Contour-Parallel Roughing G830 - HEIDENHAIN CNC PILOT 640 User Manual

DIN/ISO programming | Contour-based turning cycles

Contour-parallel roughing G830

G830 machines the contour area defined in ID, or by NS, NE, parallel
to the contour.
Further information: "Working with contour-based cycles", Page 315
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
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: parallel to Z axis, or with
facing tools: parallel to X axis)
W: Depart.angle (reference: Z axis; default: orthogonal to Z axis,
or with facing tools: orthogonal to X axis)
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)
B: Contour calculation
0: Automatic
1: Tool left (G41)
2: Tool right(G42)
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
4
323