HEIDENHAIN TNC 320 (340 551-01) - Manual (Page 211)

HEIDENHAIN TNC 320 211
8.2 Cy
cles f
o
r Dr
illing,
T
apping and Thr
ead Milling
THREAD DRILLING/MILLING (Cycle 264)
1 The TNC positions the tool in the tool axis at rapid traverse FMAX
to the programmed set-up 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 the set-up
clearance and then at FMAX 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.
12 At the end of the cycle, the TNC retracts the tool at rapid traverse
to the set-up clearance, or—if programmed—to the 2nd set-up
clearance.
Before programming, note the following:
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation R0.
The algebraic sign of the cycle parameters depth of thread,
countersinking depth or sinking depth at front determines
the working direction. The working direction is defined in
the following sequence:
1st: Depth of thread
2nd: Total hole depth
3rd: Depth at front
If you program a depth parameter to be 0, the TNC does
not execute that step.
Program the thread depth as a value smaller than the total
hole depth by at least one-third the thread pitch.