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How is Surfacing in Onshape vs. SolidWorks in 2026?
Chris_Beckett
Member Posts: 8 ✭
in General
I have done a fair bit of surface modeling in SolidWorks over the years.
Now considering Onshape and I'm wondering:
- How is the quality of Onshape’s surfacing tools compared to SolidWorks?
- Does Onshape have all the same surfacing functionality as SolidWorks?
- If not, what's missing?
- If so, is it just as easy to use in Onshape? (ie not any more difficult).
- How is the quality of the surfaces that Onshape creates compared to SolidWorks?
The only answers I found in Google were from years ago. Onshape may have changed quite a bit since then (it seems).
What has been your experience, experienced surface modelers?
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Personally, I much prefer Onshape to Solidworks these days. There's a bit more control of most things, although a true 3D sketcher is missing. You can do just about everything you'd need with the other curve tools (routing curve, bridging curve, edit curve, etc), but there's no 3D solver. The 3D solver in Solidworks was always pretty brittle/buggy and stuff would blow up in weird ways.
Surface quality is as good or better. The surface analysis tools are more capable. Both are Parasolid based, as you probably know. In theory anything that can be represented in NX, Solidworks, Shaper3D, Plasticity, etc can be modeled in Onshape since it's all the same kernel.
There are a lot of a little quality of life things that could be improved here and there, but overall I'd rather work in Onshape.
The CAD for these below was all done in Onshape:
Simon Gatrall | Product Development Specialist | Open For Work
Thank you @S1mon. Your insights and photos are a big help. That headsets photo is stunning.
@S1mon is top tier at this stuff!
The Onsherpa | Reach peak Onshape productivity
www.theonsherpa.com
Hey @Nick_Holzem, you should post some of your work here!
One thing that really changed the game for me in Onshape was the ability to Edit Curves. While you can't do directly create 3D sketches, I'm mostly using projecting 2 sketches to create the 3D curve. From there you can use Edit Curve to reduce the point count (even down to single-span) and create much cleaner surfaces. SolidWorks doesn't really have that functionality and creating 3D sketches to replicate those projected curves is very tedious and difficult.
Ramon Yip | glassboard.com
Oh I guess I should have dropped my surfacing video here too.
The Onsherpa | Reach peak Onshape productivity
www.theonsherpa.com
Thanks Evan. I will try to watch this.
Have you done surfacing in SolidWorks also?
How would you compare the two?
I have but it was 9+ years ago. Onshape can handle anything I'd have done in Solidworks. The real tell will be you doing a model in Onshape and asking here for specific troubleshooting help to see for yourself.
The Onsherpa | Reach peak Onshape productivity
www.theonsherpa.com
I would also check @GregBrown's channel as there are some good "deep dives" into Onshape's surfacing/curve tools:
Here's an example (from a year ago, so there have been things added since) that might be useful:
There are also some good videos on the face blend feature and a very recent one on Conic surfaces that is more of a "preview" of upcoming features but also features a lot of general Onshape specific surfacing functionality.
Thank you. That's what I'm doing right now. Currently frustrated by how many more clicks everything seems to take in Onshape vs. Solidworks.
I'm currently having to rebuild in SolidWorks some models that we built in Onshape and it's been ruffffff…
Onshape has so many quality of life features that I've now started to take for granted. And this is after 10 years of SolidWorks and 2 years into Onshape.
The one thing that I DO dislike is that in Loft, Sweep, and Boundary Surface, you need to expand the selection boxes to keep each selection grouped. Otherwise, I enjoy not needing to convert entities to create a new sketch if I want to keep my feature tree from absorbing my layout sketches. Currently, I'm constantly having to fight that in SolidWorks.
Ramon Yip | glassboard.com
Can you share some of the quality of life things you mention? How is Onshape better at surfacing?
I've been trying to model a part I did in SolidWorks years ago. So far it seems to me like the SolidWorks workflow is more streamlined.
But I only started Onshape a few days ago, so I'm asking more experienced users.
As far as I know, Solidworks still can't tell you how complex a surface is (e.g. degrees, spans and knots). I used to export to Rhino just to see what the isoparameters were to see how crazy a surface had become. This is built into the curvature evaluation tools in Onshape. The boundary surface tool in Onshape is better about taking existing input curves and keeping the surface as simple as possible. Loft in Solidworks (and Onshape) just wants to make really heavy multispan degree 3 surfaces which can cause a lot of downstream grief with complex models.
Bridging curve with G3 on both ends is very powerful 3D tool. Solidworks still only does a "torsion" constraint (G3) in the 2D sketcher.
Custom features add an incredible amount of power to Onshape. If you need custom airfoil shapes (or gears, etc.), for instance, there are features for that.
The Edit Curve feature (with approximate, raise degree, and planar) starts to approach some of what you can do in Alias, Rhino etc. It's not going to fully replace those, but it does a lot to get good quality curves in a mechanical CAD tool. There's nothing like it in Solidworks.
Simon Gatrall | Product Development Specialist | Open For Work
If we ignore surfacing for a moment, I would say the way that history, version control, and reference management work is really the fundamental reason I do not want to work in other tools. I've spent 30+ years using Pro/E and Solidworks for complex consumer, medical and industrial products with a lot of top down design. Managing those references in other tools was doable, but there were a lot of pain points that go away in Onshape. I also basically never loose work in Onshape. I cannot say that for any file-based CAD system I've used, even with professional PDM tools in place. I managed Solidworks EPDM (now PDM pro) for 8 years. Again, I would not go back to that. Yes there are a few things here and there that are missing in Onshape, but overall the ease of use and ability to freely experiment safely is life changing.
Simon Gatrall | Product Development Specialist | Open For Work