HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 250
8-30
8
Cycles
TNC 426/TNC 425/TNC 415 B/TNC 407
Example: Overlapping pockets with islands
Inside machining with pilot drilling, roughing-out
and finishing.
PGM S829I is based on S824I:
The main program section is expanded by the
cycle definitions and calls for pilot drilling and
finishing.
The contour subprograms 1 to 4 are identical to
the ones in PGM S824I (see page 8-26) and
are to be added after block N300.
%S829I G71 * ............................................................ Start of 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 bit
N40 G99 T2 L+0 R+3 * .............................................. Tool definition: roughing mill
N50 G99 T3 L+0 R+2.5 * ........................................... Tool definition: finishing mill
N60 L10,0 * ................................................................ Subprogram call for tool change
N70 G38 M06 * .......................................................... Program STOP
N80 T1 G17 S2500 * .................................................. Tool call: drill bit
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: roughing 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: finishing 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 subprograms on page 8-26
N99999 %S829I G71 *