Solidworks Import Limitations

[Anonymous]

I am really hoping to be able to import several of my current designs from Solidworks into Fusion, and use Fusion exclusively going forward.  But, so far, this appears to be both laborious, and of limited functionality.  I'm hoping there is something I'm missing.

When I import a Solidworks part file, I end up with a lovely-looking Fusion model.  Some features, however, are not editable, or only partially editable.  For example, for a simple part that is basically a 3/16" flat plate cut to a complex shape, with a number of thru holes, and a single pocket, I can edit the thru holes in simple ways, but I cannot modify the overall shape of the part, nor can I modify the pocket in any way.  When I edit the holes, if I use references to specify the location of the holes, those references seem to get thrown out, as soon as I click OK.  When I re-edit the holes, it shows NO references.

Am I missing something?

The file in question is attached.

Regards,

Ray L.

[Phil.E]

The SWx parts you are importing will not be parametric.

They are imported essentially as STEP files would be. They show up in a parametric Fusion design as Base Feature (non-parametric) components. If you edit the base feature you can see there are a few features that Fusion recognizes, such as holes. This is only Fusion "reading" the geometry and allowing an edit based on analysis.

But you won't see your SWx sketches or parameters in your Fusion model.

If you need to make changes, there are non-parametric editing tools to help, such as Press Pull and Move (use face option). When you are done editing it, click "finish base feature" to return to regular parametric editing.

Any feature added to the model after importing, and not inside the Base Feature, will be parametric going forward.

Thanks,

[Anonymous]

So it is not possible to modify the base geometry itself.  Rather, you can only cut/extrude/etc to modify it?  Is there a way to (even manually) extract sketch data from the base geometry so the part can be re-created as a fully parametric model?

What I'm trying to do is import all the parts for a fairly complex assembly created in Solidworks, so I can use Fusion going forward.  I don't mind spending a few days on the conversion, if it gets me a fully-functional Fusion model.  But, so far, it seems like I keep running into brick walls, that keep me from getting there, even for simple parts.  To date, my best approach appears to be to use Solidworks to extract DXFs, import those into Fusion (or, more correctly, Insert those into Fusion since Import seems to cripple the created sketches...), then re-build the geometry manually by using Press/Pull on the sketches, shifting the sketch planes, re-constraining sketch elements to lower-level features, etc.  Solidworks Import seems fine if all I want to do is import a part, and use it, as-is, in a new model.  But once I have to modify that part, things seem to get ugly real fast.  I don't want to end up with a model that 6 months from now will prevent me from making some change, because of how it was brought into the system.

Regards,

Ray L.

[Phil.E]

Yes you can modify the base part, inside the Base Feature you can manually move things around. This is non parametric editing. Anything you do here is not driven by parameters, but any downstream features that refer to it will be driven by the changes to the Base Feature.

Using DXF sketches: sounds like you have worked out the correct workflow for making your parts into parametric Fusion models.

Thanks,

[michallach81]

Hi Phil, if you would look at Ray model you would see, that Find Feature don't work as it should. For example we can edit hole feature, but only in theory:

Michał

[Phil.E]

@michallach81

Thanks for pointing that out. This particular model has a problem with recognized holes. I've logged a new bug report about it. Other SWx models I tested do not show this problem, so it may be specific to this model only.

@Anonymous

Thanks for the report and the sample file. Would you by chance have the original SWx file for us to compare with?

Please let us know if you have any further questions.

Regards,

[Anonymous]

Solidworks file attached.

Regards,

Ray L.

[Phil.E]

Can you try again with this file? I just imported it and can edit all the holes. We'll be looking into the part that shows hole failures, but for now I can work with this SWx file as expected. Try importing it again.

Thanks,

[Anonymous]

Phil,

I think you forgot the file....

Regards,
Ray L.

[loggingeq]

What file types can be imported into Fusion 360 that will retain the design tree & will allow parametric changes to be made, ie. an editable model?

[michallach81]

After small investigation, simple import and Find Feature gives nice results, everything works... but If I would create new file, then create component (everything is still empty), and then insert imported file, break link... and then use Find Feature we get an error. I think all that is caused by Break Link. Take a look:

[michallach81]

Fusion can read only its own "feature tree", and its same with all other cad programs available on market.

[Phil.E]

@loggingeq

Yes, as @michallach81 says, only .f3d files made in Fusion will retain their parametric history.

@Anonymous

By "this" file, I mean the SWx file attached to this post. I uploaded it and had no errors. So if you could try again it would be nice to know if what ever steps you take are somehow breaking the translated model. I found no problems editing the holes when I did this, unlike inside the original .f3d you attached.

Thanks,

[Phil.E]

@michallach81

Thanks for finding the steps that lead to this odd failure. I'll add these notes to the bug report.

@Anonymous

Before insert and break link, upload the SWx file and use Find Features. Or just don't insert it if you don't need to.

[michallach81]

Phil did you see my screencast?

[michallach81]

ok, you did.

[Anonymous]

Phil,

There is no file attached to either of your posts...

Regards,
Ray L.

[Phil.E]

The file in question is the one you posted. I'm trying to tell you to take this file and try again to upload and work with it. As @michallach81 has shown us, avoid breaking link.

Here is an image of your post with the file you are trying to work with attached.

[Anonymous]

Nothing has changed. I import the Solidworks model, open the new model, select the one Body, and FindFeatures. I can edit ONLY the two large thru holes, and the middle hole of the three in the pocket. I CANNOT in any way modify the large pocket, or the other small holes. As soon as I EditFeature on the pocket, the pocket disappears, and the OK button on the EditFeature dialog is disabled. When I select EditFeature on the small holes, NOTHING happens - no EditFeature dialog. And, until I hit ESC a few times, I can't do much of anything at all.

Regards,
Ray L.

[Phil.E]

@Anonymous

Since both myself and @michallach81 are having no trouble, let's review the steps that work. I think you are not dissolving the patterns.

This works for me:

1. Upload the file

2. Open the file

3. Find features

4. Dissolve the patterns (right click on the browser node and pick Dissolve)

5. Edit the holes.

Likewise, do not find all features. Uncheck the patterns box on the filter. The holes all appear independent of the pattern.

Let us know if that works.

Thanks,