The SolidWorks sketch environment lets us easily create an ellipse with a simple tool. This ellipse has a number of reference points on it to help us to locate and dimension it. Figure 1 shows what we get from SolidWorks: four vertices, and a center point. In some optical designs and other applications, the focal points of the ellipse are needed. We can add some geometry and relations to automatically locate the foci of the ellipse.
Figure 1:
The procedure requires two construction lines sketched as follows:
1) Sketch the construction line AF from one of the vertices of the major axis to the center of the ellipse. This line represents half of the longer diameter.
2) Sketch the second line DE with one endpoint on the vertex of the minor axis and the other endpoint coincident to the line AF drawn in step 1.
3) Set these two construction lines equal by adding a geometric relation
4) The free endpoint E of the second line is a focus of the ellipse!
5) Optionally, add a second point G and a construction line DF. Add a symmetric relationship between points E and G about line DF.
Why is this true? Well, recall some high school analytic geometry: an ellipse is a collection of points for which the sum of the distances from two specific points (the foci) is a constant. In other words, if I travel from focus E, to any point on the ellipse, and then to focus G, the distance traveled is the same no matter what point on the ellipse I travel to. This distance is equal to the major diameter. The two equal construction lines each represent half of that constant distance.
