DIN/ISO programming | Contour-based turning cycles
4
324
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
H: Type of cut lines
0: Constant mach.depth – contour is shifted by a constant
infeed value (paraxial)
1: Equidistant cut lines – cutting lines run at a constant
distance from the contour (contour-parallel). The contour is
scaled.
RH: Wrkpc. blank contour – evaluation only if no workpiece blank
has been defined
0: (depends on defined parameters)
No parameters: workpiece blank from ICP contour and tool
position
XA and ZA: workpiece blank from ICP contour and starting
point of workpiece blank
J: workpiece blank from ICP contour and equidistant
oversize
1: From tool position (workpiece blank from ICP contour and
tool position)
2: With blank start point (workpiece blank from ICP contour
and starting point of workpiece blank XA and ZA)
3 Equidistant oversize (workpiece blank from ICP contour and
equidistant oversize J)
4: Long.-transv. oversize (workpiece blank from ICP contour,
transverse oversize XA and longitudinal oversize ZA)
J: Workpiece blank oversize (radius value – active only if no
workpiece blank has been defined)
XA, ZA: Start point blank (definition of corner point of workpiece
blank contour – evaluation only if no workpiece blank has been
defined)
The control uses the tool definition to distinguish between external
and internal machining.
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 Returns at rapid traverse and approaches for next pass
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
To Next Page
Loading...
