HEIDENHAIN TNC 620 Programming Station

Programming contours | Approaching and departing a contour
Approaching on a circular path with tangential connection
from a straight line to the contour: APPR LCT
The tool moves on a straight line from the starting point P
S
to
an auxiliary point P
H
. It then moves to the first contour point P
A
on a circular arc. The feed rate programmed in the APPR block
is effective for the entire path that the control traversed in the
approach block (path P
S
to P
A
).
If you have programmed the coordinates of all three principal axes
X, Y and Z in the approach block, the control moves the tool from the
position defined before the APPR block to the auxiliary point P
H
on all
three axes simultaneously. Then the control moves the tool from P
H
to P
A
only in the working plane.
The arc is connected tangentially both to the line P
S
- P
H
as well as
to the first contour element. Once these lines are known, the radius
then suffices to completely define the tool path.
Use any path function to approach the starting point P
S
.
Initiate the dialog with the APPR DEP key and APPR LCT soft
key:
Coordinates of the first contour point P
A
Radius R of the circular arc. Enter R as a positive
value
Radius compensation RR/RL for machining
Example
7 L X+40 Y+10 R0 FMAX M3
Approach P
S
without radius compensation
8 APPR LCT X+10 Y+20 Z-10 R10 RR F100
P
A
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
5
HEIDENHAIN | TNC620 | Klartext Programming User's Manual | 01/2022
151