HEIDENHAIN TNC 407 (280 580) ISO Programming - Manual (Page 256)

8-36
8 Cycles
TNC 426/TNC 425/TNC 415 B/TNC 407
8.4 SL Cycles (Group II)
Part program
%S835I G71 * ............................................................ Start of program
N10 G30 G17 X+0 Y+0 Z–20 * ................................... Define workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+3 * .............................................. Define tools
N40 G99 T2 L+0 R+2.5 *
N50 G99 T3 L+0 R+2.5 *
N60 G37 P01 1 P02 2 * .............................................. Cycle definition: Contour Geometry
N70 G120 Q1=–15 Q2=1 Q3=+1 Q4=+1 Q5=+0
Q6=–2 Q7=+50 Q8=+10 Q9=+1 * ............................ Cycle definition: Contour Data
N80 L10,0 * ................................................................ Call subprogram for tool change
N90 T1 G17 S2500 *
N100 G121 Q10=–10 Q11=100 Q13=2 * .................. Cycle definition: Pilot Drilling
N110 G79 M3 * .......................................................... Cycle call: Pilot Drilling
N120 L10,0 * .............................................................. Call subprogram for tool change
N130 T2 G17 S1500 *
N140 G122 Q10=–10 Q11=100 Q12=500 * .............. Cycle definition: Rough-Out
N150 G79 M3 * .......................................................... Cycle call: Rough-Out
N160 L10,0 * .............................................................. Call subprogram for tool change
N170 T3 G17 S3000 *
N180 G123 Q11=80 Q12=250 * ................................ Cycle definition: Floor Finishing
N190 G79 M3 * .......................................................... Cycle call: Floor Finishing
N200 G124 Q9=+1 Q10=–5 Q11=100 Q12=240
Q14=+0 * ................................................................... Cycle definition: Side Finishing
N210 G79 M3 * .......................................................... Cycle call: Side Finishing
N220 G00 G40 Z+100 M2 *
N230 G98 L10 * ......................................................... Subprogram for tool change
N240 T0 G17 *
N250 G00 G40 G90 Z+100 *
N260 X–20 Y–20 M6 *
N270 G98 L0 *
N280 G98 L1 * ........................................................... Contour subprogram: Rectangular Pocket
N290 G01 G42 X+10 Y+50 *
N300 Y+90 *
N310 X+90 *
N320 Y+10 *
N330 X+10 *
N340 Y+50 *
N350 G98 L0 *
N360 G98 L2 * ........................................................... Contour subprogram: Circular Island
N370 G01 G41 X+35 Y+50 *
N380 I+50 J+50 *
N390 G02 X+35 Y+50 *
N400 G98 L0 *
N99999 %S835I G71 *