HEIDENHAIN CNC Pilot 4290 - Manual (Page 135)

HEIDENHAIN CNC PILOT 4290 123
4.7 T
u
rning Cy
cles
On 4 axis cycles, ensure that the tools
are identical (tool type, cutting edge
radius, cutting edge angle, etc.).
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
4 axis operation
■ When working on the same diameter, both slides
start simultaneously.
■ When working on different diameters, the second
slide starts when the leading slide has reached
“lead B.” This is synchronized at every step.
Each slide advances by the calculated depth of
cut. If the slides do not have to execute the same
number of cuts, the leading slide executes the
last cut.
With “constant cutting speed,” the cutting speed
depends on the speed of the leading slide. The
leading tool does not retract until the subsequent
tool is ready for use.
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
B: Slide lead for 4-axis machining
■ B=0: Both slides work on the same diameter—with double
feed rate
■ B<>0: Distance to “leading” slide (the lead). The slides
work on different diameters with the same feed rate.
■ B<0: The slide with larger number leads.
■ B>0: The slide with smaller number leads.