HEIDENHAIN TNC 360 ISO Programming - Manual (Page 181)

8-28
8 Cycles
TNC 360
8.3 SL Cycles
Example: Overlapping pockets with islands
Inside machining with pilot drilling, roughing out
and finishing.
PGM S829I is based on S824I:
The main program has been expanded by the
cycle definitions and cycle calls for pilot drilling
and finishing.
The contour subprograms 1 to 4 are identical to
those in PGM S824I (see page 8-24) and are
added after block N300.
%S829I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * ................................... Define workpiece blank
N20 G31 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+2.5 * ........................................... Tool definition drill
N40 G99 T2 L+0 R+3 * .............................................. Tool definition rough mill
N50 G99 T3 L+0 R+2.5 * ........................................... Tool definition finish mill
N60 L10,0 * ................................................................ Subprogram call for tool change
N70 G38 M06 * .......................................................... Stop program run
N80 T1 G17 S2500 * .................................................. Tool call drill
N90 G37 P01 1 P02 2 P03 3 P04 4 * .......................... Cycle definition CONTOUR GEOMETRY
N100 G56 P01 –2 P02 –10 P03 –5 P04 500 P05 +2 * .. Cycle definition PILOT DRILLING
N110 Z+2 M03 *
N120 G79 * ................................................................ Cycle call PILOT DRILLING
N130 L10,0 *
N140 G38 M06 * ........................................................ Tool change
N150 T2 G17 S1750 * ................................................ Tool call rough mill
N160 G57 P01 –2 P02 –10 P03 –5 P04 100 P05+2
P06+0 P07 500 * ........................................................ Cycle definition ROUGH-OUT
N170 Z+2 M03 *
N180 G79 * ................................................................ Cycle call ROUGH-OUT
N190 L10,0 *
N200 G38 M06 * ........................................................ Tool change
N210 T3 G17 S2500 * ................................................ Tool call finish mill
N220 G58 P01 –2 P02 –10 P03 –10 P04 100
P05 500 * ................................................................... Cycle definition CONTOUR MILLING
N230 Z+2 M03 *
N240 G79 * ................................................................ Cycle call CONTOUR MILLING
N250 Z+100 M02 *
N260 G98 L10 * ......................................................... Subprogram for tool change
N270 T0 G17 *
N280 G00 G40 G90 Z+100 *
N290 X–20 Y–20 *
N300 G98 L0 *
From block N310: add the subprograms listed on page 8-24
N9999 %S829I G71 *