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SolidWorks Defeature: How to Share a Model Without Giving Away Your Design

SolidWorks Defeature guide for sharing models without exposing IP
SolidWorks Defeature is the built-in tool that strips the design detail out of an assembly, a multibody part or a single-body part and saves what is left as dumb solids: solids with no feature definition and no feature history. The SOLIDWORKS Design Help 2026 (read 16 November 2026) states the purpose plainly: you can share the new file without revealing the design details of the model. For anyone who sends models to suppliers, customers or contractors, that makes Defeature the first IP filter you already own.
This guide covers the two Defeature methods, the PropertyManager pages that decide what leaves your company, the save option that keeps your full design out of the shared file, and a pre-send check. For the wider risks of sending models out, start with our guide to sharing CAD files with suppliers.

What does SolidWorks Defeature do?

Defeature builds a less-detailed copy of your model. Internal components disappear, small parts drop out, holes and other features are removed, and the result is saved as geometry without a feature tree. A buyer still sees the envelope, mounting points and overall shape. The sketches, feature order and design intent behind the model stay at home.
You start it from Tools > Defeature or the Defeature button on the Tools toolbar. The options you pick are stored in the original model, and a Defeature item appears in its FeatureManager design tree. Right-click it later to Edit Feature, Save Result, Save Result with Link or Delete, so a supplier who asks for an update next month gets a fresh copy in a few clicks.

Simplify Geometry or Silhouette: which Defeature method should you use?

SolidWorks gives you two methods. Simplify Geometry removes selected components and geometry details from the top-level assembly. Silhouette creates a simplified part from the silhouette outlines of components and bodies. Here is how they compare, based on the SOLIDWORKS Design Help 2026 pages for each method.
QuestionSimplify GeometrySilhouette
What you getYour model with components, bodies and features removed; saved parts carry Defeatured1 featuresNew bodies built from outlines: a box, cylinder, polygon outline, tight fit outline or an exact copy
Works onAssemblies, multibody parts and single-body partsAssemblies and parts
How you control itPages: Components or Bodies, Motion, To Keep, To RemoveDefeature groups, each with its own simplification method; rule sets for assemblies
Moving partsYes: the Motion page keeps motion between groupsNo motion page
Save as a configurationNoYes, as a derived configuration
Good fitA customer model that still shows real holes and interfacesSpace claims, layout models and heavy assemblies that need to become a light block

How does the Simplify Geometry method work?

Simplify Geometry walks you through a set of PropertyManager pages. Which pages you see depends on the model: an assembly opens on Components, a multibody part on Bodies, and a single-body part goes straight to To Keep.

1. Components or Bodies

Three removal rules do the heavy lifting. Internal components (or internal bodies) removes everything that is not visible from outside the model. Small components removes every component, inside or outside, that is smaller than the percentage of the model’s bounding box you enter. Selected components removes the items you pick. The Exceptions box keeps anything a rule would otherwise throw away, and a section view lets you see and select what sits inside.

2. Motion

Assemblies that need to move for the recipient get a Motion page. You group components, and SolidWorks allows motion between groups but not between components inside one group. The page lists the mates that survive. When you allow motion, the result is saved as an assembly with one component per group, so a customer can still check a hinge or a slide without seeing what drives it.

3. To Keep

Defeature removes external holes on parts and components automatically unless you tell it to keep them. That is the setting most people miss: a supplier who needs mounting holes gets a flat plate unless you add them here. Select all holes keeps every hole, and Select holes between keeps holes in a size range you enter. You can also keep subassemblies, parts, features (including assembly features and suppressed features), reference geometry, routing points and sketches.

4. To Remove

This page takes items that Defeature does not remove on its own: subassemblies, parts, features, reference geometry, routing points and sketches. Use it for the one feature that gives your design away, such as an internal channel that shows up in the outer shape.

How does the Silhouette method work?

Silhouette works with defeature groups. You add components or bodies to a group and give each group a simplification method:
  • Bounding Box: a cuboid around the group.
  • Cylinder: a cylinder derived from the dimensions of that cuboid.
  • Polygon Outline: an extruded polygon that fits around the outline of the selection.
  • Tight Fit Outline: an extruded body that follows the outlines of the selection; Keep internal loops adds holes that show in the silhouette.
  • None (Copy Geometry): an exact copy, with Propagate visual properties to carry appearances and textures.
Extra options decide how much survives. Enclose in one body turns the selection into a single body, Ignore small bodies drops bodies below a percentage of the assembly or part size, and Merge groups after this step joins groups that touch or overlap. You can set the orientation plane yourself and add a second direction for outline methods. In assemblies, the Apply Defeature Rule Sets page creates a set of rules to simplify the components, which pays off when the same kinds of parts go out every week.

How should you save a defeatured model for sharing?

The last page, Defeature Complete, decides where the result lives. This is the step with the biggest IP consequence.
OptionWhat SolidWorks doesUse it for
Save as a new documentSaves the less-detailed part or assembly as a separate file with no references to the original. Link to Original is optionalEvery file that leaves your company
Create a new configurationSaves the result as a derived configuration of the fully detailed model (Silhouette method only)Light stand-ins inside your own projects
Store settings for future useSaves the Defeature options in the original model so you can rerun themRepeat jobs for the same customer or supplier
A configuration lives inside the original file, next to the full design. Sending that file sends everything, so for anything external use Save as a new document and leave Link to Original unticked. If you did link it, right-click the model, open External References and break the reference before the file goes out. SolidWorks also warns that switching components between the defeatured configuration and the parent configuration leaves dangling references such as annotations and dimensions. Our guide to SOLIDWORKS external references explains the difference between locking and breaking them.

How do you defeature an assembly for a supplier, step by step?

  1. Write down what the recipient needs: overall size, mounting holes, interfaces, moving parts or only a visual model.
  2. Open the assembly and click Tools > Defeature.
  3. Pick Simplify Geometry when real holes and interfaces matter, or Silhouette when a block or outline is enough.
  4. Remove internal components and small components, and add exceptions for anything the recipient needs.
  5. Group moving components on the Motion page if the customer has to check a mechanism.
  6. On To Keep, add the holes the supplier needs, since external holes go by default.
  7. On To Remove, add any sketch, routing or feature that still reveals your know-how.
  8. Choose Save as a new document without Link to Original, and give the file a name that tells your team it is the shared copy.
  9. Open the saved file on its own and run the check below before you export it.

What should you check before you send a defeatured file?

Defeature handles geometry. The SolidWorks help pages for the tool say nothing about custom properties, file summary information or the file name, so check those yourself.
  • Open the new file on its own and cut a section in two directions to confirm nothing internal is left.
  • Open File > Properties and clear part numbers, project names, author and customer fields the recipient has no reason to see.
  • Confirm there is no external reference to the original model.
  • Pick the export format on purpose. Our page on neutral CAD file formats and their security risks explains what STEP, IGES and Parasolid exports still carry.
  • Share through a channel you control, as described in our secure CAD file sharing guide, and encrypt files that travel by email or cloud links (see CAD encryption methods).
  • Log the file, version, recipient and date, so you can prove later what you sent and to whom.

Where does Defeature stop protecting your IP?

A defeatured model still shows the outside of your product, and the outside can be measured, copied and reverse-engineered. The most common CAD file sharing vulnerabilities have nothing to do with geometry at all: wrong recipients, open links and old versions that never get revoked. Our overview of IP theft in the CAD industry shows how designs leak once they leave the building.
That is why Defeature belongs next to contracts, access control and proof of authorship. NDAs alone leave gaps for CAD files, so control who opens what with access management for external collaborators and role-based access control, and keep a dated record of your original design. BORIS for SolidWorks is a plugin that registers the existence of your design on the blockchain from inside SolidWorks and gives you a verifiable blockchain certificate of authorship or ownership, so you can prove the design was yours if a shared model turns up somewhere it shouldn’t. Try BORIS for SolidWorks, read our guide to securing SolidWorks files and our steps to prevent IP theft in architecture with SolidWorks. Autodesk Inventor users have a matching tool: see our sister guide to Inventor Simplify.

FAQ: SolidWorks Defeature

Where is the Defeature tool in SolidWorks?

Click Tools > Defeature, or the Defeature button on the Tools toolbar. Pick Simplify Geometry or Silhouette on the first page of the PropertyManager.

Does SolidWorks Defeature work on parts?

Yes. Simplify Geometry works on assemblies, multibody parts and single-body parts, and Silhouette works on assemblies and parts.

Why did Defeature remove my holes?

Defeature removes external holes on parts and components automatically. Add them on the To Keep page with Select all holes or Select holes between.

Is a defeatured file linked to my original model?

Only if you tick Link to Original when you save it as a new document. Without the link, the file has no references to the original. A linked file can be unlocked or broken through External References.

Can I send a defeatured configuration instead of a new file?

A configuration is stored inside the original file next to the full design, so sending it sends the full model. Use Save as a new document for anything that leaves your company.

Can a defeatured assembly still move?

Yes, with Simplify Geometry. Group components on the Motion page; motion is allowed between groups, and the result is saved as an assembly with one component per group.

Does Defeature remove custom properties?

The SolidWorks help pages for Defeature don’t say so. Open File > Properties in the saved file and clear anything the recipient doesn’t need.

Does a defeatured model fully protect my design?

No. The outside shape still leaves with the file. Combine Defeature with contracts, access control and a dated proof of authorship such as a BORIS for SolidWorks certificate.