HEIDENHAIN TNC 407 (280 580) ISO Programming - Manual (Page 158)

5 - 2 5 TNC 426/TNC 425/TNC 415 B/TNC 407
5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
100
–15
100 40
50
10
50
Y
X
Z
90
Example for exercise: Circular arc connecting to a straight line
Coordinates of the transition
point from the straight
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
Part program
%S525I 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 T12 L–25 R+20 * ........................................ Define the tool
N40 T12 G17 S1000 * ................................................ Call the tool
N50 G00 G40 G90 Z+100 M06 * ............................... Retract and insert tool
N60 X+30 Y–30 * ....................................................... Pre-position in the working plane
N70 Z–15 M03 * ......................................................... Move the tool to working depth
N80 G01 G41 X+50 Y+0 F100 * ................................ Approach the contour with radius compensation at
machining feed rate
N90 X+10 Y+40 * ....................................................... Straight line to which the arc tangentially connects
N100 G06 X+50 Y+50 * ............................................. Arc to end point X = 50 mm, Y = 50 mm; connects
tangentially to the straight line in block N90
N110 G01 X+100 * ..................................................... Complete the contour
N120 G00 G40 X+130 Y+70 * ................................... Depart the contour, cancel radius compensation
N130 Z+100 M02 * ..................................................... Retract in the infeed axis
N99999 %S525I G71 *