Face Roughing G820 - HEIDENHAIN CNC PILOT 640 User Manual

4

Face roughing G820

G820 machines the defined contour area. The reference to the
contour to be machined can be transferred in the cycle parameters,
or the contour can be defined directly after the cycle call.
Further information:
The contour to be machined can contain various valleys. If required,
the area to be machined is divided into several sections.
Parameters:
ID: Auxiliary contour – ID number of the contour to be machined
NS: Starting block no. of contour – beginning of contour section
NE: Contour end block no. – 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: O-size X
K: O-size Z
E: Plunging behavior
No input: Automatic feed-rate reduction
E = 0: No plunging
E > 0: Plunging feed rate in use
X: Cutting limit in X (diameter value; default: no cutting limit)
Z: Cutting limit in Z (default: no cutting limit)
A: Start angle (reference: Z axis; default: orthogonal to Z axis)
W: Depart.angle (reference: Z axis; default: parallel to Z axis)
H: Contour smoothing
0: With each cut
1: With the last cut
2: No smoothing
Q: Kind of liber. at end of cycle
0: Back to beg., X before Z
1: Before finished contour
2: Retract by safety clear.
V: Machine form elements (default: 0)
A chamfer/rounding arc is machined
0: At beginning and end
1: At beginning
2: At end
3: No machining
4: Only chamfer/rounding is machined—not the base
element (requirement: the contour section consists of a single
element)
D: Omit elements (see figure)
U: Cut line on horiz. element
0: No (uniform cutting segmentation)
1: Yes (irregular cutting segmentation if applicable)
320
"Working with contour-based cycles", Page 315
DIN/ISO programming | Contour-based turning cycles
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017