HEIDENHAIN TNC 360 ISO Programming - Manual (Page 103)

5-20
5 Programming Tool Movements
TNC 360
5.4 Path Contours - Cartesian Coordinates
Example for exercise: Milling a full circle in one block
Circle center: I = 50 mm
J = 50 mm
Beginning and end
of the circular arc:
X = 50 mm
Y = 0 mm
Milling depth: Z = – 5 mm
Tool radius: R = 15 mm
Part program
%S520I G71 * ............................................................ Begin program
N10 G30 G17 X+1 Y+1 Z–20 * .................................. Workpiece blank MIN point
N20 G31 G90 X+100 Y+100 Z+0 * ............................ Workpiece blank MAX point
N30 G99 T6 L+0 R+15 * ............................................ Tool definition
N40 T6 G17 S1500 * .................................................. Tool call
N50 G00 G40 G90 Z+100 M06 * ............................... Retract spindle and insert tool
N60 X+50 Y–40 * ....................................................... Pre-position in X, Y
N70 Z-5 M03 * ........................................................... Pre-position to the working depth
N80 I+50 J+50 * ........................................................ Coordinates of the circle center
N90 G01 G41 X+50 Y+0 F100 * ................................ Move with radius compensation and reduced feed to the
first contour point
N100 G26 R10 * ........................................................ Smooth (tangential) approach
N110 G02 X+50 Y+0 * ............................................... Mill circular arc around circle center I,J; negative direction
of rotation; end point coordinates X = +50 und Y = +0
N120 G27 R10 * ........................................................ Smooth (tangential) departure
N130 G00 G40 X+50 Y–40 * ...................................... Retract the tool in X, Y; cancel radius compensation
N140 Z+100 M02 * .................................................... Retract the tool in Z
N9999 %S520I G71 *
–5 50
50
Y
X
Z
I, J