HEIDENHAIN CNC Pilot 4290 - Manual (Page 142)

4 DIN PLUS 130
4.7 T
u
rning Cy
cles
Continued
Recess turning cycle G869
G869 machines (indents) the contour area defined by ”NS, NE”
axially/radially. The workpiece is machined by alternate recessing
and roughing movements. The machining process requires a
minimum of retraction and infeed movements.
The contour to be machined may contain various valleys. If
required, the area to be machined is divided into several sections.
The CNC PILOT uses the tool definition to distinguish between
radial and axial recesses.
With ”NS – NE” you specify the machining direction. If the contour
to be machined consists of one element, then:
■ If you program only NS: Machining in contour definition
direction
■ If you program NS and NE: Machining against the contour
definition direction
Depending on factors such as workpiece material or feed rate, the
tool tip is displaced during a turning operation. You can correct the
resulting infeed error with “turning depth compensation factor” R.
The value is usually determined empirically.
After the second infeed movement, during the transition from
turning to recessing, the path to be machined is reduced by “Offset
width B.” Each time the system switches on this side, the path is
reduced by “B”—in addition to the previous offset. The total offset
is limited to 80% of the effective cutting width (effective cutting
width = cutting width – 2 * cutting radius). If required, the CNC
PILOT reduces the programmed offset width. After precutting, the
remaining material is removed with a single cut.
Unidirectional turning (U=1): Roughing is in the machining direction
”NS – NE.”
The simplest way of programming is specifying NS or NS, NE and P.
Parameters
NS:
Starting block number (beginning of contour section, or
reference to G22/G23 Geo recess)
NE: End block number (end of contour section)—omit for contour
defined by G22/G23-Geo.
P: Maximum infeed
R: Turning depth compensation for finishing—default: 0
I: Oversize in X direction (diameter value)—default: 0
K: Oversize in Z direction—default: 0
X: Cutting limit in (diameter value)—default: no cutting limit
Z: Cutting limit—default: no cutting limit
Cycle run (where Q=0 or 1)
1 Calculate the areas to be machined and the
cutting segmentation.
2 Approach workpiece for first pass from starting
point, taking the safety clearance into account
(radial recess: first in Z, then in X direction; axial
recess: first in X, then in Z direction)
3 Execute the first cut (recessing).
4 Machine perpendicularly to recessing direction
(turning).
5 Repeat 3 to 4 until the complete area has been
machined.
6 If required, repeat 2 to 5 until all areas have been
machined.
7 Q=0: Finish-machine the contour.
G869 requires tools of the type 26*.
Cutting limitation: The tool position
before the cycle call determines the
effect of a cutting limit. The CNC PILOT
machines the area to the right or to the
left of the cutting limit, depending on
which side the tool has been positioned
before the cycle is called.
Cutter radius compensation: Active
G57 oversize: ”Enlarges” the contour
(also inside contours)
G58 oversize:
■ >0: ”enlarges” the contour
■ <0: is not considered
G57/G58 oversizes are deleted after
cycle end