Drilling (Cycle 200); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

Fixed Cycles: Drilling | DRILLING (Cycle 200)
3.3

DRILLING (Cycle 200)

Cycle run

1 The TNC positions the tool in the tool axis at rapid traverse
FMAX to set-up clearance above the workpiece surface.
2 The tool drills to the first plunging depth at the programmed
feed rate F.
3 The TNC returns the tool at FMAX to the set-up clearance,
dwells there (if a dwell time was entered), and then moves at
FMAX to the set-up clearance above the first plunging depth.
4 The tool then drills deeper by the plunging depth at the
programmed feed rate F .
5 The TNC repeats this process (2 to 4) until the programmed
depth is reached (the dwell time from Q211 is effective with
every infeed)
6 Finally, the tool path is retraced to setup clearance from the
hole bottom or—if programmed—to the 2nd setup clearance at
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 DEPTH
determines the working direction. If you program
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
the workpiece surface!
below
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 | TNC 620 | User's manual for cycle programming | 10/2017
NOTICE
3
73