HEIDENHAIN TNC 620 (81760x-02) ISO programming - Manual (Page 213)

Approaching and departing a contour 6.3
6
TNC 620 | User's ManualDIN/ISO Programming | 2/2015
213
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 TNC traversed in the approach
block (path P
S
to P
A
).
If you program all three principal axes X, Y and Z in the approach
block, the TNC initially traverses the tool from the starting point P
S
in the working plane, and then in the tool axis on the auxiliary point
P
H
. The control only traverses the tool in the working plane from
auxiliary point P
H
to the contour point P
A
.
Consider this behavior when importing programs
from earlier controls. Adapt the program if required.
Earlier controls traverse the auxiliary point P
H
in all
three principal axes simultaneously.
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
G41/G42 for machining
R0=G40; RL=G41; RR=G42
Example NC blocks
N70 G00 X+40 Y+10 G40 M3 Approach PS without radius compensation
N80 APPR LCT X+10 Y+20 Z-10 R10 G42 F100 PA with radius comp. G42, radius R=10
N90 G01 X+20 Y+35 End point of the first contour element
N100 G01 ... Next contour element