HEIDENHAIN TNC 410 ISO Programming - Manual (Page 298)

272 8 Programming: Cycles
8.7 SL Cy
cles Gr
ou
p II (no
t T
N
C
4
1
0)
ROUGH-OUT (Cycle G122)
1 The TNC positions the tool over the cutter infeed point, taking the
allowance for side into account.
2 In the first plunging depth, the tool mills the contour from inside
outward at the milling feed rate Q12.
3 The island contours (here: C/D) are cleared out with an approach
toward the pocket contour (here: A/B).
4 Then the TNC rough-mills the pocket contour retracts the tool to
the clearance height.
U U U U Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
U U U U Feed rate for plunging Q11: Traversing speed of the
tool in mm/min during penetration.
U U U U Feed rate for milling Q12: Traversing speed for
milling in mm/min.
U U U U Coarse roughing tool number Q18: Number of the
tool with which the TNC has already coarse-roughed
the contour. If there was no coarse roughing, enter
“0”; if you enter a value other than zero, the TNC will
only rough-out the portion that could not be machined
with the coarse roughing tool.
If the portion that is to be roughed cannot be
approached from the side, the TNC will mill in a
reciprocating plunge-cut; For this purpose you must
enter the tool length LCUTS in the tool table TOOL.T
(see “Tool Data,” page 99) and define the maximum
plunging ANGLE of the tool. The TNC will otherwise
generate an error message.
U U U U Reciprocation feed rate Q19: Traversing speed of
the tool in mm/min during reciprocating plunge-cut.
Example: NC block
N57 G120 Q10=+5 Q11=100 Q12=350 Q18=1
Q19=150 *
C D
A B
Before programming, note the following:
This cycle requires a center-cut end mill (ISO 1641) or pilot
drilling with Cycle G121.