HEIDENHAIN iTNC 530 (60642x-04) ISO programming - Manual (Page 240)

240 Programming: Programming Contours
6.5
Pa
th
cont
ours—P
olar
coor
dinat
es Example: Helix
%HELIX G71 *
N10 G30 G17 X+0 Y+0 Z-20 * Definition of workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N40 T1 G17 S1400 * Tool call
N50 G00 G40 G90 Z+250 * Retract the tool
N60 X+50 Y+50 * Pre-positioning the tool
N70 G29 * Transfer the last programmed position as the pole
N80 G01 Z-12.75 F1000 M3 * Move to working depth
N90 G11 G41 R+32 H+180 F250 * Approach first contour point
N100 G26 R2 * Connection
N110 G13 G91 H+3240 Z+13.5 F200 * Helical traverse
N120 G27 R2 F500 * Tangential exit
N170 G01 G40 G90 X+50 Y+50 F1000 * Retract the tool, end program
N180 G00 Z+250 M2 *
X
Y
50
50
CC
100
100
M64 x 1,5