HEIDENHAIN TNC 640 (34059x-05) ISO programming - Manual (Page 289)

Programming examples 8.6
8
TNC 640 | User's ManualDIN/ISO Programming | 1/2015
289
Example: Group of holes with several tools
Program sequence:
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 *
Centering drill tool call
N40 G00 G40 G90 Z+250 * Retract the tool
N50 G200 DRILLING Define the CENTERING cycle
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 BOTTOM
N60 L1,0 * Call subprogram 1 for the entire hole pattern
N70 G00 Z+250 M6 * Tool change
N80 T2 G17 S4000 * Drill tool call
N90 D0 Q201 P01 -25 * New depth for drilling
N100 D0 Q202 P01 +5 * New plunging depth for drilling
N110 L1,0 * Call subprogram 1 for the entire hole pattern
N120 G00 Z+250 M6 * Tool change
N130 T3 G17 S500 * Reamer tool call
N140 G201 REAMING Cycle definition: REAMING
Q200=2 ;SET-UP CLEARANCE
Q201=-15 ;DEPTH
Q206=250 ;FEED RATE FOR PLNGNG
Q211=0.5 ;DWELL TIME AT BOTTOM
Q208=400 ;RETRACTION FEED RATE
Q203=+0 ;SURFACE COORDINATE
Q204=10 ;2ND SET-UP CLEARANCE
N150 L1,0 * Call subprogram 1 for the entire hole pattern
N160 G00 Z+250 M2 * End of main program