ 0: Activate the spindle brake
„ 1: Deactivate the spindle brake
Use thread-milling tools for cycle G806.
Danger of collision!
The hole depth must exceed the thread depth by at
least F/2.