HEIDENHAIN TNC 620 User Manual page 321

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
%SP2 G71 *
N10 G30 G17 X+0 Y+0 Z-40*
N20 G31 G90 X+100 Y+100 Z+0*
N30 T1 G17 S5000*
N40 G00 G40 G90 Z+250*
N50 G200 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=0.2 ;DWELL TIME AT DEPTH
Q395=0 ;DEPTH REFERENCE
N60 L1,0*
N70 G00 Z+250 M6*
N80 T2 G17 S4000*
N90 D0 Q201 P01 -25*
N100 D0 Q202 P01 +5*
N110 L1,0*
N120 G00 Z+250 M6*
N130 T3 G17 S500*
N140 G201 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
N150 L1,0*
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Programming examples
Centering drill tool call
Retract the tool
Define the CENTERING cycle
Call subprogram 1 for the entire hole pattern
Tool change
Drill tool call
New depth for drilling
New plunging depth for drilling
Call subprogram 1 for the entire hole pattern
Tool change
Reamer tool call
Cycle definition: REAMING
Call subprogram 1 for the entire hole pattern
8
8.6
321