HEIDENHAIN iTNC 530 (340 49x-05) Cycle programming - Manual (Page 69)

HEIDENHAIN iTNC 530 69
3.2 CENTERING (Cy
c
le 240, DIN/ISO: G240)
3.2 CENTERING (Cycle 240,
DIN/ISO: G240)
Cycle run
1 The TNC positions the tool in the spindle axis at rapid traverse FMAX
to the setup clearance above the workpiece surface.
2 The tool is centered at the programmed feed rate F to the entered
centering diameter or centering depth.
3 If defined, the tool remains at the centering depth.
4 Finally, the tool moves 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 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!
Enter in MP7441 bit 2 whether the TNC should output an
error message (bit 2=1) or not (bit 2=0) if a positive depth
is entered.
Keep in mind that the TNC reverses the calculation for
pre-positioning when a positive diameter or depth is
entered. This means that the tool moves at rapid traverse
in the tool axis to setup clearance below the workpiece
surface!