Home » How to save an assembly as a part in SolidWorks?

Need to simplify a large assembly or send an assembly to a third party? Consider saving the assembly as a part. Protect intellectual property by removing internal geometry and send the file to a third party. Alternatively, simplify an assembly to external faces to reduce computer resources. This tutorial will explore the “Save As” and “Defeature” options.

To follow along with the example, download the gear pump assembly from grabcad.com here.

Original assembly, “Part 5 Body” set as wireframe.

Save As


When saving an assembly file, part can be selected from list of file formats. This will alter the available save as options.

All components – This includes all components of the assembly.

Exterior Faces – This remove all internal components, refer to the example.

Include specified components – Hide or suppress components that are not to be included.

Tip: If this feature is used on a regular basis, create an export configuration and suppress unwanted geometry.

Save as part, external surfaces only. Section view on “Part 5 Body” to show internals are removed.


The defeature tool in SolidWorks can be used to simplify parts and assemblies. Large assemblies can be simplified to improve performance, and features can be kept or removed from parts in preparation for FEA analysis.

For better performance, consider using the defeature tools at the sub-assembly levels. Trying to defeature a top level assembly can take a while.

The following example will use “Tools” – “Defeature” to remove all internal geometry from the assembly and save it as a part file. There are five steps to this process, a preview of the part will appear after step 3.

Step 1 – Component Selection

For removal, there are three options:

  • Internal Components – Removes any internal geometry.
  • Small components – Use this to specify the parts/features to remove as a percentage of the assembly size. This is useful with large assemblies as components/features do not need to be selected.
  • Selected components – Components can be manually selected from the design tree or by selection of the parts on screen.

Set display to “Hide removed components” and press the update button, removed components will show as hidden in the design tree.

Use the exceptions selection to keep specific components. These components will not be removed even if they meet the criteria of the “Remove” section.

For this example select “Internal components” only.

Step 2 – Motion

This option can be used to allow motion, if required. This will result in an assembly file as the output and will not be used.

Step 3 – Features to keep

As a result of selecting “Internal components” in step 1, holes and extruded cuts will be removed. The hole selection can be set as a range of diameter or manual. In the example below, the threaded holes and 1/2″ port hole were selected manually.

Step 4 – Faces to Remove

Depending on the auto-select options in step 3, unwanted features might be included. This step will show with a preview, and allows for the selection of items to remove. Where possible, adjust the settings in step 3 to avoid this step. For this example, only the desired features were retained, step 4 was left blank.

Note: Using defeature on a part file will only show steps 3 and 4. Select the features to keep and remove, then save the file as a new part.

Step 5 – Save

The file can be saved as a new document, with or without a link to the original. Creating the link will update the part file with changes to the assembly, this may require adjustment to steps 1 through 4.

Publish will make the part available to someone else, who has access to 3D ContentCentral. If sending to a third party, save the result as a .sldprt file and then convert it to a translation file format.

Additionally the settings applied can be stored for future use.

The final result is shown below, faces have been set to transparent to show that the internals have been removed.