Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | CIRCULAR STUD (Cycle 257, DIN/ISO: G257)

Cycle parameters

Q223 Finished part diameter?: Diameter of the
finished stud. Input range 0 to 99999.9999
Q222 Workpiece blank diameter?: Diameter
of workpiece blank. Enter the workpiece blank
diameter greater than the finished diameter. The
TNC performs multiple stepovers if the difference
between the workpiece blank diameter and
finished diameter is greater than the permitted
stepover (tool radius multiplied by path overlap
Q370). The TNC always calculates a constant
stepover. 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 stud. 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
Q206 Feed rate for plunging?: Traversing speed
of the tool in mm/min while moving to depth.
Input range 0 to 99999.999; alternatively fmax,
FAUTO, fu, FZ
Q200 Set-up clearance? (incremental): Distance
between tool tip and workpiece surface. Input
range 0 to 99999.9999; alternatively PREDEF
HEIDENHAIN | User's manual for cycle programming | 10/2017
5
187