HEIDENHAIN SW 54843x-03 DIN Programming - Manual (Page 138)

138 smart.Turn units
2.9 Units—Milling, f
a
ce
"Thread milling" unit
The unit 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 "approach 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.
Unit name: G799_Gewindefr_C / Cycle: G799 (see page 338)
Access to the technology database:
 Machining operation: Finish milling
 Affected parameters: F, S
Position form
Z1
Start point drill (starting point of hole)
P2 Thread depth
I Thread diameter
F1 Thread pitch
Cycle form
J
Direction of thread
 0: Right-hand thread
 1: Left-hand thread
H Cutting direction
 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)
R Approach radius
Further forms: see page 60