Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | CIRCULAR SLOT (Cycle 254, DIN/ISO: G254)

Cycle parameters

Q215 Machining operation (0/1/2)?: Define
machining operation:
0: Roughing and finishing
1: Only roughing
2: Only finishing
Side finishing and floor finishing are only machined
when the specific allowance (Q368, Q369) is
defined
Q219 Width of slot? (value parallel to the
secondary axis of the working plane): Enter the
slot width. If you enter a slot width that equals the
tool diameter, the TNC will carry out the roughing
process only (slot milling). Maximum slot width for
roughing: Twice the tool diameter. Input range 0 to
99999.9999
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range 0 to 99999.9999
Q375 Pitch circle diameter?: Enter the diameter
of the pitch circle. Input range 0 to 99999.9999
Q367 Ref. for slot pos. (0/1/2/3)?: Position of the
slot in reference to the position of the tool when
the cycle is called:
0: The tool position is not taken into account. The
slot position is determined from the entered pitch
circle center and the starting angle
1: Tool position = center of left slot arc. Starting
angle Q376 refers to this position. The entered
pitch circle center is not taken into account
2: Tool position = center of centerline. Starting
angle Q376 refers to this position. The entered
pitch circle center is not taken into account
3: Tool position = center of right slot arc. Starting
angle Q376 refers to this position. The entered
pitch circle center is not taken into account.
Q216 Center in 1st axis? (absolute): Center of
the stud in the reference axis of the working
plane. Only effective if Q367 =
-99999.9999 to 99999.9999
HEIDENHAIN | User's manual for cycle programming | 10/2017
0. Input range
5
177