HEIDENHAIN TNC 620 Programming Station, Руководство пользователя

Страница: 249 / 695

Approaching and departing a contour 6.3
6
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
249
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 have programmed the coordinates of all three principal axes
X, Y and Z in the approach block, the TNC moves the tool from the
position defined before the APPR block to the auxiliary point P
H
on
all three axes simultaneously. Then the TNC 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.
Please note that earlier programs may need to be
adapted.
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