HEIDENHAIN iTNC 530 (340 49x-03) - Manual (Page 618)

618 11 Programming: Q Parameters
1
1
.12 Pr
ogr
a
mming Examples
11.12 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.
0 BEGIN PGM ELLIPSE MM
1 FN 0: Q1 = +50 Center in X axis
2 FN 0: Q2 =+50 Center in Y axis
3 FN 0: Q3 = +50 Semiaxis in X
4 FN 0: Q4 = +30 Semiaxis in Y
5 FN 0: Q5 = +0 Starting angle in the plane
6 FN 0: Q6 = +360 End angle in the plane
7 FN 0: Q7 = +40 Number of calculation steps
8 FN 0: Q8 = +0 Rotational position of the ellipse
9 FN 0: Q9 = +5 Milling depth
10 FN 0: Q10 = +100 Feed rate for plunging
11 FN 0: Q11 = +350 Feed rate for milling
12 FN 0: Q12 = +2 Set-up clearance for pre-positioning
13 BLK FORM 0.1 Z X+0 Y+0 Z-20 Define the workpiece blank
14 BLK FORM 0.2 X+100 Y+100 Z+0
15 TOOL DEF 1 L+0 R+2.5 Define the tool
16 TOOL CALL 1 Z S4000 Tool call
17 L Z+250 R0 FMAX Retract the tool
X
Y
50
50
30
50