What is a Configuration in SOLIDWORKS?
A configuration is a file which is stored internally within parts or assemblies. For parts, different versions of a model can be created by suppressing certain features or changing dimensions.
For example, in the below model, we need to add a small tab to an existing model. Configurations allow an identical model to be copied and the new tab feature to be suppressed in the original model.
Two configurations of the same part.
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Learn More When should you use SOLIDWORKS Configurations?
Configurations are great to use in situations where a part or assembly may be similar to another, but it would be time consuming to recreate it.
For assemblies, you may need to show different positions or modes for a model. In the example below, three separate versions of an assembly have been created by suppressing and un-suppressing components in each configuration.
Three configurations exist within one subassembly file. How to Create Configurations in SOLIDWORKS
Configurations are stored in the dedicated ‘configuration manager’ tab, this is where you will come to view, change, or edit configurations. Every part or assembly begins with a ‘default’ configuration. This can be deleted or renamed if necessary.
A new configuration can be added by right clicking in a blank area of the configuration manger and clicking add configuration.
There are multiple ways to start creating new configurations besides the above method.
If you right click on a feature, sketch dimension, or part in an assembly you will see the ‘Configure [Item Name]’ option. This will open a configuration table for the selected parameters, allowing you to suppress or modify properties.
What are Derived Configurations?
Note that if an existing configuration is right clicked, a different option to ‘add derived configuration’ will appear. This type of configuration will automatically inherit all parameters of the ‘parent’ configuration, creating a parent-child link.
A derived configuration is used to show holes on a machined configuration and hide them on the default. This could be used in situations where it is important for a configuration to copy major geometry changes from the parent but include additional features such as final machining operations.
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SOLIDWORKS Configuration Tables Explained
The SOLIDWORKS configuration table allows you to easily configure multiple parameters in a single table.
Activate the table by right clicking the first part, feature, or sketch dimension which you would like to modify and then ‘configure’.
Once the table is open, new parameter columns can be added by double-clicking additional features, dimensions, or parts. Columns can be deleted by right clicking the header and any associated feature dimensions can be added as columns using the drop-down arrow in the header.
Use configuration tables to quickly suppress and edit multiple design parameters. You can learn more about how to use Configuration tables in SOLIDWORKS in this detailed tutorial.
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Learn More Using Configurations in Assemblies
Assembly configurations are great way to show different layouts and structures to use for drawings or assembly guides. You can configure components, subassemblies or assembly features and patterns by suppressing by suppressing, unsuppressing and modifying values. You call also suppress and create new mates in configurations to change component positions.
Parts, subassemblies, and top-level assemblies can all be configured. The possibilities quickly multiply with every assembly level, so it is important to understand how each level interacts with one another. We will take you through an example workflow to show you what to do when creating assembly configurations.
Here we have two different part configurations for a claw machine prize box. One includes a red tab which will be used in a different claw machine game, requiring a separate configuration.
To change the configuration of a part in an an assembly, simply left click on it from the graphics area or within the feature tree. Then use the drop-down menu to select the required configuration.
Changing the prize configuration in the top – level assembly. Using Subassemblies to Organise Configurations
In theory, all top-level configurations could be controlled by configuring individual parts both at the top level, and those stored in subassemblies.
Two different game versions, created by suppressing, adding, and configuring parts. However, to avoid making mistakes and to allow different versions of several parts to be used in other assemblies, it is best practice to create subassembly configurations.
In this case, we have three separate subassembly configurations where the claw machine games will be laid out.
The ‘with tab’ configuration will be used in the ‘Game 2’ configuration. When configuring subassemblies, make sure to activate the configuration you are working on by double clicking it. Then, configure components by suppressing them or changing part level configurations.
In cases where you have several design parameters or hundreds of configurations to create, consider using a design table created in a Microsoft Excel spreadsheet.
For more information on using design tables and creating multiple configurations at once, check out this tutorial for advanced SOLIDWORKS techniques.
Creating Top-Level Assembly Configurations
Now it is time to add the different games to the top-level assembly. Currently, there is only the ‘default’ configuration where neither game is specified.
The top-level configuration manager where only ‘default’ currently exists. When configuring subassemblies rather than parts, it is very important to select the subassembly from the feature tree rather than individual parts. This ensures that the configuration being changed is that of the entire subassembly. This can also be achieved by right clicking a part and then ‘select subassembly’.
Left click the subassembly from the feature tree, then change configuration. After clicking ‘select subassembly’ you can change configuration using the drop-down as normal. To represent four different game modes layouts, four new top -level configurations are created.
New configurations created and named. However, there is an issue in this case. When switching back to the default configuration, the original setup has changed.
The default configuration is now showing the ‘Game 1’ subassembly configuration. The problem here is that the game subassembly sits within another subassembly layer. Currently there is only one ‘default’ configuration for this subassembly and as a result, all configurations of the top level will only ever show one version of the game configurations.
To fix this, we must add configurations within the necessary casing subassembly to represent the games in each configuration.
It is best to think of assembly configurations like a chain, if you miss a link in the chain, the top level will not be able to recognise the full array of configurations which might be stored in lower subassemblies and parts.
Flow chart representing the importance of adding configurations at each assembly level. Finally, we have four different claw machine configurations to demonstrate the various ways in which it could be set up.
The final configurations for the claw machine assembly. Using Configurations in Drawings
Configurations can also be inserted into SOLIDWORKS drawings. Fabricators and those who work with sheet metal parts will be familiar with the flat pattern tool, which is a configuration in itself.
To use configurations in drawings, we can choose the desired configuration when inserting a drawing view to make a new drawing.
Existing drawing views of parts and assemblies with configurations can also be modified to show each configuration by selecting the drawing view and using the 'Reference Configuration' drop-down menu inside the property manager to change the configuration displayed.
Tips for Working with Configurations
Configurations are a great way to save time when representing different versions of a model.
It is important to carefully consider how you want each subassembly to be configured and how this might behave when placed into a top-level assembly.
Let's run back over some of the best tips when working with configurations in SOLIDWORKS:
- Track through assemblies to ensure each subassembly layer has appropriate configurations.
- Select subassemblies in the feature tree before changing the configuration to avoid changing the configurations of parts instead when working in top-level assemblies.
- Use subassembly configurations to your advantage, rather than configuring all parts in the top-level assembly.
Configurations are covered in detail in the SOLIDWORKS Essentials training course and, if you ever get stuck using configurations or have any other SOLIDWORKS queries, then don't forget to make the most of your SOLIDWORKS subscription and get in touch with our expert Technical Support team.
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