HEIDENHAIN TNC 320 (340 551-02) - Manual (Page 157)

HEIDENHAIN TNC 320 157
6.6 P
a
th Cont
ours—FK F
ree Cont
our Pr
ogr
a
mming
Example: FK programming 1
0 BEGIN PGM FK1 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20 Define the workpiece blank
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+10 Define the tool
4 TOOL CALL 1 Z S500 Tool call
5 L Z+250 R0 FMAX Retract the tool
6 L X-20 Y+30 R0 FMAX Pre-position the tool
7 L Z-10 R0 F1000 M3 Move to working depth
8 APPR CT X+2 Y+30 CCA90 R+5 RL F250 Approach the contour on a circular arc with tangential connection
9 FC DR- R18 CLSD+ CCX+20 CCY+30 FK contour section:
10 FLT Program all known data for each contour element
11 FCT DR- R15 CCX+50 CCY+75
12 FLT
13 FCT DR- R15 CCX+75 CCY+20
14 FLT
15 FCT DR- R18 CLSD- CCX+20 CCY+30
16 DEP CT CCA90 R+5 F1000 Depart the contour on a circular arc with tangential connection
17 L X-30 Y+0 R0 FMAX
18 L Z+250 R0 FMAX M2 Retract in the tool axis, end program
19 END PGM FK1 MM
X
Y
100
100
20
75
30
50 20 75
R15
R18
R15