Large STEP files—typically 300 MB or more—need to be imported into SolidWorks for a project I’m working on, but I’m having trouble with stability and performance. I can successfully import the files, however the process is very slow and the program occasionally crashes. The files are created by another CAD program. Even simple tasks like rotating, zooming, and modifying the model become extremely slow after imported.
I’ve tried shrinking the STEP file to make it simpler, but doing so loses important elements for my task. I’ve also attempted modifying SolidWorks’ settings (such turning off pointless add-ons and tinkering with the performance settings), but I’m still not noticing appreciable performance gains. I suspect it’s a hardware constraint because I’m using a high-spec system with a fast processor, 64GB of RAM, and a top-tier GPU right now.
Has anyone else encountered such problems while importing big STEP files? Exist any particular methods or configurations in SolidWorks or outside programs that can help streamline the file import procedure without sacrificing the specifics?
Are there any suggested procedures or best practices for handling big SolidWorks files as well? Any advice or ideas on how to expedite the procedure and improve the cognos effectiveness of my job would be greatly appreciated.
Hello Yes, importing large STEP files is sometimes complicated or even impossible. The typical example are the bom files from Teckla for example, which are a disaster to exploit in Solidworks. As proof, Dassault has developed via its 3Dexperience DELMIA Plant Layout Designer in order to overcome this problem (as well as that of the import of point cloud and large implementation (or all at the same time). Afterwards, as explained in other posts, this is on paper, not tested yet for my part. Here is a link to another topic where I talk about it:
During the presentation demo I attended, they were carrying out a substantial import of the framework (in a few seconds vs solidworks where it can take more than a day for a result that is more than uncertain in terms of usability.
On the other hand of course this has a cost not included in the SW version (additional role in 3D experience) for a cost not evaluated for me
My method for importing large STEP files (or other formats):
Identify the software behind the format to be imported: Edit the file to be imported with notepad+... If the Step was created with Solidworks: ask if it is not possible to send us the assemblies in native format.
Always work on a local disk.
Close all open software and empty Windows and Solidworks Temporary Devices (with " Clean Up " from Windows and Solidworks RX).
Open Solidworks and use your own browser to open the STEP file (do not drag and drop the file from the Windows browser window).
When the import started, go get me a coffee... and wait.
Assuming that Solidworks manages to open the file, save it as *.sldprt / *.sldasm (still local)
If the file to be imported is an assembly: Lock the position of all the components (Constraints) then I try to identify the bolts or the name of the small dispensable components to remove them (via the search filter of the featuremanger). I use the " Select from Solidworks " feature to Select Hidden/Deleted Components to completely erase them.
I save again.
I close Solidworks, empty all temporary files again (see step n°3)
I open the file converted to *.sld...
I start step 7 again
If so, depending on the destination usage of the imported file, either I leave it as an assembly and use Pack&Go to send it to our Server, or I save it as *.sldprt (even if it is an assembly) to the server.
If the *.sldprt file reacts well to the conversion, I try to save it as *. Parasolid to automatically combine the maximum number of components (this also allows a large number of surfaces to be converted into Solids/Bodies).
On my side, all STEP import files of more than 180M go through another CAD software that opens them without problems. I export it in .xt. This poses much less problems when importing to SW If the file is really big, I make a drawing, which I save in .dwg or .dxf that I open on SW and I make do with the sketches.
I stopped bothering with long procedures and where SW crashes every other time.
Have you looked at the 3D Interconnect option? Either by activating it or by deactivating it
But 300MB is huge. It might be wiser to remodel it to have a simplified file (with only the data you actually need) It is an investment of time that quickly pays off.
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