HEIDENHAIN iTNC 530 (606 42x-02) ISO programming - Manual (Page 316)

316 Programming: Q-Parameters
9.1
1
Pr
ogr
amming Examples
Example: Concave cylinder machined with spherical cutter
Program sequence
„ This program functions only with a spherical
cutter. The tool length refers to the sphere
center.
„ The contour of the cylinder is approximated by
many short line segments (defined in Q13). The
more line segments you define, the smoother
the curve becomes.
„ The cylinder is milled in longitudinal cuts (here:
parallel to the Y axis).
„ The machining direction can be altered by
changing the entries for the starting and end
angles in space:
Clockwise machining direction:
starting angle > end angle
Counterclockwise machining direction:
starting angle < end angle
„ The tool radius is compensated automatically.
%CYLIN G71 *
N10 Q1 = +50 * Center in X axis
N20 Q2 = +0 * Center in the Y axis
N30 Q3 = +0 * Center in Z axis
N40 Q4 = +90 * Starting angle in space (Z/X plane)
N50 Q5 = +270 * End angle in space (Z/X plane)
N60 Q6 = +40 * Cylinder radius
N70 Q7 = +100 * Length of the cylinder
N80 Q8 = +0 * Rotational position in the X/Y plane
N90 Q10 = +5 * Allowance for cylinder radius
N100 Q11 = +250 * Feed rate for plunging
N110 Q12 = +400 * Feed rate for milling
N120 Q13 = +90 * Number of cuts
N130 G30 G17 X+0 Y+0 Z-50 * Definition of workpiece blank
N140 G31 G90 X+100 Y+100 Z+0 *
N160 T1 G17 S4000 * Tool call
N170 G00 G40 G90 Z+250 * Retract the tool
N180 L10.0 * Call machining operation
N190 Q10 = +0 * Reset allowance
N200 L10.0 Call machining operation
X
Y
50 100
100
Z
Y
X
Z
-50
R40