HEIDENHAIN TNC 620 (81760x-02) ISO programming - Manual (Page 284)

Programming: Subprograms and program section repeats
8.6 Programming examples
8
284
TNC 620 | User's ManualDIN/ISO Programming | 2/2015
Example: Groups of holes
Program sequence:
Approach the groups of holes in the main program
Call the group of holes (subprogram 1) in the main
program
Program the group of holes only once in subprogram
1
%SP1 G71 *
N10 G30 G17 X+0 Y+0 Z-40 *
N20 G31 G90 X+100 Y+100 Z+0 *
N30 T1 G17 S3500 *
Tool call
N40 G00 G40 G90 Z+250 * Retract the tool
N50 G200 Define the DRILLING cycle
Q200=2 ;SET-UP CLEARANCE
Q201=-30 ;DEPTH
Q206=300 ;FEED RATE FOR PLNGNG
Q202=5 ;
Q210=0 ;DWELL TIME AT TOP
Q203=+0 ;SURFACE COORDINATE
Q204=2 ;2ND SET-UP CLEARANCE
Q211=0 ;DWELL TIME AT DEPTH
Q395=0 ;
N60 X+15 Y+10 M3 * Move to starting point for group 1
N70 L1,0 * Call the subprogram for the group
N80 X+45 Y+60 * Move to starting point for group 2
N90 L1,0 * Call the subprogram for the group
N100 X+75 Y+10 * Move to starting point for group 3
N110 L1,0 * Call the subprogram for the group
N120 G00 Z+250 M2 * End of main program
N130 G98 L1 * Beginning of subprogram 1: Group of holes
N140 G79 * Call cycle for 1st hole
N150 G91 X+20 M99 * Move to 2nd hole, call cycle
N160 Y+20 M99 * Move to 3rd hole, call cycle
N170 X-20 G90 M99 * Move to 4th hole, call cycle
N180 G98 L0 * End of subprogram 1