I created nested elliptical cylinders in two different ways recently, and neither of them work. 1. Thin Feature Extrude. 2. Extrude the cylinders after sketching them together in 2D. Interestingly SW assumes that the user wants a hollow cylindrical cylinder While a third method works, which is sketching and extruding the larger cylinder, then positioning the sketch of the smaller one on it and doing an extruded cut. What I mean by 'work' is there are no geometrical peculiarities and when I import the CAD file into COMSOL, it behaves--it meshes ok. But when I import the nested cylinders into COMSOL using the first two methods, I get a gap and the geometry won't mesh.
If you run Tools/Interference Detection on the cylinders, the gap shows up in red on the right. My question is why the gap? And is there a fix for it? Is this an example of what Jerry Steiger told me in "Mate a rod curving in 3D to a curved surface," that SW can get confused about which bits are in or out of two bordering parts so experienced users often create an over-sized part and cut it back with a surface?
Thank you.
Kris,
I wouldn't expect to see issues with relatively simple extrudes like you are using here. Digging a bit into your assembly, I think the problem is that the Right Plane for the outer ellipse is offset .0005 mm from the Right Plane of your inner ellipse and the gray matter. I suspect this has to do with the way you mated your parts. Life usually works much better if you can mate the three main planes of your parts directly with the three main planes of your assembly. It seems like you could have easily done it that way, but for some reason chose not to.
It's also not a good idea to leave your sketches under defined. It makes it very easy for your parts to change inadvertently.
I would make a master sketch, either in the assembly or in a master part. Convert edges off of that master sketch to make your three parts, or three bodies in the master part. If using a master part, split the bodies into your three parts. You could also use Sketch Contours and just one sketch if you use the master part, which saves the added sketches and convert edges, but is not as robust.
I didn't take the time to prove that better mating and sketching would allow all three methods to work, but I'm pretty confident that you will find that it will.
Jerry Steiger