HEIDENHAIN TNC 360 ISO Programming - Manual (Page 108)

5-25 TNC 360
5 Programming Tool Movements
5.4 Path Contours - Cartesian Coordinates
Example for exercise: Circular arc connecting to a straight line
Coordinates of the
transition point from
the line to the arc:
X = 10 mm
Y = 40 mm
Coordinates of the
arc end point:
X = 50 mm
Y = 50 mm
Milling depth: Z = –15 mm
Tool radius: R = 20 mm
100
–15
100 40
50
10
50
Y
X
Z
90
Part program
%S525I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * .................................. Define workpiece blank
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T12 L-25 R+20 * ......................................... Define the tool
N40 T12 G17 S1000 * ................................................ Call the tool
N50 G00 G40 G90 Z+100 M06 * ............................... Retract the spindle and insert the tool
N60 X+30 Y–30 * ....................................................... Pre-position in X, Y
N70 Z–15 M03 * ........................................................ Pre-position to the working depth
N80 G01 G41 X+50 Y+0 F100 * ................................ Move with radius compensation and reduced
feed to the first contour point
N90 X+10 Y+40 * ...................................................... Straight line connecting tangentially to the arc
N100 G06 X+50 Y+50 *
Arc to end point with coordinates X = 50 and Y = 50;
connects tangentially to the straight line in block N90
N110 G01 X+100 * .................................................... End of contour
N120 G00 G40 X+130 Y+70 * ................................... Retract the tool in X, Y; cancel radius compensation
N130 Z+100 M02 * .................................................... Retract the tool in Z
N9999 %S525I G71 *