HEIDENHAIN SW 54843x-02 DIN Programming - Manual (Page 272)

272 DIN programming
4.1
7
Cont
our
-based t
u
rn
ing cy
cles
The control uses the tool definition to distinguish between external
and internal machining.
Parameters
B
Contour calculation
 0: Automatic
 1: Tool to the left (G41)
 2: Tool to the right (G42)
D Omit elements (see figure)
J aß (radius value)—active only if no blank has been defined.
H Contour-parallel—Type of cutting paths:
 0: Constant machining depth
 1: Equidistant cut lines
XA, ZA Starting point of blank (only effective if no blank was
programmed):
 XA, ZA not programmed: The workpiece blank contour is
calculated from the tool position and the ICP contour.
 XA, ZA programmed: Definition of the corner point of the
workpiece blank.
 The tool radius compensation is active.
 A G57 oversize enlarges the contour (also inside
contours).
 A G58 oversize
 >0: Enlarges the contour
 <0: Is not offset
 G57/G58 oversizes are deleted after cycle end.
Cycle run
1
Calculates the areas to be machined and the cutting
segmentation.
2 Approaches workpiece for first pass from starting point, taking
the safety clearance into account.
3 Executes the first cut (roughing).
4 Approaches for the next pass and execute the next cut (roughing)
in the opposite direction.
5 Repeats 3 to 4 until the complete area has been machined.
6 If required, repeats 2 to 5 until all areas have been machined.
7 Retracts as programmed in Q.