CAD FAMILY/CONFIGURATIONS

toomdog · July 22, 2026, 4:59pm

Hi folks,

I have discovered a new (?) feature in SW25 (was it released in 24?) called CAD FAMILY which seems to be related in some fashion to 3D Experience…
I have created a virtual part within an assembly and would like to show it on the BOM. Previously, I would go to configuration properties of the virtual part and select user specified name, then type what should show in the parent assembly’s BOM.

What do I need to do to add custom properties to this item and control how it shows in the BOM? Do I just delete this one and build it again? It’s not terribly complicated… If it could shed any more light on the situation, this item shows dimensions in meters when sketching but inches when editing dimensions.

Here is the properties window I am familiar with:

And here is what I get instead:

JimSculley · July 22, 2026, 6:25pm

Assuming you aren’t using SW Makers, or 3D Experience:

Turn off (via Tools…Add Ins) or uninstall the 3D Experience add-in
Go to the ConfigurationManager tab in the feature manager tree.
Right-click on the top-level CAD Family (or the master Physical Product) and select Remove CAD Family.
Save the file

If you can’t disable/remove the add-in:

Close any open files in SolidWorks (the option will be grayed out if a part is open).
Go to Tools > Options > System Options > 3DEXPERIENCE Integration.
Uncheck the option for Allow Multiple Physical Products in New Parts and Assemblies.

toomdog · July 22, 2026, 7:08pm

Jim:
Sorry, I forget there are so many products these days. Yes, I’m running SolidWorks Professional 2025 SP5.0 on my local machine and we do not use 3D Experience.

3D Experience add-in was already disabled and set to not run at startup.
I have removed the CAD Family, but nothing else changes after save and/or rebuild.
Furthermore, I have no 3DEXPERIENCE Integration options in System Options; even searching in options, ‘3de’ returns no results and ‘3d expe’ returns no results.
I do see a 3DEXPERIENCE Integration heading in Document properties. The only option is ‘Use the Physical Product title for single physical products with no CAD family’ and it is unchecked in the original virtual part I posted this question about.

I have created a new virtual part in the same assembly and get the same behaviour. Same for a new virtual part or virtual assembly in a new assembly or even an older unrelated assembly.

I don’t understand what has changed. I have created virtual assemblies since our last update and had no issues. Is SolidWorks turning on options without telling us?

JimSculley · July 22, 2026, 7:38pm

I have the same version and SP and don’t see this behavior. I do not have the 3DE add-in installed. Have you tried saving the part as a real file and seeing if you can get rid of the CAD family stuff from there? If so, you can then make it virtual again and be on your way.

As to why the virtual part did this, perhaps it has to do with your templates. If you have virtual parts automatically using a different template than non-virtual, that may explain some of this.

toomdog · July 22, 2026, 8:41pm

Very interesting, I hadn’t considered virtual part templates. But we have had other people in the office create new virtual parts and no one else has had this issue… Maybe my settings are unique… I am not an admin; I’ll have to ask about that.

In any case, this notice pops up when I remove the CAD Family. From here, I can right click on the ‘Default’ item in the tree and choose 'Save Physical Products…" and that allows me to save it externally and it attains a typical configuration tree where I can set the properties I need.

I think my solution for the time being is to have a blank external part I can drop into assemblies and make virtual when I need a virtual part.

mp3-250 · July 22, 2026, 10:56pm

IIRC there are multiple open BR about this kind of behavior when using the default “empty” template in SW even without 3d experience.

JimSculley · July 23, 2026, 1:02pm

There was one report (BR10000382804) that opening an assembly in lightweight mode would cause this, but it was supposedly fixed in SW2024 SP5.

Another report (BR10000396878) of CAD Family appearing out of nowhere was listed as fixed in SW2025 SP3, but didn’t list a cause or method to reproduce.

And then there is another report (BR10000414533) of it happening and was supposedly fixed in SW2026 SP0.

And then we have a report (BR10000413423) which is marked as closed and says emphatically in all caps:

THIS PROBLEM WILL BE FIXED ON SOLIDWORKS 2026 SP1.

And its companion report (BR10000412884) with the same haughty claim that it will be fixed in 2026 SP1, but it also has a step by step way to reproduce, which does involve part templates:

1) Start SOLIDWORKS
2) Tools > Options > Default Template > be sure a default template is set for the Part > OK
3) Go to Windows Explorer > location of the default Part template > rename the Part template in order for SOLIDWORKS not to find it
4) Create a new Part > OK
5) SOLIDWORKS prompts: ”Default template not available” message > chose ‘Use a blank template’ option
6) Go to ConfigurationManager > Configurations change to Cad Family

I tried this in SW2025 SP5 and it does in fact switch to CAD Family:

But this only happened when creating a new virtual part. The Default template not available message has to appear in order for the bad behavior to happen.

So, @toomdog, you should probably check that the default templates listed here:

point to actual files that exist, or switch the setting to Prompt user to select document template which will then use the folders listed in System Options...File Locations...Document Templates

Lastly (and I find this really funny), the opposite problem shows up (BR10000426749) where parts that should be CAD Family are incorrectly showing Configurations. Supposedly fixed in SW2026 SP3. However, the end of the report has conflicting information:

So it was not reproducible, but there’s a fix coming?

mp3-250 · July 23, 2026, 2:48pm

before upgrading our company to sw2025 I did some test and I stomped in the template issue. That was the reason I unified all our users installation switching non pdm users to an offline pdm mode, forcing them to use our standard template instead of the empty one SW would generate automatically.

Anyway 2024-25-26 are funny releases, so many oddballs like the BR you found. Sometimes I find myself looking at the KB with disbelief. so many regressions from one SP to another, it seems like the main release cycle lost its core meaning.

toomdog · July 23, 2026, 3:10pm

You can’t make this stuff up, and I am regretful that it is the case.

In other news, the random error I had been encountering intermittently for the last number of months when creating a new part or assembly makes a lot more sense now. It was some kind of error about a document template from a particular vault (special project specific, not used very often any more) that could not be found in my app data/roaming folder.

I checked the default templates in settings and sure enough, both parts and assemblies were missing references. I pointed them where they belong and my latest virtual part has a default configuration!

I see it now and I say “duh” but I don’t think I would have ever connected those dots… Thank you for pointing me in the right direction!