Cycle Parameters - HEIDENHAIN TNC 640 User Manual

5
Fixed Cycles: Pocket Milling / Stud Milling / Slot Milling | RECTANGULAR STUD (Cycle 256, DIN/ISO: G256)

Cycle parameters

Q218 First side length?: Stud length, parallel to
the reference axis of the working plane. Input
range 0 to 99999.9999
Q424 Workpiece blank side length 1?: Length
of the unmachined stud, parallel to the reference
axis of the working plane. Enter Workpiece
blank side length 1 greater than First side
length. The TNC performs multiple stepovers if
the difference between blank dimension 1 and
finished dimension 1 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
Q219 Second side length?: Stud length, parallel
to the minor axis of the working plane. Enter
Workpiece blank side length 2 greater than
Second side length The TNC performs multiple
stepovers if the difference between blank
dimension 2 and finished dimension 2 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
Q425 Workpiece blank side length 2?: Length of
the unmachined stud, parallel to the minor axis of
the working plane. Input range 0 to 99999.9999
Q220 Radius / Chamfer (+/-)?: Enter the value
for the input form radius or chamfer. If you enter
a positive value between 0 and +99999.9999,
the TNC rounds every corner. The radius refers
to the value you entered. If you enter a negative
value between 0 and -99999.9999 all corners of
the contour are chamfered and the value entered
refers to the length of the chamfer.
Q368 Finishing allowance for side? (incremental):
Finishing allowance in the working plane, is left
over after machining. Input range 0 to 99999.9999
Q224 Angle of rotation? (absolute): Angle by
which the entire machining is rotated. The center
of rotation is the position at which the tool is
located when the cycle is called. Input range
-360.0000 to 360.0000
Q367 Position of stud (0/1/2/3/4)?: Position of
the stud in reference to the position of the tool
when the cycle is called:
0: Tool position = stud center
1: Tool position = left corner below
2: Tool position = right corner below
3: Tool position = right corner top
4: Tool position = left corner top
182
HEIDENHAIN | User's manual for cycle programming | 10/2017