Assembly Size Ranges

SOLIDWORKS configurations are a powerful feature that allow you to create variations of a design within a single file. When working with assembly size ranges, configurations can be particularly useful. The common uses cases include, but are not limited to, creating:

1. Product families
2. Parametric design

Maintaining one Physical Product configuration per SOLIDWORKS file reduces unnecessary complexity for all SOLIDWORKS and 3DEXPERIENCE platform users within an organization.

The recommendation is to not use multiple SOLIDWORKS configurations and instead use a single Physical Product configuration. In order to handle the product structure, the best practice is to create multiple assembly files with single Physical Product configurations. If you have legacy data with multiple SOLIDWORKS configurations, then it is recommended to use the Save Configurations command to save each configuration as a separate assembly file.
 

Mirrored Components and Split Parts

When you create opposite-hand mirrored components as new files or you create split parts, and the base part has multiple configurations, the resulting derived part is created with multiple configurations that map to the base part configurations. You can edit the external reference of the derived part and change the referenced base part configuration if you need to. In these types of derived parts, SOLIDWORKS does not enforce any external reference after the derived part is created.

The recommendation for these types of parts is to create one Physical Product configuration and create SOLIDWORKS Representation configurations for any additional design needs. This means that if you add a new Physical Product configuration to your base part, SOLIDWORKS will not automatically create a matching Physical Product configuration in the derived part. It is your responsibility to create a corresponding Physical Product configuration in the derived part if needed. And then you can then edit the external references in the derived part to map to the appropriate Physical Product configuration in the base part.

In the case of opposite-hand mirrored components, the components should have a unique Enterprise Item Number and should be independently life-cycled. Therefore, the recommendation is to always create opposite-hand mirrored components as new files, instead of creating derived configurations in the base part. This way, the components will have individual Physical Products configurations, with individual Enterprise Item Numbers. Only create multiple Physical Product configurations in mirrored components if all the components have the same lifecycle.

Alternate Component Positions

While designing, users can configure whether the position of a component is fixed or floating in an assembly. To fix or float an assembly component:

1. Right-click the component. 
2. Select Fix or Float, and then one of the following options:

•  This configuration
•  All configurations
• Specify configurations

When incorporating an assembly containing dynamic components into a larger assembly, the default behavior restricts the movement of those components. If you intend to enable these movements within the top-level assembly, you must adjust the properties. To do so, right-click on the subassembly within the assembly tree and open the properties window. From there, you can switch the assembly from "Rigid" to "Flexible," and your desired functionality will be achieved. Users should use flexible assemblies in one Physical Product configuration. It's a current limitation that 3DPlay will only show the Physical Product positioning, not the flexible positions.

Simplified Assemblies 

Cosmetic features add edges and faces without helping assure their fit and function within assemblies. In some cases, these features can double the total number of faces in an assembly and lead to a degradation of performance in assemblies and especially in drawings. You can use a detailed version for the part design, and a simplified version for higher-level assemblies referencing the part design. Each version can be stored as a different configuration. 
In some cases, such as purchased parts, a highly detailed model is not necessary. Use the Defeature tool or the Simplify utility to automatically reduce the face count, edge count, and file size of the model. You can also strategically target cosmetic features. You should first target the parts used most often. Common examples include:

• Internal components, such as rollers in bearings
• Threads
• Extruded text
• Vents and fasteners on purchased parts

These configurations get created as Representation Configurations.

SpeedPak Configurations

SpeedPak configurations can help reduce the amount of data that's required to be loaded in a sub-assembly or top-level assembly, and they may be enough to fully represent the model. A good application of SpeedPak configurations is with purchased parts and imported files. 

When an imported part does not import cleanly - for example, with many unknit surfaces - you can create a SpeedPak configuration to keep only the geometry that is necessary. Faces and reference geometry can be defined within the SpeedPak configuration for use in mates. 

An important consideration is that SpeedPak configurations increase the file size of the part or assembly because you are adding a new configuration to the file. Despite this, it is faster to open or reference a SpeedPak configurations. Thus, SpeedPak configurations should be created as SOLIDWORKS Representation configurations.

Display States

Display states can be seen or used as a lighter weight version of a configuration. You can and should use configurations to store different designs of an assembly, however if you want to show different displays of an assembly, use display states. Think of a configuration as an entirely new assembly contained within the file. Assemblies (and parts) with configurations contain much more data than assemblies that only use display states. 

Display states store information about appearances (including transparency), and the hide/show state of components. For example, if you want to show different colors of components, or hide or isolate certain components, it is much more efficient to represent that display of the model with a display state than with a configuration. Using display states also mitigates file size increases and reduces the need to rebuild an assembly.

Likewise, if you need to show different displays in drawings, then you should also use display states instead of configurations. If your drawing references multiple configurations of an assembly, then you must update each of those configurations before the drawing can update. Whereas an assembly with a single configuration, with multiple display states, only needs to update once.

To summarize, one Physical Product configuration will represent each part and assembly file in the 3DEXPERIENCE platform.

• Maintain one Physical Product configuration per part and assembly file.
  • A single Physical Product configuration represents the engineering definition of the component.
    • Lifecycle information
    • Enterprise Item Number
    • Attribute information
• Create additional configurations as SOLIDWORKS Representation configurations.