HEIDENHAIN TNC 320 User Manual page 311

Example: Group of holes with several tools
Program run:
Program the fixed cycles in the main program
Call the complete hole pattern (subprogram 1) in the
main program
Approach the groups of holes (subprogram 2) in
subprogram 1
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 CALL 1 Z S5000
4 L Z+250 R0 FMAX
5 CYCL DEF 200 DRILLING
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 DEPTH
Q395=0 ;DEPTH REFERENCE
6 CALL LBL 1
7 L Z+250 R0 FMAX
8 TOOL CALL 2 Z S4000
9 FN 0: Q201 = -25
10 FN 0: Q202 = +5
11 CALL LBL 1
12 L Z+250 R0 FMAX
13 TOOL CALL 3 Z S500
HEIDENHAIN | TNC 320 | Conversational Programming User's Manual | 9/2016
Programming examples
Centering drill tool call
Retract the tool
Cycle definition: CENTERING
Call subprogram 1 for the entire hole pattern
Drill tool call
New depth for drilling
New plunging depth for drilling
Call subprogram 1 for the entire hole pattern
Reamer tool call
8
8.6
311