Circular Pocket (Cycle 252, Din/Iso: G252, Software Option 19); Cycle Run - HEIDENHAIN TNC 620 User Manual

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | CIRCULAR POCKET (Cycle 252, DIN/ISO: G252,
5.3 CIRCULAR POCKET (Cycle 252, DIN/ISO:
G252, software option 19)

Cycle run

Use Cycle 252 CIRCULAR POCKET to machine circular pockets.
Depending on the cycle parameters, the following machining
alternatives are available:
Complete machining: Roughing, floor finishing, side finishing
Only roughing
Only floor finishing and side finishing
Only floor finishing
Only side finishing
Roughing
1 The TNC first moves the tool at rapid traverse to the set-up
clearance Q200 above the workpiece.
2 The tool plunges to the first plunging depth at the pocket center.
Specify the plunging strategy with parameter Q366.
3 The TNC roughs out the pocket from the inside out, taking
the path overlap (parameter Q370) and the finishing allowance
(parameters Q368 and Q369) into account.
4 At the end of a roughing operation, the TNC moves the tool
tangentially away from the pocket wall by the set-up clearance
Q200 in the working plane, then retracts the tool by Q200 at
rapid traverse and returns it from there at rapid traverse to the
pocket center.
5 Steps 2 to 4 are repeated until the programmed pocket depth is
reached, taking the finishing allowance Q369 into account.
6 If only roughing was programmed (Q215=1) the tool moves
away from the pocket wall tangentially by the set-up clearance
Q200, then retracts at rapid traverse to the 2nd set-up clearance
Q204 in the tool axis and returns at rapid traverse to the pocket
center
156
HEIDENHAIN | TNC 620 | User's manual for cycle programming | 10/2017
software option 19)