Centering (Cycle 240, Din/Iso: G240); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Drilling | CENTERING (Cycle 240, DIN/ISO: G240)
3.2

CENTERING (Cycle 240, DIN/ISO: G240)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse
FMAX to the set-up clearance above the workpiece surface.
2 The tool is centered at the programmed feed rate F to the
programmed centering diameter or centering depth.
3 If defined, the tool remains at the centering depth.
4 Finally, the tool path is retraced to setup clearance or—if
programmed—to the 2nd setup clearance at rapid traverse
FMAX.

Please note while programming:

Program a positioning block for the starting point
(hole center) in the working plane with the radius
compensation R0
The algebraic sign for the cycle parameter Q344
(diameter) or Q201 (depth) determines the working
direction. If you program the diameter or depth = 0, the
cycle will not be executed.
Danger of collision!
If you enter a positive depth with a cycle, the TNC reverses
calculation of the pre-positioning. This means that the tool
moves at rapid traverse in the tool axis to set-up clearance
below the workpiece surface!
Enter depth as negative
Enter in machine parameter displayDepthErr (No. 201003)
whether the TNC should output an error message (on) or not
(off) if a positive depth is entered
HEIDENHAIN | User's manual for cycle programming | 10/2017
NOTICE
3
79