How to Save a SOLIDWORKS Assembly as a Part

You can save a SOLIDWORKS assembly as a part when you need a lighter reference model, a simplified file for a customer or supplier, or a single part document for use in another assembly. Open the assembly, choose File > Save As, select Part (*.sldprt), choose the components or geometry to include, and save the result under a new name.

This operation does not turn the assembly into one editable feature tree. The saved part normally contains imported-style solid or surface bodies rather than the original mates, component features, assembly motion, BOM structure, or component-level design history. Keep the source assembly as the master model.

When saving an assembly as a part makes sense

• Insert a purchased machine or equipment package into a larger layout without loading every component.
• Provide envelope geometry for space claims, packaging, or clearance studies.
• Share an external shape while removing internal components and unnecessary detail.
• Create a simplified reference for downstream CAD software.
• Reduce the component count in a large top-level assembly.

Do not use this as a substitute for a Pack and Go archive when the recipient needs the real editable assembly. Do not use it for manufacturing when component identities, tolerances, materials, BOM information, or motion relationships are required.

Save the assembly directly as a part

1. Open the assembly and rebuild it.
2. Activate the configuration and display state you want to export.
3. Suppress, hide, or exclude anything that should not be considered.
4. Choose File > Save As.
5. Select Part (*.sldprt) as the file type.
6. Review the Save Assembly as Part options and included components.
7. Save to a new filename so the purpose and revision are clear.

Current versions can include or remove components using criteria such as external visibility, component volume, and whether an item is a Toolbox component. Component properties can also affect inclusion. Always inspect the preview or result instead of assuming an automatic criterion understands your design intent.

Choose how much geometry to include

The safest choice depends on the recipient:

• All required components: preserves the selected component bodies but can create a large multibody part.
• Exterior or visible geometry: removes internal details and is useful for envelope models, but may omit openings or internal interfaces the recipient needs.
• Specified components: gives more control when only selected housings, brackets, interfaces, or reference items matter.

For repeat work, create a dedicated export configuration or display state rather than manually hiding components every time. Name it clearly and document its intended recipient and level of detail.

Use Defeature when Save As is not controlled enough

Tools > Defeature provides a guided simplification workflow. It can remove components, preserve selected features or faces, simplify groups by silhouette, and save the result as a new document or configuration. It is better than a basic Save As when you need to protect details, control interfaces, or generate a repeatable simplification.

SOLIDWORKS offers Simplify Geometry and Silhouette methods. Simplify Geometry removes selected components and details. Silhouette creates simplified bodies from component or body outlines using methods such as bounding boxes, cylinders, polygon outlines, tight-fit outlines, or copied geometry.

Defeature step 1: choose components or groups

Start by deciding what should disappear and what must remain. Depending on the method and version, you can remove internal components, small components, Toolbox items, or manually selected components. With the Silhouette method, define logical groups and choose a simplification method for each group.

Keep mounting interfaces, connector locations, clearance-critical surfaces, and reference geometry that the downstream user needs. Remove fasteners, internal mechanisms, cosmetic details, and proprietary geometry only when they are not required for fit or function.

Defeature step 2: decide whether motion must remain

If groups must move relative to one another, preserve motion deliberately. A result that allows motion may remain an assembly instead of becoming a single part. For a static envelope, group components accordingly and produce a fixed simplified result.

Defeature step 3: retain critical features

Keep holes, faces, or other features that define mounting, connection, or clearance requirements. Threaded ports, bolt patterns, locating faces, shaft centers, and fluid connections are common examples. Removing them can make the simplified model unusable even when its outer shape looks correct.

Defeature step 4: remove remaining faces or details

Review the simplified preview and remove details that survived the automatic rules. Adjust the earlier criteria when possible rather than building a long manual cleanup list that is difficult to maintain after source changes.

Defeature step 5: save and manage the result

At the final step, choose how the simplified model should be managed:

• Save as a new document: creates a separate simplified file.
• Link to Original: allows the defeatured result to update from the source, but adds an external-reference dependency.
• Create a new configuration: stores a derived defeature configuration when the selected method supports it.
• Store settings for future use: retains the Defeature choices in the source model.

An independent file is easier to send but does not update automatically. A linked result can stay current but may fail when paths, permissions, or source files change. Choose based on the delivery workflow, not convenience during export.

Verify the saved part before sharing it

• Open the saved part independently and force a rebuild.
• Check body count, file size, and external references.
• Use section views to confirm internal geometry is removed.
• Measure mounting faces, hole locations, envelopes, and connector positions.
• Confirm proprietary details are not visible through openings or surface bodies.
• Insert the simplified part into a test assembly and perform a clearance check.
• Export to STEP or another neutral format only after the SOLIDWORKS part passes review.

For clearance verification, see collision detection in SOLIDWORKS. If the full assembly is slow before simplification, review SOLIDWORKS Large Assembly Mode and the CAD desktop workstation guide.

Common problems

The saved part is still too large

Exclude small, internal, or Toolbox components; use exterior geometry or Defeature; and remove unnecessary surface bodies and cosmetic detail.

Required holes disappeared

Return to the source assembly or Defeature settings and explicitly retain the mounting or connection features. Do not repair the exported part manually if the workflow needs to be repeatable.

The result has many separate bodies

That may be expected when component geometry is preserved. Use an appropriate simplification method or enclosing body only when a single envelope body meets the downstream requirement.

The linked simplified model will not update

Check external references, source paths, permissions, and whether the original assembly is accessible. Break the link only when an independent frozen result is intended.

The recipient needs an editable assembly

Do not send a saved part. Use Pack and Go or another controlled assembly-delivery method that includes the required component files and references.

Bottom line

Use Save Assembly as Part for a quick, controlled conversion to a simplified part. Use Defeature when you need repeatable removal rules, silhouette simplification, retained interfaces, or stronger intellectual-property protection. In both cases, keep the source assembly as the master and verify geometry, references, clearances, and hidden details before sharing the result.

Official references: Saving an Assembly as a Part, Defeature, and Defeature Complete.