HEIDENHAIN CNC Pilot 4290 - Manual (Page 140)

4 DIN PLUS 128
4.7 T
u
rning Cy
cles
Recessing G860
G860 machines (indents) the contour area defined by “NS, NE”
axially/radially. The contour to be machined may contain various
valleys. The CNC PILOT uses the tool definition to distinguish
between external and internal machining, or between radial and
axial recesses.
Calculation of the cut segmentation (SBF: see machining
parameter 6): maximum offset = SBF * width of cut
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
If required, the area to be machined is divided into several sections,
for example, for machining contour valleys.
The simplest way of programming is specifying NS, or NS and NE.
Parameters
NS:
Starting block number (beginning of contour section, or
reference to recess defined by G22/G23-Geo).
NE: End block number (end of contour section)—omit for contour
defined by G22/G23-Geo.
I: Oversize in X direction (diameter value)—default: 0
K: Oversize in Z direction—default: 0
Q: Sequence—default: 0
■ Q=0: Roughing and finishing
■ Q=1: Roughing only
■ Q=2: Finishing only
X: Cutting limit in X direction (diameter value)—default: no
cutting limit
Z: Cutting limit in Z direction—default: no cutting limit
Code start/end—default: 0
A chamfer/rounding arc is machined:
■ V=0: At the start and end
■ V=1: At the start
■ V=2: At end
■ V=3: No machining
E: Feed rate for finishing—default: Active feed rate
H: Retraction at end of cycle—default: 0
■ H=0: Return to starting point (axial recess: first Z and then X
direction; radial recess: first X and then Z direction)
■ H=1: Position in front of the finished contour
■ H=2: Move to clearance height and stop
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
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 first cut (roughing).
4 Return at rapid traverse and approach for next
pass.
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.