HEIDENHAIN iTNC 530 (340 49x-04) ISO programming - Manual (Page 406)

406 8 Programming: Cycles
8.6 SL c
y
cles
 Plunging depth Q10 (incremental value): Dimension
by which the tool plunges in each infeed.
 Feed rate for plunging Q11: Traversing speed of the
tool in mm/min during penetration.
 Feed rate for milling Q12: Traversing speed for
milling in mm/min.
 Coarse roughing tool Q18 or QS18: Number or name
of the tool with which the TNC has already coarse-
roughed the contour. Switch to name input: Press the
TOOL NAME soft key. The TNC automatically inserts
the closing quotation mark when you exit the input
field. If there was no coarse roughing, enter “0”; if
you enter a number or a name, 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 193 and
define the maximum plunging ANGLE of the tool. The
TNC will otherwise generate an error message.
 Reciprocation feed rate Q19: Traversing speed of
the tool in mm/min during reciprocating plunge-cut.
 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.
 Feed rate factor in %: Q401: Percentage factor by
which the TNC reduces the machining feed rate(Q12)
as soon as the tool moves within the material over its
entire circumference during roughing. If you use the
feed rate reduction, then you can define the feed rate
for roughing so large that there are optimum cutting
conditions with the path overlap (Q2) specified in
Cycle 20. The TNC then reduces the feed rate as per
your definition at transitions and narrow places, so
the machining time should be reduced in total.
 Fine-roughing strategy Q404: Specify how the TNC
should move the tool during fine roughing when the
radius of the fine-roughing tool is larger than half the
coarse roughing tool.
„ Q404 = 0
Move the tool along the contour at the current
depth between areas that need to be fine-roughed.
„ Q404 = 1
Between areas that need to be fine-roughed,
retract the tool to safety clearance and move to the
starting point of the next area to be rough-milled.
Example: NC block
N59 G122 ROUGH-OUT
Q10=+5 ;PLUNGING DEPTH
Q11=100 ;FEED RATE FOR PLUNGING
Q12=350 ;FEED RATE FOR ROUGHING
Q18=1 ;COARSE ROUGHING TOOL
Q19=150 ;RECIPROCATION FEED RATE
Q208=99999 ;RETRACTION FEED RATE
Q401=80 ;FEED RATE REDUCTION
Q404=0 ;FINE ROUGH STRATEGY
Feed rate reduction through parameter Q401 is an FCL3
function and is not automatically available after a software
update (see “Feature content level (upgrade functions)”
on page 8).