HEIDENHAIN TNC 620 (73498x-01) ISO programming - Manual (Page 182)

182 Programming: Programming contours
6.4 P
a
th cont
ours—Car
te
sian coor
dinat
e
s
Example: Linear movements and chamfers with Cartesian coordinates
%LINEAR G71 *
N10 G30 G17 X+0 Y+0 Z-20 * Define blank form for graphic workpiece simulation
N20 G31 G90 X+100 Y+100 Z+0 *
N30 T1 G17 S4000 * Call tool in the spindle axis and with the spindle speed S
N40 G00 G40 G90 Z+250 * Retract tool in the spindle axis at rapid traverse
N50 X-10 Y-10 * Pre-position the tool
N60 G01 Z-5 F1000 M3 * Move to working depth at feed rate F = 1000 mm/min
N70 G01 G41 X+5 Y+5 F300 * Approach the contour at point 1, activate radius compensation G41
N80 G26 R5 F150 * Tangential approach
N90 Y+95 * Move to point 2
N100 X+95 * Point 3: first straight line for corner 3
N110 G24 R10 * Program chamfer with length 10 mm
N120 Y+5 * Point 4: 2nd straight line for corner 3, 1st straight line for corner 4
N130 G24 R20 * Program chamfer with length 20 mm
N140 X+5 * Move to last contour point 1, second straight line for corner 4
N150 G27 R5 F500 * Tangential exit
N160 G40 X-20 Y-20 F1000 * Retract tool in the working plane, cancel radius compensation
N170 G00 Z+250 M2 * Retract in the tool axis, end program
N99999999 %LINEAR G71 *
X
Y
9 5
95
5
10
10
20
20
1 4
2
3