HEIDENHAIN TNC 360 ISO Programming - Manual (Page 97)

5-14 TNC 360
5 Programming Tool Movements
5.4 Path Contours - Cartesian Coordinates
Example for exercise: Chamfering a corner
Coordinates of the
corner point E : X = 95 mm
Y = 5 mm
Chamfer length: LF = 10 mm
Milling depth: Z = –15 mm
Tool radius: R = +10 mm
85
X
Y
Z
95
100
E
15
5
100
–15
Part program
%S514I G71 * ............................................................ Begin program
N10 G30 G17 X+0 Y+0 Z–20 * .................................. Workpiece blank MIN point
N20 G31 G90 X+100 Y+100 Z+0 * ............................ Workpiece blank MAX point
N30 G99 T5 L+5 R+10 * ............................................ Tool definition
N40 T5 G17 S2000 * .................................................. Tool call
N50 G00 G40 G90 Z+100 M06 * ............................... Retract spindle and insert tool
N60 X–10 Y–5 * ......................................................... Pre-position in X, Y
N70 Z–15 M03 * ........................................................ Pre-position to the working depth, spindle on
N80 G01 G42 X+5 Y+5 F200 * .................................. Move with radius compensation and reduced feed to
................................................................................... the first contour point
N90 X+95 * ................................................................ Program the first straight line for corner E
N100 G24 R10 * ........................................................ Chamfer block: inserts a chamfer with L = 10 mm
N110 Y+100 * ............................................................ Program the second straight line for corner E
N120 G00 G40 X+110 Y+110 * ................................. Retract the tool in X, Y and Z, cancel radius
................................................................................... compensation
N130 Z+100 M02 * .................................................... Move tool to setup clearance
N9999 %S514I G71 *