HEIDENHAIN TNC 426, User Manual

Page: 379 / 502

HEIDENHAIN TNC 426, TNC 430 353
9.6 Pr
ogr
amming Examples
Example: Groups of holes with several tools
Program sequence
n
Program the fixed cycles in the main program
n
Call the entire hole pattern (subprogram 1)
n
Approach the groups of holes in subprogram 1,
call group of holes (subprogram 2)
n
Program the group of holes only once in
subprogram 2
0 BEGIN PGM UP2 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z-20
2 BLK FORM 0.2 X+100 Y+100 Z+0
3 TOOL DEF 1 L+0 R+4 Define tool: center drill
4 TOOL DEF 2 L+0 R+3 Define tool: drill
5 TOOL DEF 3 L+0 R+3.5 Define tool: reamer
6 TOOL CALL 1 Z S5000 Call tool: center drill
7 L Z+250 R0 F MAX Retract the tool
8 CYCL DEF 200 DRILLING Cycle definition: Centering
Q200=2 ; SET-UP CLEARANCE
Q201=-3 ; DEPTH
Q206=250 ; FEED RATE FOR PLNGNG
Q202=3 ; PLUNGING DEPTH
Q210=0 ; DWELL TIME AT TOP
Q203=+0 ; SURFACE COORDINATE
Q204=10 ; 2ND SET-UP CLEARANCE
Q211=0.25 ; DWELL TIME AT BOTTOM
9 CALL LBL 1 Call subprogram 1 for the entire hole pattern
X
Y
15
60
100
100
75
10
45
20
20
5
Z
Y
-20
-15
1 2
1 1 3 1