Contour Programming - HEIDENHAIN CNC PILOT 640 User Manual

4

Contour programming

The blank form update function and contour-related turning cycles
require the previous description of the blank and finished part. For
milling and drilling, contour definition is a precondition if you wish to
use fixed cycles.
Use ICP (Interactive Contour Programming) for describing
blank and finished parts.
Contours for turning:
Describe a continuous contour
The direction of the contour description is independent of the
direction of machining
Contour descriptions must not extend beyond the turning center
The contour of the finished part must lie within the contour of the
blank part
When machining bars, define only the required section as blank
Contour definitions apply to the entire NC program, even if the
workpiece is rechucked for machining the rear face
In the fixed cycles, the defined contour is used to program
reference values
To describe workpiece blanks
G20 "Blank part macro" for standard parts (cylinder, hollow
cylinder)
G21 "Cast-part macro" for blank-part contours based on finished-
part contours G21 is only used for describing workpiece blanks
Individual contour elements (such as are used for finished-part
contours) where use of G20 or G21 is not possible
To describe finished parts, use individual contour elements and
form elements. The contour elements or the complete contour
can be assigned attributes accounted for during the machining of
the workpiece (example: oversizes, additive compensation, special
feed rates, etc.). The control always uses paraxial elements to close
finished parts.
For intermediate machining steps, define auxiliary contours. Auxiliary
contours (TEMPORARY) are programmed in the same way as
finished-part descriptions. One contour description is possible
per TEMPORARY. A TEMPORARY is assigned a name (ID) that can
be referenced by the cycles. Auxiliary contours are not closed
automatically.
Contours for C-axis machining:
Contours for C-axis machining are programmed within the
FINISHED PART section.
Identify the contours as FRONT or LATERAL. You can use section
codes more than once or program multiple contours within one
section code
234
and auxiliary workpiece
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017
DIN/ISO programming | Programming in ISO Mode
blanks, use: