HEIDENHAIN TNC 640 (34059x-01) - Manual (Page 210)

210 Programming: Programming Contours
6.5 P
a
th Cont
ours—P
o
lar Coor
dinat
e
s
Example: Linear movement with polar coordinates
0 BEGIN PGM LINEARPO MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Definition of workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S4000 Tool call
4 CC X+50 Y+50 Define the datum for polar coordinates
5 L Z+250 R0 FMAX Retract the tool
6 LP PR+60 PA+180 R0 FMAX Pre-position the tool
7 L Z-5 R0 F1000 M3 Move to working depth
8 APPR PLCT PR+45 PA+180 R5 RL F250 Approach the contour at point 1 on a circular arc with tangential
connection
9 LP PA+120 Move to point 2
10 LP PA+60 Move to point 3
11 LP PA+0 Move to point 4
12 LP PA-60 Move to point 5
13 LP PA-120 Move to point 6
14 LP PA+180 Move to point 1
15 DEP PLCT PR+60 PA+180 R5 F1000 Depart the contour on a circular arc with tangential connection
16 L Z+250 R0 FMAX M2 Retract in the tool axis, end program
17 END PGM LINEARPO MM
X
Y
50 100
50
CC
5
100
R45
60°
5
4 1
2
6 5
3