Using Defeature: How to Protect your Intellectual Property (IP) with SOLIDWORKS

What does the Defeature Tool do in SOLIDWORKS?

The 'Defeature' tool is a SOLIDWORKS command used to simplify assembly components by removing unnecessary, unwanted, or sensitive details from a model.

This resulting, simplified model can be saved as a separate file, and all references to the original part or assembly are retained alongside the original mass properties and centre of gravity.

The SOLIDWORKS defeature tool serves two main purposes: protecting the intellectual property of your designs when sharing them externally, and improving performance when working with large models by reducing open and rebuild times.

Which SOLIDWORKS Defeature Method Should I Use?

There are two ways to reduce the complexity of a model with the defeature tool: Simplify Geometry and Silhouette.

When it comes to choosing the best method for you, as with many things in a design process, there's no easy answer. However, there are some basic guidelines to help you choose:

• Simplify Geometry - choose this method if the simplified model needs to closely match the original or you are working with small to medium sized assemblies.
• Silhouette - creates a highly-simplified version from the outline of all components and is the best choice when working with large and complex assemblies.

How to Use the Defeature Tool in SOLIDWORKS

We'll use the model of this track-setting machine to demonstrate how to use the defeature tool as it has a subassembly that we would like to defeature.

Method One: Simplifying Complex Geometry in SOLIDWORKS

Let's first walk you through how to use defeature to simplify complex geometry in SOLIDWORKS.

The defeature tool is found in the menus under Tools > Defeature

Step 1: Choose the Components to Remove

The first page of the simplify geometry option allows you to control the components to be removed in the simplified model.

1. Internal Components - select any internal components that you want to remove from inside your assembly.
2. Small Components - this is a threshold that allows you to specify a percentage of the assembly size below which components will be removed.
3. Display - switch between viewing components to be removed and components remaining.
4. Exceptions - any components that must not be removed go in this box; these will not be removed from the model even if they are considered 'small' or internal components.
5. Section View - temporarily section the assembly to aid selection of internal components.

Components can be selected from the FeatureManager tree or the viewport. After selecting the components you want to remove and keep, click 'Next' to take you to the next step in the process.

Step 2: Restrict Motion

If you need to prevent a recipient from moving components in an assembly, then this tab lets you specify which component groups and mates to restrict, without breaking relationships.

Select groups of components that have no movement between them, and list any mates to maintain between them when using Defeature.

Motion is not required for this example, but temporary sections can again be utilised to aid component selection.

Select the 'Next' button to progress to the next step.

Step 3: Choose Features to Keep

So far the process has focused on components and parts within an assembly. The third step in the defeaturing process is to pick specific features you want to keep in the model.

This helps to ensure you maintain any important geometry such as mounting holes or reference geometry.

The FeatureManager tree for this third step contains the following options:

1. Features to Keep - select features in the model to be kept intact when defeaturing.
2. Select All Holes - retain all holes in the assembly.
3. Select Holes Between - keep only holes where the size falls in a specific range.

Once all the relevant features have been selected we can hit 'Next' to progress to the next step

Step 4: Remove Any Additional Items

This step allows you to select any additional faces, features, bodies or components that have not been removed as they do not meet the criteria specified in previous steps.

Select Next to progress to the next step.

Step 5: Save The Document

The final screen shows you a comparison between the original file and the resulting defeatured model.

The two options we have for saving are:

1. Save as a new document - this saves the defeatured part file to your chosen file location. The checkbox 'link to original' allows you to control whether the model will maintain its link (and therefore references) to the original file.
2. Store settings for future use - this saves the defeature options into the original model but does not create a new file. Instead, the FeatureManager tree will contain a defeature entity which can be right clicked to save the model at a later date.

Method Two: Using 'Silhouette' to Defeature CAD Files

SOLIDWORKS 2024 introduced the ability to defeature using the 'Silhouette' option.

This method will utilise the outer edges of the assembly (known as the silhouette) to provide a defeatured model that preserves the existing volume while removing internal details.

Step 1: Apply Defeature Rule Sets

The first page of the property manager allows you to define a set of rules which can be used to simplify the model.

You can choose to load an already existing set of rules to apply to the model or you can create a new set of rules.

Selecting Edit Rules in the property manager opens the Defeature rules editor

You can then begin to specify rules based of SOLIDWORKS Properties. The rule above specifies that any components with a mass less than 210 grams will be replaced with a dumb solid of the components bounding box.

Select 'OK' to confirm the rules and hit next to move onto the next step.

Step 2: Set Up Component Groups

The next page gives you the options to create groups of components and specify how you would like to simplify them.

1. Groups – list all the groups that have been created. If you select them, you can then edit their definition below.
2. Edit a group – select components and bodies to be included in the group
3. Simplification Method – pick how the group selected in edit a group are simplified the options available can be seen in the image below.

4. When you hit “apply” SOLIDWORKS will open a preview window showing you the result of the current defeature groups.

Once all the group have been set up and you are happy with the result in the preview select next to move to the final step.

Step 3: Save The Silhouette Model

The final step in the defeature tool allows you to control how the defeatured model is saved.

This method gives us an additional option to the Simplify Geometry method that allows us to save the defeatured assembly as a configuration within the original model. The three save options are:

1. Save as a new document - save the defeatured part file to a chosen file location. The checkbox 'link to original' allows you to control whether the model will maintain its link to the original file.
2. Create a new configuration - create a derived configuration inside of the original part file. Check the option to “Include top-level reference geometry” to add reference geometry when defeaturing assemblies.
3. Save settings for future use- Saves the defeature options in the original model. The feature tree will contain a defeature entity which can be right clicked to save the model at a later date.

How to Replace Assembly Components with Defeature

Now that our subassembly has been suitable simplified, we can return to the top-level assembly to replace the original subassembly with our simplified version.

In the top-level assembly, we'll locate the component which has been defeatured, right-click on it, and select 'Replace Component' from the menu.

Select browse and locate the defeatured file.

Select 'Match name' and reattach mates and confirm the replace by hitting the green tick.

The result in the top-level assembly contains the defeatured component in place of the original. Replacing the component is the final part of the defeaturing process to simplify assemblies and protect your IP before sending your CAD data.

You can learn more techniques for working with assemblies in our Assembly Modelling training course, so you can equip yourself and your team with time-saving tools and enhance your workflows.

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