HEIDENHAIN iTNC 530 (606 42x-02) ISO programming - Manual (Page 314)

314 Programming: Q-Parameters
9.1
1
Pr
ogr
amming Examples
9.11 Programming Examples
Example: Ellipse
Program sequence
„ The contour of the ellipse is approximated by
many short lines (defined in Q7). The more
calculation steps you define for the lines, the
smoother the curve becomes.
„ The machining direction can be altered by
changing the entries for the starting and end
angles in the plane:
Clockwise machining direction:
starting angle > end angle
Counterclockwise machining direction:
starting angle < end angle
„ The tool radius is not taken into account.
%ELLIPSE G71 *
N10 Q1 = +50 * Center in X axis
N20 Q2 = +50 * Center in the Y axis
N30 Q3 = +50 * Semiaxis in X
N40 Q4 = +30 * Semiaxis in Y
N50 Q5 = +0 * Starting angle in the plane
N60 Q6 = +360 * End angle in the plane
N70 Q7 = +40 * Number of calculation steps
N80 Q8 = +30 * Rotational position of the ellipse
N90 Q9 = +5 * Milling depth
N100 Q10 = +100 * Feed rate for plunging
N110 Q11 = +350 * Feed rate for milling
N120 Q12 = +2 * Set-up clearance for pre-positioning
N130 G30 G17 X+0 Y+0 Z-20 * 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
X
Y
50
50
30
50