HEIDENHAIN TNC 620 (340 56x-01) - Manual (Page 246)

246
8.2 Cy
cles f
o
r Dr
illing, T
apping and Thr
ead Milling
TAPPING WITH CHIP BREAKING (Cycle 209,
Advanced programming features software
option)
The tool machines the thread in several passes until it reaches the
programmed depth. You can define in a parameter whether the tool is
to be retracted completely from the hole for chip breaking.
1 The TNC positions the tool in the spindle axis at rapid traverse
FMAX to the programmed set-up clearance above the workpiece
surface. There it carries out an oriented spindle stop.
2 The tool moves to the programmed infeed depth, reverses the
direction of spindle rotation and retracts by a specific distance or
completely for chip release, depending on the definition. If you
have defined a factor for increasing the spindle speed, the TNC
retracts from the hole at the corresponding speed
3 It then reverses the direction of spindle rotation again and
advances to the next infeed depth.
4 The TNC repeats this process (2 to 3) until the programmed thread
depth is reached.
5 The tool is then retracted to the set-up clearance. If programmed,
the tool moves to the 2nd set-up clearance at FMAX.
6 The TNC stops the spindle turning at set-up clearance.
Machine and control must be specially prepared by the
machine tool builder for use of this cycle.
This cycle is effective only for machines with controlled
spindle.
Before programming, note the following
Program a positioning block for the starting point (hole
center) in the working plane with radius compensation R0.
The algebraic sign for the parameter thread depth
determines the working direction.
The TNC calculates the feed rate from the spindle speed.
If the spindle speed override is used during tapping, the
feed rate is automatically adjusted.
The feed-rate override knob is disabled.
At the end of the cycle the spindle comes to a stop. Before
the next operation, restart the spindle with M3 (or M4).