HEIDENHAIN TNC 407 (280 580) ISO Programming - Manual (Page 145)

TNC 426/TNC 425/TNC 415 B/TNC 407 5 - 1 2
5 Programming Tool Movements
5.4 Path Contours – Cartesian Coordinates
Example for exercise: Milling a rectangle
Coordinates of the corner points:
1 X = 5 mm Y = 5 mm
2
X = 5 mm Y = 95 mm
3 X = 95 mm Y = 95 mm
4 X = 95 mm Y = 5 mm
Milling depth: Z = –10 mm 100
95
5
–10
5
100
95
3
1
2
4
Y
X
Z
Part program
%S512I G71 * ............................................................ Begin the program. Program name S512I,
................................................................................... dimensions in millimeters
N10 G30 G17 X+0 Y+0 Z–20 *
N20 G31 G90 X+100 Y+100 Z+0 * ............................ Define blank form for graphic workpiece simulation
(MIN and MAX point)
N30 G99 T1 L+0 R+5 * .............................................. Define tool in the program
N40 T1 G17 S2500 * .................................................. Call tool in the infeed axis Z (G17);
Spindle speed S = 2500 rpm
N50 G00 G40 G90 Z+100 M06 * ............................... Retract in the infeed axis; rapid traverse; miscellaneous
function for tool change
N60 X–10 Y–10 * ....................................................... Pre-position near the first contour point
N70 Z–10 M03 * ........................................................ Pre-position in the infeed axis, spindle ON
N80 G01 G41 X+5 Y+5 F150 * .................................. Move to
1 with radius compensation
N90 Y+95 * ................................................................ Move to corner point 2
N100 X+95 * .............................................................. Move to corner point 3
N110 Y+5 * ................................................................ Move to corner point 4
N120 X+5 * ................................................................ Move to corner point 1 , end of machining
N130 G00 G40 X–10 Y–10 M05 * .............................. Depart the contour, cancel radius compensation, spindle STOP
N140 Z+100 M02 * .................................................... Retract in the infeed axis, spindle OFF, coolant OFF,
................................................................................... program stop, return to block 1
N99999 %S512I G71 * .............................................. End of program