HEIDENHAIN TNC 620 User Manual page 319

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*
N40 G00 G40 G90 Z+250*
N50 I+50 J+50*
N60 G10 R+60 H+180*
N70 G01 Z+0 F1000 M3*
N80 G98 L1*
N90 G91 Z-4*
N100 G11 G41 G90 R+45 H+180 F250*
N110 G26 R5*
N120 H+120*
N130 H+60*
N140 H+0*
N150 H-60*
N160 H-120*
N170 H+180*
N180 G27 R5 F500*
N190 G40 R+60 H+180 F1000*
N200 L1,4*
N200 G00 Z+250 M2*
N99999999 %PGMWDH G71 *
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Programming examples
Tool call
Retract the tool
Set pole
Pre-position in the working plane
Pre-position to the workpiece surface
Set label for program section repeat
Infeed depth in incremental values (in space)
First contour point
Contour approach
Contour departure
Retract tool
Return jump to label 1; section is repeated a total of 4 times
Retract the tool, end program
8
8.6
319