HEIDENHAIN iTNC 530 (340 49x-01) - Manual (Page 378)

378 8 Programming: Cycles
8.6 SL Cy
cles
8 Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
8 Feed rate for plunging Q11: Traversing speed of the
tool in mm/min during penetration.
8 Feed rate for milling Q12: Traversing speed for
milling in mm/min.
8 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” on page 144) and define the
maximum plunging ANGLE of the tool. The TNC will
otherwise generate an error message.
8 Reciprocation feed rate Q19: Traversing speed of
the tool in mm/min during reciprocating plunge-cut.
8 Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting after machining. If
you enter Q208 = 0, the TNC retracts the tool at the
feed rate in Q12.
FLOOR FINISHING (Cycle 23)
The tool approaches the machining plane smoothly (in a vertically
tangential arc). The tool then clears the finishing allowance remaining
from rough-out.
8 Feed rate for plunging Q11: Traversing speed of the
tool during penetration.
8 Feed rate for milling Q12: Traversing speed for
milling.
8 Retraction feed rate Q208: Traversing speed of the
tool in mm/min when retracting after machining. If
you enter Q208 = 0, the TNC retracts the tool at the
feed rate in Q12.
Example: NC blocks
60 CYCL DEF 23.0 FLOOR FINISHING
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR ROUGHING
Q208=99999 ;RETRACTION FEED RATE
X
Z
Q11
Q12
The TNC automatically calculates the starting point for
finishing. The starting point depends on the available
space in the pocket.