HEIDENHAIN TNC 640 (34059x-02) Cycle programming - Manual (Page 372)

Cycles: Turning
13.28 THREAD LONGITUDINAL
(Cycle 831, DIN/ISO: G831)
13
372
TNC 640 | User's Manual Cycle Programming | 5/2013
13.28 THREAD LONGITUDINAL
(Cycle 831, DIN/ISO: G831)
Application
This cycle enables you to run longitudinal turning of threads.
You can process single threads or multi-threads with the cycle.
If you do not enter a thread depth, the cycle uses thread depth in
accordance with the ISO1502 standard.
The cycle can be used for inside and outside machining.
Cycle run
The TNC uses the tool position as cycle starting point when a cycle
is called.
1 The TNC positions the tool in rapid traverse at set-up clearance
in front of the thread and runs an infeed motion.
2 The TNC runs a paraxial longitudinal cut. Here the TNC
synchronizes feed rate and speed so that the defined pitch is
machined.
3 The TNC retracts the tool at rapid traverse by the set-up
clearance.
4 The TNC positions the tool back at rapid traverse to the
beginning of cut.
5 The TNC runs an infeed motion. The infeeds are run according
to the angle of infeed
Q467.
6 The TNC repeats the process (2 to 5) until the thread depth is
completed.
7 The TNC runs the number of air cuts as defined in Q476.
8 The TNC repeats the process (2 to 7) according to the number
of traverses
Q475.
9 The TNC positions the tool back at rapid traverse to the cycle
starting point.