12
Finishing cycle run
The TNC uses the tool position as cycle starting point when a cycle
is called.
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:
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).
434
Cycles: Turning | AXIAL RECESSING
(Cycle 850, DIN/ISO: G850)
HEIDENHAIN | User's manual for cycle programming | 10/2017