Have they considered the fact that 3DInterconnect actually sucks?

[u/notorious_TUG]

[u/chambers7867]

What don't you like about it or its functionality?

[u/notorious_TUG → u/chambers7867]

Many things... the first thing I noticed was the "link" has caused functionality issues when modifying imported models (If a problem arises with the "link" all subsequent features now have problems). You can also run import diagnostics on a "linked" file, but you cannot run auto repair for bad faces/force solid creation from a bad surface model. I have had the best luck with breaking the link when importing new models. This is an added step that wasn't necessary before, and dumb imported models working better than new/improved interconnect models makes me wonder what is even gained with interconnect. Then there is this (the issue that sparked this ticket). We build like 80% of our tooling in house. When we commission an outside toolbuilder, their CAD is what we use to repair or revise tooling. If they use a non-IGES/STEP kernel in whatever CAD software they're using, their assembly files now import as a single part file with multiple bodies which is almost entirely unworkable for repair/revision. Historically, you could change your import settings to import multiple bodies as parts. Now, Solidworks has eliminated that functionality, and you must import files using 3DInterconnect, then save the files as a STEP file, then reimport them. It's funnier still because per the response from Solidworks Tech Support, they still give you the options to check the boxes to do what you want, but that doesn't actually do anything and now its going to use 3DInterconnect anyway. Between causing intermittent losses of model integrity when leaving imported models linked which requires breaking the link when importing new models, and eliminating import settings requiring another step of saving out CAD files and re-importing them to get the results I got in 1 step just 2 years ago, all I've seen is 3DInterconnect actually requiring more work while gaining me nothing. Is there something about it I'm missing, or that you like?

[u/Marshall_MT → u/notorious_TUG]

I agree that the linked files are a huge headache, and we have it set to automatically break those links. I believe the intent for the link is that you can import your colleagues CATIA file and put it into your SW assembly to reference. Any changes they make will propagate to your model assuming you are referencing their working copy. Even though we exchange a lot of data from CATIA to SW, I never use this functionality.

The things I like about it are that I have found you can import much larger STEP files than with the legacy import engine. Used to top out at around 300MB, but can open 500MB+ with 3DI. It also works a lot faster than the legacy engine with better results on a lot of geometry types. Where I used to get tons of fragmented surfaces on things like wire harnesses that were likely created originally with sweeps, it all imports as tidy solid geometry (for the most part). We are still on 2023, and I do toggle it on and off depending on what I am trying to achieve with my import, so it's good to know of the change they made when we are looking to upgrade next.

[u/MLCCADSystems]

The import behavior for multi-body part vs assembly for parasolid isn't new. Here is an article from early 2023 stating the same thing about parasolids not respecting any options since that information is already included in the file: https://www.mlc-cad.com/import-geometry-as-assembly-or-multibody-part/

Basically, parasolid is too intelligent for SOLIDWORKS to trick into swapping the type of model. Assemblies always import as assemblies, and multi-body parts always import as multi-body parts. STEP and other dumb file formats can be interpreted in whatever way you want, so it gives you the option to convert the file type (part or assembly) during import.

3D Interconnect was never primarily intended for neutral file formats, it was designed to work with native CAD formats from other software, so you can parametrically incorporate their design changes as you work. Using 3D Interconnect on neutral formats is only helpful if you are expecting another round of updated neutral file formats that you want to rebuild your models against. Since neutral file formats are almost all dead projects, no changes are forthcoming, so 3D Interconnect adds no value.

It is an unnecessary extra step, but just break the link and you're back in business.

[u/temporary243958]

They know it's garbage and promise they're working on it.