HEIDENHAIN TNC 426, User Manual

Page: 380 / 502

354 9 Programming: Subprograms and Program Section Repeats
9.6 Pr
ogr
amming Examples
10 L Z+250 R0 F MAX M6 Tool change
11 TOOL CALL 2 Z S4000
Call the drilling tool
12 FN 0: Q201 = -25 New depth for drilling
13 FN 0: Q202 = +5
New plunging depth for drilling
14 CALL LBL 1 Call subprogram 1 for the entire hole pattern
15 L Z+250 R0 F MAX M6
Tool change
16 TOOL CALL 3 Z S500 Tool call: reamer
17 CYCL DEF 201 REAMING
Cycle definition: REAMING
Q200=2 ; SET-UP CLEARANCE
Q201=-15 ; DEPTH
Q206=250 ; FEED RATE FOR PLNGNG
Q211=0.5 ; DWELL TIME AT DEPTH
Q208=400 ; RETRACTION FEED RATE
Q203=+0 ; SURFACE COORDINATE
Q204=10 ; 2ND SET-UP CLEARANCE
18 CALL LBL 1
Call subprogram 1 for the entire hole pattern
19 L Z+250 R0 F MAX M2 End of main program
20 LBL 1 Beginning of subprogram 1: Entire hole pattern
21 L X+15 Y+10 R0 F MAX M3
Move to starting point for group 1
22 CALL LBL 2 Call subprogram 2 for the group
23 L X+45 Y+60 R0 F MAX
Move to starting point for group 2
24 CALL LBL 2 Call subprogram 2 for the group
25 L X+75 Y+10 R0 F MAX
Move to starting point for group 3
26 CALL LBL 2 Call subprogram 2 for the group
27 LBL 0
End of subprogram 1
28 LBL 2
Beginning of subprogram 2: Group of holes
29 CYCL CALL 1st hole with active fixed cycle
30 L IX+20 R0 F MAX M99
Move to 2nd hole, call cycle
31 L IY+20 R0 F MAX M99 Move to 3rd hole, call cycle
32 L IX-20 R0 F MAX M99
Move to 4th hole, call cycle
33 LBL 0 End of subprogram 2
34 END PGM UP2 MM