Cycle Parameters - HEIDENHAIN TNC 640 User Manual

Cycles: Special Functions | FACE MILLING (Cycle 232, DIN/ISO: G232)

Cycle parameters

Q389 Machining strategy (0/1/2)?: Determine
how the TNC should machine the surface:
0: Meander machining, stepover at the positioning
feed rate outside the surface being machined
1: Meander machining, stepover at the feed
rate for milling at the edge of the surface being
machined
2: Line-by-line machining, retraction and stepover
at the positioning feed rate
Q225 Starting point in 1st axis? (absolute):
Starting point coordinate of the surface to be
machined in the reference axis of the working
plane. Input range -99999.9999 to 99999.9999
Q226 Starting point in 2nd axis? (absolute):
Starting point coordinate of the surface to be
machined in the minor axis of the working plane.
Input range -99999.9999 to 99999.9999
Q227 Starting point in 3rd axis? (absolute):
Coordinate of the workpiece surface used to
calculate the infeeds. Input range -99999.9999 to
99999.9999
Q386 End point in 3rd axis? (absolute):
Coordinate in the spindle axis on which the surface
is to be face-milled. Input range -99999.9999 to
99999.9999
Q218 First side length? (incremental): Length
of the surface to be machined in the reference
axis of the working plane. Use the algebraic sign
to specify the direction of the first milling path in
reference to the starting point in the 1st axis.
Input range -99999.9999 to 99999.9999
Q219 Second side length? (incremental): Length
of the surface to be machined in the minor axis
of the working plane. Use the algebraic sign
to specify the direction of the first transverse
approach in reference to the STARTNG PNT 2ND
AXIS. Input range -99999.9999 to 99999.9999
Q202 Maximum plunging depth? (incremental):
Maximum
actual plunging depth from the difference between
the end point and starting point of the tool axis
(taking the finishing allowance into account), so
that uniform plunging depths are used each time.
Input range 0 to 99999.9999
Q369 Finishing allowance for floor?
(incremental): Distance used for the last infeed.
Input range 0 to 99999.9999
HEIDENHAIN | User's manual for cycle programming | 10/2017
infeed per cut. The TNC calculates the
11
349