Contour-Parallel Thread (Cycle 830, Din/Iso: G830); Application; Cycle Run - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | CONTOUR-PARALLEL THREAD
(Cycle 830, DIN/ISO: G830)
12.30 CONTOUR-PARALLEL THREAD
(Cycle 830, DIN/ISO: G830)

Application

This cycle enables you to run both face turning and longitudinal
turning of threads with any form.
You can process single threads or multi-threads with the cycle.
If you do not enter a thread depth in the cycle, the cycle uses a
standardized thread depth.
The cycle can be used for inside and outside machining.
Danger of collision!
The cycle 830 runs the overrun Q466 following the programmed
contour. Note the spatial conditions.
Clamp the workpiece in such a way that there is no danger of
collision if the TNC extends the contour by Q466, Q467

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 thread cut parallel to the defined thread contour.
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.
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
12
471