Sandvik Coromant Threading - Manual (Page 93)

93
5. Technical reference
Programming – machining centre
In thread milling; rolling in and out of cut achieves good tool life
and high thread quality
When programming a large thread profi le, it may be necessary to
split up the machining into at least two passes.
The most useful software for selection of cutting data, tool and
programming a thread with a milling cutter is PluraGuide (non-CAM
software).
The only difference between programming CoroMill Plura and
CoroMill 327/CoroMill 328 is the need to repeat the circular
motion until the correct thread depth has been reached (circular
ramping).
Programming the feed rate on most machining centres is based on
the centre line of the spindle. This must be taken into account to
avoid shortened tool life, vibration or tool breakdown.
Example ISO longhand code (lathe)
T0101 (THREADING TOOL)
G97 S2103 M3
G0 X26.0 Z8.5 M8
G0 X23.623 Z4.5
G32 Z-26.5 F2.0
G0 X26.0
G0 Z4.404
G0 X23.083
G32 Z-26.5 F2.0
G32 is the command for the threading movement in the machine.
This code can differ depending of the CNC system (check your
machine manual to confi rm). If the start point for the threading
operation varies in the z-axis, the thread should be programmed
with fl ank infeed.