HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 215)

HEIDENHAIN CNC PILOT 4290 215
4.20 Cont
our
-Based T
u
rn
ing Cy
cles
Use as 4 axis cycle
„ Same diameter: Both slides start simultaneously.
„ Differing 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 surface 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.
Face roughing G820
G820 machines the contour area from NS to NE defined by NS, NE. If
required, the area to be machined is divided into several sections
(example: with contour valleys).
On 4 axis cycles, ensure that the tools are identical (tool
type, cutting edge radius, cutting edge angle, etc.).
0
2
H
1
X Z
A
–W
P
K
Z
I Ø
Parameters
NS Starting block number (beginning of contour section)
NE End block number (end of contour section)
„ NE not programmed: The contour element NS is machined
in the direction of contour definition.
„ NS=NE programmed: The contour element NS is machined
opposite to the direction of contour definition.
P Maximum infeed
I Oversize in X direction (diameter value) – (default: 0)
K Oversize in Z direction (default: 0)
E Plunging behavior
„ E=0: Descending contours are not machined.
„ E>0: Plunging feed rate
„ No input: Feed rate reduction depending on the plunge
angle – maximum 50%
X Cutting limit in X direction (diameter value) – (default: no
cutting limit)
Z Cutting limit in Z direction (default: no cutting limit)
H Type of departure (default: 0)
„ H=0: Machines contour outline after each pass
„ H=1: Retracts at 45°; contour smoothing after last pass
„ H=2: Retracts at 45° – no contour smoothing
A Approaching angle (reference: Z-axis) – (default: 90°/270°;
perpendicular to Z-axis)