Yx z – HEIDENHAIN TNC 407 (280 580) ISO Programming User Manual
Page 156
5 - 2 3
TNC 426/TNC 425/TNC 415 B/TNC 407
5
Programming Tool Movements
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 the 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 and insert tool
N60 X+25 Y–30 * ....................................................... Pre-position in the working plane
N70 Z–18 M03 * ........................................................ Move tool to working depth
N80 G01 G42 X+0 Y+0 F100 * .................................. Approach the contour with radius compensation at
machining feed rate
N90 G02 X+100 Y+0 R–50 * ...................................... Mill arc to end point X = 100mm, Y = 0;
radius = 50mm, direction of rotation negative
N100 G00 G40 X+70 Y–30 * ...................................... Depart the contour, cancel radius compensation
N110 Z+100 M02 * .................................................... Retract in the infeed axis
N99999 %S523I G71 *