HEIDENHAIN CNC Pilot 4290 V7.1 - Manual (Page 118)

118
4.2 Pr
ogr
a
mming Not
e
s
Contour programming
The “contour follow-up” 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.
Contours for turning
„ Describe a continuous contour.
„ The direction of the contour description is independent of the
direction of machining.
„ CNC PILOT closes open contours paraxially.
„ 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 blank parts, use
„ G20 “Blank part macro” for standard parts (cylinder, hollow
cylinder).
„ G21 “Cast-part macro” for blank-part contours based on finished-
part contours.
„ 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. The
contour elements or the complete contour can be assigned attributes
accounted for during the machining of the workpiece (example:
roughness, oversizes, etc.).
For intermediate machining steps, define auxiliary contours.
Auxiliary contours are programmed in the same way as finished-part
descriptions. One contour description is possible per AUXILIARY
CONTOUR. You can make multiple AUXILIARY CONTOURS.
Contours for C-axis machining:
„ Contours for C-axis machining are programmed within the
FINISHED PART section.
„ Identify the contours as a FRONT or SURFACE. You can use section
codes more than once or program multiple contours within one
section code.
Multiple contours in an NC program
The CNC PILOT supports up to four contours (workpiece blank and
finished part) per NC program. The CONTOUR section code
introduces the description. Parameters on zero point shift and the
coordinate system define the position of the contour in the working
space. A G99 in the machining section assigns the machining to a
contour.