HEIDENHAIN TNC 320 (34055x-06) ISO programming - Manual (Page 205)

Programming examples 7.6
7
TNC 320 | User's Manual for DIN/ISO Programming | 5/2013
205
7.6 Programming examples
Example: Milling a contour in several infeeds
Program sequence:
Pre-position the tool to the workpiece surface
Enter the infeed depth in incremental values
Contour milling
Repeat infeed and contour-milling
%PGMREP 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 I+50 J+50 *
Set pole
N60 G10 R+60 H+180 * Pre-position in the working plane
N70 G01 Z+0 F1000 M3 * Pre-position to the workpiece surface
N80 G98 L1 *
Set label for program section repeat
N90 G91 Z-4 * Infeed depth in incremental values (in space)
N100 G11 G41 G90 R+45 H+180 F250 *
First contour point
N110 G26 R5 * Contour approach
N120 H+120 *
N130 H+60 *
N140 H+0 *
N150 H-60 *
N160 H-120 *
N170 H+180 *
N180 G27 R5 F500 *
Contour departure
N190 G40 R+60 H+180 F1000 * Retract tool
N200 L1,4 * Return jump to label 1; section is repeated a total of 4 times
N200 G00 Z+250 M2 *
Retract the tool, end program
N99999999 %PGMWDH G71 *