Home » How to Create a Configuration in a Part/Assembly in SolidWorks?

You can create Configurations in a Part/Assembly file to allow you to store multiple versions of that part or assembly in a single file. SolidWorks Toolbox components use configuration extensively to create families of parts with different dimensions, features, and properties. You can create configurations to store the mirrored version of the part.

Configurations are used to create simplified versions of parts and assemblies by suppressing computationally heavy features such as Patterns and Fillets or by suppressing highly detailed components altogether in assemblies. Simplified versions are useful when you are creating a very large or complex assembly or when you need to perform simulations on the part (running a simulation on a highly detailed part may take a long time).

Configurations can save a lot of time when you want to perform modifications before proceeding further with your design and also want to keep the original design because you don’t have to start from scratch, and also features added to the part after the modification will be available in both versions.

There are 3 methods of creating configurations:

  1. Create configurations manually.
  2. Use design tables to create and manage configurations in a Microsoft Excel worksheet.
  3. Use the Modify Configurations dialog box to create and modify configurations for commonly configured parameters.

Method 1: To create a configuration manually:


1. In either a part or assembly document, click the ConfigurationManager tab at the top of the FeatureManager design tree to create a new Configuration. In the ConfigurationManager, right-click the Part or Assembly Name and select Add Configuration.

2. In the Add Configuration PropertyManager, type the Configuration Name and Description. Specify properties for the new configuration as per your requirements.

Select Suppress Features options under the Advanced Options menu if you want all the features that are added afterward in other configurations to be suppressed in this one.

Tip: Check Use Configuration Specific Color to automatically apply the selected color to the features that have been changed in this configuration. Useful when the differences are not clearly visible such as in complex parts or large assemblies.

3. Click Ok and now you will have a new configuration available. Click the FeatureManager design tree tab to return to the FeatureManager design tree.

4. Modify the model as needed to create the design variation by changing dimensions, and appearances or by adding and suppressing features. When you are changing a dimension, you can specify whether you want to change that dimension for this configuration, for some specific configurations, or for all configurations by clicking on the Configuration icon.

The name of the configuration in which you are currently working will be stated at the top of the Feature Tree along with the Part’s/ Assembly’s name.

Some features or options inside a feature do not support variations and hence, these features can’t directly be edited to create variations for Configurations. In order to remedy that, suppress the original feature and make a new one with the desired inputs.

5. You can switch between the new configuration and the old one by double-clicking on them in the ConfigurationManager.

For this tutorial, we changed the height of the screw bolt in this configuration.

Method 2: Creating Configurations using the Design Table:

1. To create a Design Table, click Insert -> Tables -> Excel Design Table. (You must have Microsoft Excel installed on your machine to use Design Tables in SolidWorks). This will launch the Design Table PropertyManager.

2. Here, select Auto-create in the Source menu. (You could also use a blank or linked Excel file but that file should be formatted as formatting in Design Tables is very important). Under the Edit Control menu, you can choose whether or not you want the Design Table to be updated by the edits in the SolidWorks file.

3. Click OK, and Excel will launch inside of SolidWorks. You can use all the powerful tools and commands provided by Excel to edit your Design Table.

To create new a configuration, type the name of the new configuration in the cell below the existing configuration(s). You can create as many configurations as you want by adding their names in the Configurations column.

You can also use the Design Table to create and modify configurations for parameters such as:

  • Dimensions and suppression state of features in parts and assemblies.
  • Configuration properties such as part number in a bill of materials, derived configurations, equations, sketch relations, comments, materials, and custom properties in parts and assemblies.
  • Suppression state, referenced configuration, fixed or floating position of components in an assembly.
  • Dimensions of distance and angle mates and suppression states of mates in an assembly.

When done editing the Design Table, click anywhere in the Solidworks window to return to SolidWorks. You will receive a message for all the new configurations that have been created by the Design Table and the model will update itself according to the changes made in the Design Table.

4. You can always find this Design Table in the Tables folder under ConfigurationManager Tab. Double click on the table to edit it.

Method 3: Creating Configurations using Modify Configuration:

1. You can access the Modify Configuration Table by right-clicking on a dimension or feature and selecting Configure Dimension or Configure Feature.

2. Now, Modify Configurations table will be presented. You can create new configurations and also specify values for the feature or dimension on which you right-clicked. You can also suppress or unsuppress them here.

After you are done, save the table by giving it a name and then clicking on the Save icon.

3. You will now find that the New configurations had been added.

So, in this quick tutorial, you have learned three different ways to create a new configuration. When inserting these parts/assembly files into an assembly SolidWorks will ask you which configuration you want to add and you can choose it there. Also, when you select components or subassemblies in an assembly, a context toolbar appears and if your selection has multiple configurations, you can change the configuration from the context toolbar.