HEIDENHAIN TNC 640 (34059x-02) - Manual (Page 273)

Programming examples 8.6
8
TNC 640 | User's Manual
HEIDENHAIN Conversational Programming | 5/2013
273
8.6 Programming examples
Example: Milling a contour in several infeeds
Program sequence:
Pre-position the tool to the workpiece surface
Enter the infeed depth in incremental values
Contour milling
Repeat infeed and contour-milling
0 BEGIN PGM PGMWDH MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-40
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL CALL 1 Z S500
Tool call
4 L Z+250 R0 FMAX Retract the tool
5 L X-20 Y+30 R0 FMAX
Pre-position in the working plane
6 L Z+0 R0 FMAX M3 Pre-position to the workpiece surface
7 LBL 1 Set label for program section repeat
8 L IZ-4 R0 FMAX
Infeed depth in incremental values (in space)
9 APPR CT X+2 Y+30 CCA90 R+5 RL F250 Contour approach
10 FC DR- R18 CLSD+ CCX+20 CCY+30
Contour
11 FLT
12 FCT DR- R15 CCX+50 CCY+75
13 FLT
14 FCT DR- R15 CCX+75 CCY+20
15 FLT
16 FCT DR- R18 CLSD- CCX+20 CCY+30
17 DEP CT CCA90 R+5 F1000
Contour departure
18 L X-20 Y+0 R0 FMAX
Retract tool
19 CALL LBL 1 REP 4 Return jump to LBL 1; section is repeated a total of 4 times
20 L Z+250 R0 FMAX M2 Retract the tool, end program
21 END PGM PGMWDH MM