Finishing Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Cycles: Turning | RECESSING CONTOUR RADIAL
(Cycle 840, DIN/ISO: G840)

Finishing cycle run

1 The TNC positions the tool at rapid traverse to the first slot side.
2 The TNC finishes the side walls of the slot at the defined feed
rate Q505.
3 The TNC finishes the slot floor at the defined feed rate.
4 The TNC positions the tool back at rapid traverse to the cycle
starting point.

Please note while programming:

Danger of collision!
The cutting limit defines the contour range to be machined. The
approach and departure paths can exceed the cutting limits. The
tool position before the cycle call influences the execution of the
cutting limit. The TNC 640 machines the area to the right or to
the left of the cutting limit, depending on which side the tool has
been positioned before the cycle is called.
Before the cycle is called position the tool so that it is already
on the side of the cutting limit on which the material is to be
cut
Program a positioning block to the starting position with
radius compensation R0 before the cycle call.
The tool position at cycle call defines the size of the area
to be machined (cycle starting point).
Before calling the cycle you must program the cycle 14
CONTOUR to define the subprogram number.
When you use local QL Q parameters in a contour
subprogram you must also assign or calculate these in
the contour subprogram.
From the second infeed, the TNC reduces each further
cutting traverse by 0.1 mm. This reduces lateral
pressure on the tool. If the offset width Q508 was
input into the cycle, the TNC reduces the cutting
traverse by this value. After clearance roughing, the
remaining material is removed with a single cut. The
TNC generates an error message if the lateral offset
exceeds 80 % of the effective cutting width (effective
cutting width = cutting width –2*cutting radius).
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
12
423