Pilot Drilling (Cycle 21, Din/Iso: G121, Software Option 19); Cycle Run; Please Note While Programming - HEIDENHAIN TNC 620 User Manual

PILOT DRILLING (Cycle 21, DIN/ISO: G121, software option 19)

7.5 PILOT DRILLING (Cycle 21, DIN/ISO:
G121, software option 19)

Cycle run

1 The tool drills from the current position to the first plunging
depth at the programmed feed rate F.
2 When it reaches the first plunging depth, the tool retracts in
rapid traverse FMAX to the starting position and advances again
to the first plunging depth minus the advanced stop distance t.
3 The advanced stop distance is automatically calculated by the
control:
At a total hole depth up to 30 mm: t = 0.6 mm
At a total hole depth exceeding 30 mm: t = hole depth / 50
Maximum advanced stop distance: 7 mm
4 The tool then advances with another infeed at the programmed
feed rate F .
5 The TNC repeats this process (1 to 4) until the programmed
total hole depth is reached.
6 After a dwell time at the hole bottom, the tool is returned to the
starting position in rapid traverse FMAX for chip breaking.
Application
Cycle 21 is for PILOT DRILLING of the cutter infeed points. It
accounts for the allowance for side and the allowance for floor as
well as the radius of the rough-out tool. The cutter infeed points
also serve as starting points for roughing.

Please note while programming:

When calculating the infeed points, the TNC does
not account for the delta value DR programmed in a
TOOL CALL block.
In narrow areas, the TNC may not be able to carry
out pilot drilling with a tool that is larger than the
rough-out tool.
TNC 620 | User's Manual Cycle Programming | 3/2014
7
7.5
181