HEIDENHAIN CNC Pilot 4290 - Manual (Page 144)

4 DIN PLUS 132
4.7 T
u
rning Cy
cles
G890 Q4—Residual finishing
Finish contour G890
G890 finishes the contour area defined by „NS, NE“ parallel to the
contour in one pass and takes chamfers/rounding into account.
Undercuts are machined where tool geometry permits.
The CNC PILOT uses the tool definition to distinguish between
external and internal machining.
With „NS – NE“ you specify the machining direction. If the contour
to be machined consists of one element, the following applies:
■ The contour is machined in the defined direction if you program
only NS
■ The contour is machined opposite to the defined direction if
you program NS and NE.
You activate the residual finishing with Q=4 (example: hollowing
with finishing tools that machine in the direction opposite to that
defined). The CNC PILOT knows the areas that have already been
machined and does not machine them again. If Q=4, you cannot
influence the approach type. It is determined by the finishing cycle.
Note for small chamfers/rounding:
■ Peak-to-valley height or feed rate (with G95-Geo) are not
programmed: The CNC PILOT automatically reduces the feed
rate. The chamfer/rounding arc is machined with at least 3
revolutions.
■ If peak-to-valley height or feed rate (with G95 Geo) are
programmed: no automatic feed reduction
For chamfers/rounding which, as a result of their size, are machined
with at least three revolutions, the feed rate is not reduced
automatically.
Parameters
NS:
Starting block number (beginning of contour section)
NE: End block number (end of contour section)
E: Approach behavior
■ E=0: Descending contours are not machined
■ E>0: Approach behavior
■ No input: Feed rate reduced depending on approach angle
—maximum reduction: 50%
V: Identifier beginning/end—default: 0
A chamfer/rounding arc is being machined:
■ V=0: At beginning and end
■ V=1: At beginning
■ V=2: At end
■ V=3: No machining
■ V=4: Chamfer/rounding is being machined—not the basic
element (prerequisite: Contour section with an element)
Type of approach—default: 0
■ Q=0: Automatic selection—the CNC PILOT checks:
– Diagonal approach
– First X, then Z direction
Continued
During residual finishing (G890 – Q4),
the CNC PILOT checks whether the tool
can move into the contour valley without
a collision. The collision check is based
on tool parameter „width dn“ (see “
8.1.2
Notes on Tool Data”).