Users are frequently contacting our support to ask why it is so slow to save SOLIDWORKS files to other file formats such as STEP format. They are also wondering why the exported files have large file sizes.
Large file sizes and long save times occur usually due large amount of geometrical details. Upgrading to more powerful workstation is usually not a solution to this issue. But instead, users should pay attention to those details and which details are relevant and which are not relevant for the recipient user who opens the exported model.
So how simplifying and reducing file size of the model actually happens?
At first, users can have a look if the SOLIDWORKS "Defeature" tool can be used as a solution. But unfortunately, quite often it is not possible to use it for simplifying. Then it is needed to simplify the model manually. This is done by following these steps:
Step 1: Removing irrelevant components from the assembly
When working with assemblies, you should start with deleting or suppressing the irrelevant components from the assembly. But first it is recommended to save the assembly as a new file copy to avoid making unintended changes to original assembly. Let's imagine that the designer only needs to export this perforated plate (image below) and the fasteners connected to holes are not the area of interest. Then it is better to just delete or suppress those fasteners.
TIP: If the fasteners are Toolbox components ("bolt" icon in assembly tree) it is really easy to select all those components by using the filter "Component Selection > Select Toolbox".
Step 2: Saving assembly as SLDPRT part
After you have removed the unnecessary components from the assembly, it can be saved as SLDPRT part to make the simplifying process smoother.
When saving assembly as part, it is best to use the option "All Components". This option will convert assembly components as solid bodies in resulting SLDPRT file. Removing or modifying solid bodies is usually much easier compared to surface bodies.
It is also worth of testing the option "Include Specified Components" which might actually remove the need of deleting components manually (step 1).
Step 3: Simplifying part
After you have saved the assembly as part, this part can be simplified. Simplifying is usually done by using extrude features to eliminate details. In the pictures below you can see the example of part simplifying and how the simple extrude can decrease the exported *.STEP file size significantly.
Plate has a huge amount of holes. When file is saved as *.STEP format, resulting *.STEP file's size is 5,5 MB.
Holes are removed by using simple Extruded Boss feature. When file is saved as *.STEP format, resulting *.STEP file's size is around 200 times smaller, only around 26 KB.
If the same file is saved as Parasolid format (*.x_t file format), resulting file will be twice as small.
Note: SOLIDWORKS is a Parasolid-based software and therefore the Parasolid file format is always the recommended format to be used between different SOLIDWORKS major versions for example. So when file has to opened with older SOLIDWORKS major version, you should export files as Parasolid file from new major version and then import those files with older major version. Downside of Parasolid format is that it is not supported for importing in all CAD software.
Another good example of reducing the file size is to reduce the amount of solid bodies by using Combine feature.
In the example picture below you can see the perforated plate that has a lot of bolts connected to holes. When the file is saved as *.STEP format, resulting *.STEP file's size is around 3,3 MB.
Previous 67 pcs of solid bodies have been merged to one single solid body by using Combine feature. Resulting *.STEP file's size is now dropped to 2,5 MB.
Summary:
Considering the previously mentioned examples it can be concluded that reducing the part's details and the amount of solid bodies has a huge impact on resulting file's size when the file is exported to *.STEP or some other non-SOLIDWORKS file format.
Please also read these articles about importing files to SOLIDWORKS:
Working with imported files in SOLIDWORKS
Working with imported files in SOLIDWORKS - Part 2
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