HEIDENHAIN TNC 426B (280 472) ISO programming - Manual (Page 126)

110 6 Programming: Programming Contours
6.4 P
ath Cont
ours — Car
tesian Coor
dinat
es Example: Circular movements with Cartesian coordinates
%CIRCULAR G71 *
N10 G30 G17 X+0 Y+0 Z-20 *
N20 G31 G90 X+100 Y+100 Z+0 *
N30 G99 T1 L+0 R+10 *
N40 T1 G17 S4000 *
N50 G00 G40 G90 Z+250 *
N60 X-10 Y-10 *
N70 G01 Z-5 F1000 M3 *
N80 G01 G41 X+5 Y+5 F300 *
N90 G26 R5 F150 *
N100 Y+85 *
N110 G25 R10 *
N120 X+30 *
N130 G02 X+70 Y+95 R+30 *
N140 G01 X+95 *
N150 Y+40 *
N160 G06 X+40 Y+5 *
N170 G01 X+5 *
N180 G27 R5 F500 *
N190 G40 X-20 Y-20 F1000 *
N200 G00 Z+250 M2 *
N999999 %CIRCULAR G71 *
Define blank form for graphic workpiece simulation
Define tool in the program
Call tool in the spindle axis and with the spindle speed S
Retract tool in the spindle axis at rapid traverse
Pre-position the tool
Move to working depth at feed rate F = 1000 mm/min
Approach the contour at point 1, activate radius compensation G41
Tangential approach
Point 2: first straight line for corner 2
Insert radius with R = 10 mm
Move to point 3: starting point of the arc with G02
Move to point 4: end point of the arc with G02, radius 30 mm
Move to point 5
Move to point 6
Move to point 7: End point of the arc, radius with tangential
connection to point 6, TNC automatically calculates the radius
Move to last contour point 1
Tangential departure
Retract tool in the working plane, cancel radius compensation
Retract tool in the spindle axis, end of program
X
Y
95 5
95
5
85
40
40 30 70
R10
R30
Gkap6.pm6 29.06.2006, 08:06 110