HEIDENHAIN TNC 410 ISO Programming - Manual (Page 386)

360 10 Programming: Q Parameters
1
0
.1
0 Pr
og
ra
m
m
ing
Exam
ple
s
Example: Convex sphere machined with end mill
Program sequence
n This program requires an end mill.
n The contour of the sphere is approximated by
many short lines (in the Z/X plane, defined in
Q14). The smaller you define the angle
increment, the smoother the curve becomes.
n You can determine the number of contour cuts
through the angle increment in the plane
(defined in Q18).
n The tool moves upward in three-dimensional
cuts.
n The tool radius is compensated automatically.
%BALL G71 *
N10 D00 Q1 P01 +50 * Center in X axis
N20 D00 Q2 P01 +50 * Center in Y axis
N30 D00 Q4 P01 +90 * Starting angle in space (Z/X plane)
N40 D00 Q5 P01 +0 * End angle in space (Z/X plane)
N50 D00 Q14 P01 +5 * Angle increment in space
N60 D00 Q6 P01 +45 * Radius of the sphere
N70 D00 Q8 P01 +0 * Starting angle of rotational position in the X/Y plane
N80 D00 Q9 P01 +360 * End angle of rotational position in the X/Y plane
N90 D00 Q18 P01 +10 * Angle increment in the X/Y plane for roughing
N100 D00 Q10 P01 +5 * Allowance in sphere radius for roughing
N110 D00 Q11 P01 +2 * Setup clearance for pre-positioning in the tool axis
N120 D00 Q12 P01 +350 * Feed rate for milling
N130 G30 G17 X+0 Y+0 Z-50 * Define the workpiece blank
N140 G31 G90 X+100 Y+100 Z+0 *
N150 G99 T1 L+0 R+7.5 * Define the tool
N160 T1 G17 S4000 * Tool call
N170 G00 G40 G90 Z+250 * Retract the tool
N180 L10.0 * Call machining operation
N190 D00 Q10 P01 +0 * Reset allowance
X
Y
50 100
100
Z
Y
-50
R45
50
R45