HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 214)

Programming: Programming contours
6.3 Approaching and departing a contour
6
214
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
Polar coordinates
You can also program the contour points for the following approach/
departure functions over polar coordinates:
APPR LT becomes APPR PLT
APPR LN becomes APPR PLN
APPR CT becomes APPR PCT
APPR LCT becomes APPR PLCT
DEP LCT becomes DEP PLCT
Select by soft key an approach or departure function, then press
the orange P key.
Radius compensation
The tool radius compensation is programmed together with
the first contour point P
A
in the APPR block. The DEP blocks
automatically discard the tool radius compensation.
If you program APPR LN or APPR CT with G40, the
control stops the machining/simulation with an error
message.
This method of function differs from the iTNC 530
control!
Approaching on a straight line with tangential
connection:
APPR LT
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 straight line that connects tangentially to the contour. The
auxiliary point P
H
is separated from the first contour point P
A
by the
distance LEN.
Use any path function to approach the starting point P
S
.
Initiate the dialog with the APPR/DEP key and APPR LT soft key:
Coordinates of the first contour point P
A
LEN: Distance from the auxiliary point P
H
to the
first contour point P
A
Radius compensation G41/G42 for machining
R0=G40; RL=G41; RR=G42
Example NC blocks
N70 G00 X+40 Y+10 G40 M3 Approach P
S
without radius compensation
N80 APPR LT X+20 Y+20 Z-10 LEN15 G42 F100 P
A
with radius comp. G42, distance P
H
to P
A
: LEN=15
N90 G01 X+35 Y+35 End point of the first contour element
N100 G01 ... Next contour element