Splines compared to SolidWorks

Phillip_B

I noticed some differences in the way splines are handled between Onshape and SolidWorks:

SolidWorks:


Onshape:


I am unable to define splines in the same way as SolidWorks. Once curvatures are used, Onshape can no longer resolve the sketch.

Is there a way to generate stil-splines?


Can't Onshape handle curvatures in splines? How can I edit spline definitions at middle spline points?

S1mon

Splines in Onshape are nowhere near what 2D and 3D splines are in Solidworks (or just about any other serious CAD system). You can work around some of the limitations with adding points to 2D splines, but you need to be careful not to end up with something lumpy. Onshape's 2D sketcher is limited to degree-3 b-splines (or with no internal spline point, you get a single degree 3 Bézier). Degree 3 b-splines maintain C2 continuity internally by definition, but allowing C2 at the ends is dependent on the number of internal points and their arrangement. Approaching G3 is really a matter of very carefully tweaking the points around. 

In the sketch you have, if you add some internal spline points to your splines, you might be able to get closer to your intent. Here's a version of your sketch where I added 2 internal points per spline, and some construction lines to space the points out roughly evenly (see sketch1).



If you're willing to take some extra steps, you can use the bridging curve feature to get curvature at the ends. You'll then need to use that edge in a secondary sketch, or make a composite curve or something for you next steps. (see sketch 2, and bridging curve 1+2).

Phillip_B

Thanks Simon for the detailed explanation. I'm not a mathematician, but I'm an excessive user of C2 splines. My company operates in the consumer goods industry. C2 splines are essential here. Are there any plans to expand the onahape sketcher here in the future? in my understanding, onshape wants to be a professional CAD system.

S1mon

@Phillip_B

I really don't know what Onshape plans to do. I've been following them for about 5 years, and only seriously started using it recently. I've had countless conversations with their sales and technical people where I've emphasized how important decent splines are to doing the kind of work that I (and countless others) do. A real 3D sketcher is also essential. I get the impression that they do care, and that these things are coming some day, but there are lot of directions that they are expanding at the same time. There is an add-on called Phi3D which they pushed a bit, but so far it doesn't seem to be a good fit for class-a surfacing. It might be interesting for form-finding, but at that point I'd rather just use a completely different tool like Rhino.

For me I can get Onshape to do some decent surfacing because I know how it's done in other tools (Solidworks, Creo, Alias, Rhino, etc). I can work around the limitations. It's a little like using canned vegetables for a gourmet meal. It's not an ideal solution, but if you know what you're doing, maybe it can be made to work.