There are two methods to update existing SOLIDWORKS files for 3DEXPERIENCE compatibility. 

System-Defined Update Logic

The name and Part number displayed when used in a bill of materials property, for each configuration, determines whether a configuration is updated to a Physical Product configuration or a Representation configuration. The following logic, which applies to parts and assemblies, satisfies the majority of use cases.

3DEXPERIENCE SOLIDWORKS

Collaborative Designer for SOLIDWORKS +
SOLIDWORKS 2023 SP4.0 and newer versions
 

• If there is a configuration named Default, it takes precedence to update as a Physical Product configuration.

• Document Name updates to a Physical Product configuration.

• If there are multiple configurations with this property and one is named Default, then all others update as Representation configurations of Default. 

• If there are multiple configurations with this property and none are named Default, then the first history-based configuration updates as a Physical Product configuration, and all others update as Representation configurations of the first.

• Derived configurations with this property update as Representation configurations.

• Configuration Name updates as a Physical Product configuration.

• Derived configurations with this property update as Physical Product configurations.

• User Specified Name updates as a Physical Product configuration.

• If a User Specified Name matches a Configuration Name, then it updates as a Representation configuration of the matching Physical Product configuration.

• Derived configurations with this property update as Physical Product configurations.

• Link to Parent Configuration updates as a Representation configuration.
 

Collaborative Designer for SOLIDWORKS +
SOLIDWORKS 2023 SP3.0 and older versions
 

• Document Name updates as a Representation configuration and the system automatically creates a parent Physical Product configuration with a name that equals the Windows file name.

• Derived configurations with this property update as Representation configurations.

• Configuration Name updates as a Physical Product configuration.

• Derived configurations with this property update as Physical Product configurations.

• User Specified Name updates as a Physical Product configuration.

• Derived configurations with this property update as Physical Product configurations.

• Link to Parent Configuration updates as a Representation configuration.

Here is an example of what to expect when you update legacy files for 3DEXPERIENCE compatibility:

User-Defined Update Logic | 3DEXPERIENCE Integration Rules Editor

If you have very specific use cases or company standards to follow where the system-coded update logic does not give you the desired result, then you can create user-defined update logic instead using the 3DEXPERIENCE Integration Rules Editor. 

NOTE: This utility is only available in 3DEXPERIENCE SOLIDWORKS and Collaborative Designer for SOLIDWORKS + SOLIDWORKS 2024 SP0.1 and newer versions.

Unlike the system-defined update logic, which applies to parts and assemblies, the 3DEXPERIENCE Integration Rules Editor allows you to define different update logic for both file types, if needed. Defining update logic requires two sets of rules:

• Sub-typing rules: These rules categorize your part and assemblies files.
• Configuration mapping rules: These rules determine if a part or assembly sub-type will update as a single Physical Product configuration with Representation configurations, or multiple Physical Product configurations.

Combined, the rules determine how parts and assemblies are updated for 3DEXPERIENCE compatibility. For example:

1. In the Sub-typing rules pane on the Parts tab, click the + button.

2. In the Sub-Type Rule Definition dialog, enter a description for the rule.

3. Define a condition that identifies the parts based on any combination of: filename, custom property, is sheet metal part, or is weldment part. In this example, a custom property named MakeOrBuy that equals Buy is defined.

4. Give the sub-typing rule a name, then click OK to save.

5. Select a sub-type rule.

6. Choose a configuration mapping. In this example, Multiple physical product.

7. In the Configuration Mapping Rule Definition dialog, enter a description for the rule.

8. Define a condition that identifies the parts based on any combination of: configuration name, configuration property, configuration BOM option, active configuration, or first configuration. In this example, a configuration property named PartNo that starts with the number 900.

9. Choose a configuration mapping object type. In this example, Physical Product.

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10. Click OK to save the rules.

NOTE: Your rules are saved to an XML file. By default, the XML file is saved to [%appdata%\SolidWorks\SOLIDWORKS 20XX\3DXIntegrationSubTypeRules]. If you want to share the rules to other users, you can either send them the XML file or you change the file location to shared network location that all users have access to. If you understand the structure of the XML file, then you can edit it in any XML editor or text editor.

Continue creating sub-typing rules and configuration mapping rules that you need. With both sets of rules defined, when you update files for 3DEXPERIENCE compatibility, whether you do so manually or automatically, files that meet the conditions will update per your user-defined rules.

See the Recommended Strategies for Working With Part and Assembly Configurations page for best practices on when to map configurations to multiple Physical Product configurations and when to map to a single Physical Product configuration with Representation configurations.

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