Cycle Parameters - HEIDENHAIN TNC 620 User Manual

10
Fixed Cycles: Multipass Milling
10.5 FACE MILLING (Cycle 233, DIN/ISO: G233, software option 19)

Cycle parameters

Machining operation (0/1/2) Q215: 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
Milling strategy (0 to 4) Q389: Determine how the
TNC should machine the surface:
0: Meander machining, stepover at the positioning
feed rate outside the surface to be machined
1: Meander machining, stepover at the feed rate for
milling at the edge of the surface to be machined
2: Line-by-line machining, retraction and stepover at
the positioning feed rate outside the surface to be
machined
3: Line-by-line machining, retraction and stepover at
the positioning feed rate at the edge of the surface
to be machined
4: Helical machining, uniform infeed from the
outside toward the inside
Milling direction Q350: Axis in the machining plane
that defines the machining direction:
1: Reference axis = machining direction
2: Minor axis = machining direction
1st side length Q218 (incremental): Length of the
surface to be multipass-milled in the reference axis
of the working plane, referenced to the starting
point in the 1st axis. Input range 0 to 99999.9999
2nd side length Q219 (incremental value): 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 stepover in reference to
the starting point in the 2nd axis. Input range
-99999.9999 to 99999.9999
246
Q357
TNC 620 | User's Manual Cycle Programming | 3/2014
Q227