HEIDENHAIN TNC 320, User Manual

Page: 192 / 581

Programming: Programming contours
6.3 Approaching and departing a contour
6
192
TNC 320 | User's Manual
HEIDENHAIN Conversational Programming | 3/2014
Approaching on a circular path with tangential
connection:
APPR CT
The tool moves on a straight line from the starting point P
S
to an
auxiliary point P
H
. It then moves from PH to the first contour point
PA following a circular arc that is tangential to the first contour
element.
The arc from P
H
to P
A
is determined through the radius R and
the center angle
CCA
. The direction of rotation of the circular arc
is automatically derived from the tool path for the first contour
element.
Use any path function to approach the starting point P
S
.
Initiate the dialog with the APPR/DEP key and APPR CT soft key:
Coordinates of the first contour point P
A
Radius R of the circular arc
If the tool should approach the workpiece in the
direction defined by the radius compensation:
Enter R as a positive value
If the tool should approach from the workpiece
side: Enter R as a negative value.
Center angle CCA of the arc
CCA can be entered only as a positive value.
Maximum input value 360°
Radius compensation RR/RL for machining
Example NC blocks
7 L X+40 Y+10 R0 FMAX M3 Approach PS without radius compensation
8 APPR CT X+10 Y+20 Z-10 CCA180 R+10 RR F100
PA with radius compensation RR, radius R=10
9 L X+20 Y+35 End point of the first contour element
10 L ...
Next contour element