HEIDENHAIN TNC 360 ISO Programming - Manual (Page 106)

5-23 TNC 360
5 Programming Tool Movements
5.4 Path Contours - Cartesian Coordinates
Example for exercise: Milling a concave semicircle
Semicircle radius: R = 50 mm
Coordinates of the
arc starting point:
X = 0
Y = 0
Coordinates of the
arc end point:
X = 100 mm
Y = 0
Tool radius: R = 25 mm
Milling depth: Z = –18 mm
–18
50
100
100
Y
X
Z
–20
Part program
%S523I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * .................................. Define the workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+25 * ............................................ Define the tool
N40 T1 G17 S780 * .................................................... Call the tool
N50 G00 G40 G90 Z+100 M06 * ............................... Retract the spindle and insert the tool
N60 X+25 Y-30 * ........................................................ Pre-position in X, Y
N70 Z–18 M03 * ........................................................ Pre-position to the working depth
N80 G01 G42 X+0 Y+0 F100 * .................................. Move with radius compensation and reduced feed to
the first contour point
N90 G02 X+100 Y+0 R–50 * ...................................... Mill circular arc to the end point X = 100, Y = 0;
radius = 50, negative direction of rotation
N100 G00 G40 X+70 Y–30 * ...................................... Retract the tool in X, Y; cancel radius compensation
N110 Z+100 M02 * .................................................... Retract the tool in Z
N9999 %S523I G71 *