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

12

Finishing cycle run

The TNC uses the tool position as cycle starting point when a cycle
is called. If the Z coordinate of the starting point is less than Q492
Contour start in Z, the TNC positions the tool in the Z coordinate
to Q492 and begins the cycle there.
1 The TNC positions the tool at rapid traverse to the first slot side.
2 The TNC finishes the side wall of the slot at the defined feed
rate Q505.
3 The TNC finishes the slot floor at the defined feed rate. If a
radius for contour edges Q500 was specified, the TNC finishes
the complete slot in one pass.
4 The TNC returns the tool at rapid traverse.
5 The TNC positions the tool at rapid traverse to the second slot
side.
6 The TNC finishes the side wall of the slot at the defined feed
rate Q505.
7 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).
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).
430
Cycles: Turning | AXIAL RECESSING EXTENDED
(Cycle 852, DIN/ISO: G852)
HEIDENHAIN | User's manual for cycle programming | 10/2017