HEIDENHAIN TNC 320 - 8.6 Programming examples; Example: Milling a contour in several infeeds

Subprograms and Program Section Repeats | Programming examples
8
332
HEIDENHAIN | TNC 320 | ISO Programming User's Manual | 10/2017
8.6 Programming examples
Example: Milling a contour in several infeeds
Program run:
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 *