HEIDENHAIN CNC Pilot 4290 - Manual (Page 139)

HEIDENHAIN CNC PILOT 4290 127
4.7 T
u
rning Cy
cles
Contour-parallel with neutral tool G835
G830 machines the contour area defined by “NS, NE” parallel to
the contour and bidirectionally. The CNC PILOT uses the tool
definition to distinguish between external and internal machining.
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, NE and P.
Parameters
NS:
Starting block number (beginning of contour section)
NE: End block number (end of contour section)
P: Maximum infeed
I: Oversize in X direction (diameter value)—default: 0
K: Oversize in Z direction—default: 0
X: Cutting limit in X direction (diameter value)—default: no
cutting limit
Z: Cutting limit in Z direction—default: no cutting limit
A: Approach angle (reference: Z axis)—default: 0°/180° (parallel
to Z-axis)
W: Departing angle (reference: Z axis)—default: 90°/270°
(perpendicular to Z-axis)
Q: Type of retraction after machining—default: 0
■ Q=0: Return to starting point (first in X direction, then in Z)
■ Q=1: Position in front of finished contour
■ Q=2: Move to clearance height and stop
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)
D: Omit element (influences the machining of undercuts, relief
turns: see table)—default: 0
D G22 G23 G23 G25 G25 G25
= H0 H1 H4 H5/6 H7..9
0 • • • • • •
1 • • • – – –
2 • • – • • •
3 • • – – – –
4 • • – • • –
”•”: Skip elements
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
1 Calculate the areas to be machined and the
cutting segmentation (infeeds).
2 Approach workpiece for first pass from starting
point, taking the safety clearance into account.
3 Execute the first cut (roughing).
4 Approach for the next pass and execute the next
cut (roughing) in the opposite direction.
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 Retract as programmed in ”Q.”