Understanding SOLIDWORKS Feature Scope

Article by Brandee Videcak updated February 12, 2024

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When creating a model, there are many features that we use regularly to help us achieve the model we intend to create. Many of our feature-based commands within SOLIDWORKS have additional options in the feature PropertyManager that allow us to further define the scope of that feature. Let’s take a few moments to focus on the SOLIDWORKS Feature Scope options available for some of our feature-based commands.

The Feature Scope tool within many features in SOLIDWORKS, will allow you to specify which body or bodies are being selected for the desired feature. This is beneficial when you only want specific areas of the multi-body part or assembly to be affected by these changes.

Where to find the SOLIDWORKS Feature Scope

The Feature Scope area will appear in the Property Manager of the specific feature you are looking to complete, shown below with a cut-extrude for this example.

The SOLIDWORKS Feature Scope is circled in red within a Cut extrude Property Manager

The SOLIDWORKS Feature Scope is circled in red within a Cut extrude Property Manager

When you expand this area, there are a few main options that you will see, and depending on what you select, will activate additional options. The main two options you will see are All and Selected [Bodies or Components], depending on if you are within a multibody part or assembly, respectively.

By selecting the option All [Bodies or Components], the modification made will be affected by all the bodies or components within the model each time the feature regenerates. If a new body or component is added to the model that intersects the feature, the new body/component is regenerated to include the feature.

The next option listed is Selected [Bodies or Components]. By enabling this option, SOLIDWORKS will then provide some additional options for you to select, depending on whether you are within a multi-body part or assembly.

Feature Scope in a SOLIDWORKS Multibody Part

Within a multibody part, the next option that is enabled when selecting Selected Bodies would be the Auto-select checkbox, as well as an area to indicate the solid bodies that would be affected. If Auto-select is enabled, it will select and process all the relevant intersecting parts, and only regenerate those bodies, versus the entire model. If you deselect the auto-select checkbox, then you will select the bodies that are to be affected in the graphics area of the part. These bodies will be highlighted and shown in the Solid Bodies to Affect box.

Highlighted body in green in the graphics area is the specific body enabled for feature scope

Highlighted body in green in the graphics area is the specific body enabled for feature scope

Feature Scope in a SOLIDWORKS Assembly

For an assembly file, you will see the same options as the multi-body part, along with an additional selection, Propagate feature to parts.

This option is available to select when either All or Selected components are enabled. With the Propagate feature to parts option enabled, you will see the same feature being included in your individual part file as well as the overall assembly. If you do not wish for the modification to be made to the individual part files, such as ones in other assemblies or to be used elsewhere, then de-selecting this option is the best way to go.

An additional note when selecting Selected Components in the assembly, is if you add a new component to your assembly, and want the feature to affect the new component, right-click on the feature and select ‘Edit Feature’. You can then add in the additional component to be affected. If you add in the new component, the feature will not automatically affect this component.

 

Selected components is selected, indicating the components in blue in the graphics area

Selected components is selected, indicating the components in blue in the graphics area

The Feature Scope options allow you to gain more control over your model and help create a very efficient workflow for adding features to multiple entities.

Learn more about the SOLIDWORKS Feature Scope

Attend a live online SOLIDWORKS Advanced Part Modeling training course from Javelin to learn more about using the feature scope along with other advanced features

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Brandee Videcak

Brandee Videcak is a Client Success Analyst with Javelin/TriMech