HEIDENHAIN TNC 410 ISO Programming - Manual (Page 242)

216 8 Programming: Cycles
8.3 Cy
cles f
o
r Dr
illing
, T
a
p
p
ing
and
Th
read Millin
g THREAD DRILLING/MILLING (Cycle G264)
not TNC 410)
1 The TNC positions the tool in the tool axis at rapid traverse to the
programmed setup clearance above the workpiece surface.
Drilling
2 The tool drills to the first plunging depth at the programmed feed
rate for plunging.
3 If you have programmed chip breaking, the tool then retracts by
the entered retraction value. If you are working without chip
breaking, the tool is moved at rapid traverse to set-up clearance
and then at rapid traverse to the entered starting position above
the first plunging depth.
4 The tool then advances with another infeed at the programmed
feed rate.
5 The TNC repeats this process (2 to 4) until the programmed total
hole depth is reached.
Countersinking at front
6 The tool moves at the feed rate for pre-positioning to the sinking
depth at front.
7 The TNC positions the tool without compensation from the center
on a semicircle to the offset at front, and then follows a circular
path at the feed rate for countersinking.
8 The tool then moves in a semicircle to the hole center.
Thread milling
9 The TNC moves the tool at the programmed feed rate for pre-
positioning to the starting plane for the thread. The starting plane
is determined from the thread pitch and the type of milling (climb
or up-cut).
10 Then the tool moves tangentially on a helical path to the thread
diameter and mills the thread with a 360° helical motion.
11 After this, the tool departs the contour tangentially and returns to
the starting point in the working plane.