Surface Y Section - HEIDENHAIN CNC PILOT 640 User Manual

1

SURFACE Y section

The section code identifies the YZ plane (G19). For machines
equipped with a B axis, it defines the tilted plane.
Without tilted plane:
position in the X direction; the C axis angle defines the position on
the workpiece.
Parameters:
X: Reference diameter
C: C axis angle – defines the spindle position
With tilted plane: SURFACE Y additionally performs the following
transformations and rotations for the tilted plane:
Shifts the coordinate system to the position I, K
Rotates the coordinate system by the Plane angle B; Plane ref.
in X, Plane ref. in Z: I, K
H=0: Shifts the rotated coordinate system by –I. The coordinate
system is moved back
Parameters:
X: Reference diameter
C: C axis angle – defines the spindle position
B: Plane angle (reference: positive Z axis)
I: Plane ref. in X (radius)
K: Plane ref. in Z
H: Automatic shift – automatic shift of the coordinate system
(default: 0)
0: Shift by -I – the rotated coordinate system is shifted by -I
1: Do not shift – the coordinate system is not shifted
Shifting back coordinate system:
reference diameter for the cutting limit. This value is also used
as the reference value for the depth that you program for drilling
operations and milling contours.
Since the Reference diameter is referenced to the current datum,
it is recommended when working in a tilted plane, to shift the
rotated coordinate system back by the distance –I. If the cutting
limits are not needed, for example for drilling holes, you can disable
the shift of the coordinate system (H=1) and set the Reference
diameter to 0.
Please note:
X is the infeed axis in a tilted coordinate system. X
coordinates are entered as diameter coordinates.
Mirroring the coordinate system has no effect on the
reference axis of the tilt angle (B axis angle of the
tool call)
66
The reference diameter defines the contour
The control evaluates the
NC programming | Program section code
HEIDENHAIN | User's Manual smart.Turn and DIN Programming | 12/2017