Thread Drilling/Milling (Cycle 264, Din/Iso: G264, Software Option 19); Cycle Run - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Tapping / Thread Milling | THREAD DRILLING/MILLING (Cycle 264, DIN/ISO: G264, software
option 19)
4.8 THREAD DRILLING/MILLING (Cycle 264,
DIN/ISO: G264, software option 19)

Cycle run

1 The TNC positions the tool in the tool 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 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 that 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 in rapid
traverse to setup clearance or, if programmed, to the 2nd setup
clearance.
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
4
135