HEIDENHAIN TNC 640 (34059x-01) Cycle programming - Manual (Page 112)

112 Fixed Cycles: Tapping / Thread Milling
4.8 THREAD DRILLING/MILLING
(Cy
c
le 264, DIN/ISO: G264)
4.8 THREAD DRILLING/MILLING
(Cycle 264, DIN/ISO: G264)
Cycle run
1 The TNC positions the tool in the spindle axis at rapid traverse FMAX
to the entered 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
countersinking 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.