HEIDENHAIN TNC 407 (280 580) ISO Programming - Manual (Page 153)

TNC 426/TNC 425/TNC 415 B/TNC 407 5 - 2 0
5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
Example for exercise: Mill a full circle with one block
Circle center: I = 50 mm
J = 50 mm
Beginning and end
of the arc:
X = 50 mm
Y = 0 mm
Milling depth: Z = –5 mm
Tool radius: R = 15 mm
Part program
%S520I G71 * ............................................................ Begin the 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 * ............................................ Define the tool
N40 T6 G17 S1500 * .................................................. Call the tool
N50 G00 G40 G90 Z+100 M06 * ............................... Retract and insert tool
N60 X+50 Y–40 * ....................................................... Pre-position in the working plane
N70 Z-5 M03 * ............................................................ Move tool to working depth
N80 I+50 J+50 * ......................................................... Coordinates of the circle center
N90 G01 G41 X+50 Y+0 F100 * ................................ Approach first contour point with radius compensation at
machining feed rate
N100 G26 R10 * ......................................................... Soft (tangential) approach
N110 G02 X+50 Y+0 * ............................................... Mill arc around circle center I,J; direction of rotation negative
(clockwise); coordinates of end point X = +50 mm, Y = +0
N120 G27 R10 * ......................................................... Soft (tangential) departure
N130 G00 G40 X+50 Y–40 * ...................................... Depart the contour, cancel radius compensation
N140 Z+100 M02 * ..................................................... Retract in the infeed axis
N99999 %S520I G71 *
–5 50
50
Y
X
Z
I, J