HEIDENHAIN TNC 640, User Manual, Page: 295 / 948

Programming Contours | Approaching and departing a contour
7
HEIDENHAIN | TNC 640 | Conversational Programming User's Manual | 10/2017
295
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 connect goes from P
H
to
P
A
only on 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 PS without radius compensation
8 APPR LCT X+10 Y+20 Z-10 R10 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