8 Programming: Cycles
198
ROUGH-OUT (Cycle 22)
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.
3 First the island contours (
C
and
D
in the figure at right) are rough-
milled until the pocket contour (
A
,
B
) is approached.
4 Then the pocket contour is rough-milled and the tool is retracted
to the clearance height.
Before programming, note the following:
This cycle requires a center-cut end mill (ISO 1641) or
pilot drilling with Cycle 21.
ú
Plunging depth Q10 (incremental value):
Dimension by which the tool plunges in each infeed
ú
Feed rate for plunging Q11: Traversing speed of the
tool in mm/min during penetration
ú
Feed rate for milling Q12: Traversing speed for milling
in mm/min
ú
Coarse roughing tool number Q18: Number of the tool
with which the TNC has already coarse-roughed the
contour. If the contour has not been coarse-roughed,
enter zero. If you enter a value other than 0, 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 fine-roughed cannot be
approached from the side, the TNC will mill in a
reciprocating plunge-cut. For this purpose, you must
enter the tooth length LCUTS and the maximum
plunge angle ANGLE of the tool in the tool table
TOOL.T (see Chapter 5.2). The TNC will otherwise
generate an error message.
ú
Reciprocation feed rate Q19: Traversing speed of the
tool in mm/min during reciprocating plunge-cut
Example NC blocks:
59 CYCL DEF 22.0 ROUGH-OUT
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR MILLING
Q18=1 ;COARSE ROUGHING TOOL
Q19=150 ;RECIPROCATION FEED RATE
C
D
A
B
8.5 SL Cycles
kkap8.pm6 30.06.2006, 07:03198
www.EngineeringBooksPdf.com
To Next Page
Loading...
Need help?
General
