Thread Milling (Cycle 262, Din/Iso: G262); Cycle Run - HEIDENHAIN TNC 640 User Manual

4
4.6 THREAD MILLING (Cycle 262, DIN/ISO:
G262)

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.
2 The tool moves at the programmed feed rate for pre-positioning
to the starting plane. The starting plane is derived from the
algebraic sign of the thread pitch, the milling method (climb or
up-cut milling) and the number of threads per step.
3 The tool then moves tangentially on a helical path to the thread
major diameter. Before the helical approach, a compensating
motion of the tool axis is carried out in order to begin at the
programmed starting plane for the thread path.
4 Depending on the setting of the parameter for the number of
threads, the tool mills the thread in one helical movement, in
several offset helical movements or in one continuous helical
movement.
5 After that the tool departs the contour tangentially and returns
to the starting point in the working plane.
6 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.
136
Fixed Cycles: Tapping / Thread Milling | THREAD MILLING (Cycle 262, DIN/ISO: G262)
HEIDENHAIN | User's manual for cycle programming | 10/2017