Cycle Parameters - HEIDENHAIN TNC 640 User Manual

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

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
Q223 Circle diameter?: Diameter of the finished
pocket. Input range 0 to 99999.9999
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the machining plane. Input
range 0 to 99999.9999
Q207 Feed rate for milling?: Traversing speed of
the tool in mm/min while milling. Input range 0 to
99999.999 alternatively FAUTO, fu, FZ
Q351 Direction? Climb=+1, Up-cut=-1: Type of
milling operation with M3:
+1 = Climb
–1 = Up-cut
PREDEF: The TNC uses the value from the
GLOBAL DEF block (if you enter 0, climb milling is
performed)
Q201 Depth? (incremental): Distance between
workpiece surface and bottom of pocket. Input
range -99999.9999 to 99999.9999
Q202 Plunging depth? (incremental): Infeed per
cut; enter a value greater than 0. Input range 0 to
99999.9999
Q369 Finishing allowance for floor?
(incremental): Finishing allowance for the floor.
Input range 0 to 99999.9999
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while moving to depth.
Input range 0 to 99999.999, alternatively FAUTO,
FU, FZ
168
HEIDENHAIN | User's manual for cycle programming | 10/2017