Revision History

Note

All SolidPractices are written as guidelines. It is a strong recommendation to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, Partners, and Customers that are on active subscription. You may not post this document on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.

This document was updated using 3DEXPERIENCE platform On Cloud R2024x FD02 and SOLIDWORKS Connected 2024 SP2.0. It is a companion to the wiki pages available in the SOLIDWORKS News & Info community. If you have questions or need assistance in understanding the content, please get in touch with your designated Partner.

Preface

This SolidPractices guide explains the recommended best practices for using SOLIDWORKS part and assembly configurations with the 3DEXPERIENCE platform. Configurations are a versatile toolset with many different use cases. Therefore, adopting the right strategy for using configurations with the 3DEXPERIENCE platform is important to avoid an unnecessarily complex experience for both SOLIDWORKS and other 3DEXPERIENCE users in your company.

Introduction to Using SOLIDWORKS Configurations with 3DEXPERIENCE

SOLIDWORKS configurations allow a user to represent different variations of a part or assembly within the same file. Common use cases for SOLIDWORKS configurations include capturing a size range of a part or assembly, different component positions within an assembly, and different levels of geometric detail, plus many more.

One of the key advantages of using SOLIDWORKS configurations is that all the different variations associated with a specific part or assembly are contained within the part and assembly file. The ability to apply design changes to specific configurations makes it easier to manage SOLIDWORKS files using the Microsoft® Windows file system because only one part or assembly file is created.

For example, when a user modifies a part or assembly that contains configurations, they can apply the change to all or individual configurations within the file.

, which is located within the same window as the FeatureManager design tree. The ConfigurationManager is available in every part and assembly. or a Microsoft® Excel spreadsheet-driven Design Table. (document name, configuration name, or user defined). When saving SOLIDWORKS parts and assemblies to the 3DEXPERIENCE platform, the Bill of Materials property may affect the amount of design information that becomes available to other users.EXPERIENCE platform that contain configurations, and before creating any new designs with the intention of adding configurations.

1. Data Model and Identifiers in the 3DEXPERIENCE Platform
2. SOLIDWORKS Data Model

Understanding the SOLIDWORKS Data Model and identifiers is a prerequisite for using and accessing SOLIDWORKS data within the3DEXPERIENCE platform.

1. Windows

In Windows (a file management-based platform), you create documents or files and you store that data in a file system. The file system is more commonly known as a hard drive or disk drive, and you use the File Explorer app to organize and access your data. Within this platform, apps create and use a wide variety of common file types (like TXT and ZIP) as well as app-specific file types. SOLIDWORKS creates and uses its own documents (SLDPRT, SLDASM, SLDDRW), document templates (PRTDOT, ASMDOT, DRWDOT), sheet formats (SLDDRT), library features (SLDLFP), and so forth. These app-specific file types are known as the SOLIDWORKS Data Model for Windows.

3DEXPERIENCE Platform

In the 3DEXPERIENCE platform (a Product Lifecycle Management (PLM) or data management-based platform), you create objects or content, and you store that data in a database. The database is more commonly known as a collaborative space. (The concepts of a file system do not apply.) Within this platform, apps create and use a wide variety of common content types (like Physical Product and Drawing) as well as app-specific content types. When you save SOLIDWORKS files to the 3DEXPERIENCE platform, the system does two things:

1. Uploads your SOLIDWORKS files to a File Collaboration Server (FCS).
2. Creates objects that represent and link to your SOLIDWORKS files.

The objects and object hierarchy are known as the SOLIDWORKS Data Model for the 3DEXPERIENCE platform. The objects are what you search for, interact with, and open in 3DEXPERIENCE platform apps. The following objects are created: 

• For each SOLIDWORKS part file, the system creates the following hierarchy:
  • One CAD Family object. This is a container for all configurations in the file.
    • One or multiple Physical Product objects. One for each configuration in the file.
      • One 3D Shape object for each Physical Product object.
• For each SOLIDWORKS assembly file, the system creates the following hierarchy:
  • One CAD Family object. This is a container for all configurations in the file.
    • One or multiple Physical Product objects. One for each configuration in the file.
    • One or multiple Embedded Physical Products for each virtual part.
• For each SOLIDWORKS drawing file, the system creates a Drawing object.

NOTE: For single-configuration part and assembly files, CAD Family and 3D Shape objects do not appear in 3DSearch, 3DSpace, or MySession. These objects are visible in some dashboard apps like Bookmark Editor, Product Structure Explore, and Relations. You cannot delete SOLIDWORKS-mastered 3D Shape objects. If you delete the CAD Family or Physical Product object that represents a SOLIDWORKS file or configuration, then the system automatically deletes the corresponding 3D Shape object as well.

You must be familiar with these four content types when using SOLIDWORKS and the 3DEXPERIENCE platform. 

Physical Product

, 3D Shape, and Drawing are common content types. CAD Family is a content type that is unique to external CAD (xCAD) apps like SOLIDWORKS.  

You can use the Relations app to visualize and better understand these objects and the object hierarchy.

SOLIDWORKS & 3DEXPERIENCE Platform Identifiers

Once you understand the SOLIDWORKS Data Model for the 3DEXPERIENCE platform, you can better understand the identifiers that are used within SOLIDWORKS. Understanding the identifiers is another essential part of using and accessing CAD data within the 3DEXPERIENCE platform.

1. File name is the unique identifier for Windows. It is the name of the file on disk and includes a file extension. After you save a SOLIDWORKS file to the 3DEXPERIENCE platform, you cannot change the File name.
2. Name is the unique identifier for the 3DEXPERIENCE platform. It is the name of the object in your collaborative space. You cannot change the Name.
3. File Title is the common identifier for Windows and the 3DEXPERIENCE platform. It is a 3DEXPERIENCE platform attribute that appears in the FeatureManager design tree, title bar, and other areas of the user interface. You can change the File Title at any time. Changes to the File Title propagate to CAD Family, Physical Product, 3D Shape, and Drawing object Titles.
4. Component Name is a unique identifier for SOLIDWORKS. It is a 3DEXPERIENCE platform attribute that appears in the MySession app. It matches the File Title that appears in the FeatureManager design tree, including instance numbers when used in assemblies. You change the File Title to change the Component Name.
5. Title, also called Physical Product Title in some contexts, is an identifier for the 3DEXPERIENCE platform. It is a 3DEXPERIENCE platform attribute that appears in the MySession app and dashboard apps like Properties and Bookmark Editor. You can change the Title at any time.

By default, the Title for parts and assemblies with one configuration is the same as the File Title. The Title for parts and assemblies with multiple configurations is a concatenation of the File Title and configuration name, with the configuration name enclosed in parentheses. For drawings, the Title matches either:

• The File Title of the part or assembly that the drawing references.
• Its own specified File Title.

The MySession option highlighted in the following image determines the Title behavior for drawings.

• Overview

• As described in the 

  Data Model and Identifiers in the 3DEXPERIENCE Platform

  ​​​​​​​ section, when you save SOLIDWORKS files to the 3DEXPERIENCE platform, the system automatically creates a hierarchy of objects that represent and link to the SOLIDWORKS files. This out-of-the-box approach is great for people who want to get up and running with the data-management platform as quickly as possible, with no impact to their traditional or legacy workflows. However, the best practice is to update your SOLIDWORKS files for compatibility before you save files to the 3DEXPERIENCE platform.

  NOTE: If you have Collaborative Designer for SOLIDWORKS, this only applies to SOLIDWORKS Desktop 2023 SP4.0 and newer versions.

  The benefits of updating files for compatibility are:

  • Optimal open and save performance.
  • Exposure to 3DEXPERIENCE platform terminology and content types within SOLIDWORKS.
  • Visibility of the SOLIDWORKS data model for the 3DEXPERIENCE platform. 

  How to Update Files for 3DEXPERIENCE Compatibility

  There are two ways to update files for compatibility:

  1. Manual Update

  Create or open a part or assembly file and select the Update for 3DEXPERIENCE compatibility command from the FeatureManager Design Tree context menu.

  

  Activate theUpdate SOLIDWORKS files for compatibility with the 3DEXPERIENCE platformsystem option and create or open a part or assembly file.

  :
  • If you update files for 3DEXPERIENCE compatibility, then make sure to update existing document templates as well, or create new updated document templates.

  • With SOLIDWORKS Connected and SOLIDWORKS Desktop 2024 SP1.0 and newer versions, you can update files for compatibility, in bulk, using the SOLIDWORKS Task Scheduler.

  What Happens to Files That are Updated for 3DEXPERIENCE Compatibility?

  After you update a part or assembly file for compatibility, three things happen:

  1. New configuration view becomes available in the FeatureManager Design Tree

  The CAD Family View uses 3DEXPERIENCE platform terminology and concepts. It displays the CAD Family object, Physical Product configurations, and Representation configurations. With CAD Family View, you can create Physical Product configurations or Representation configurations, convert from one mode to the other, and then back again if you wish.

  

  Like traditional derived configurations, and as the name suggests, Representation configurations represent your Physical Product configurations in a different way, to aid in the design. These include sheet metal flat-pattern configurations, weldment "As Welded" configurations, SpeedPak configurations, and any other use cases where positional or alternate views of the Physical Product configuration are needed.

  The 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.

  1. Custom properties are removed

  If custom properties exist, then they are merged into configuration properties.

  

  

  Working with Existing SOLIDWORKS Files

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

  System-Defined Update Logic

   

  

   

  1. 3DEXPERIENCE SOLIDWORKS / Collaborative Designer for SOLIDWORKS and SOLIDWORKS 2023 SP4.0 and newer versions
  • If there is a configuration named Default, it takes precedence to update as a Physical Product configuration.
  • Configuration Name updates as a Physical Product configuration.
  • Derived configurations with this property update as Physical Product configurations.
  • 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.
  • 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.

  1. 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:

  

  If system-coded update logic does not give you the results that you expected, then you can create user-defined update logic 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 assembly 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.
  
• Choose a configuration mapping. In this example, Multiple physical product.
• In the Configuration Mapping Rule Definition dialog, enter a description for the rule.
• 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

  .

  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

  Recommended Strategies for Working with Part and Assembly Configurations

  for best practices and guidance on when to map configurations to multiple Physical Product configurations and when to map to a single Physical Product configuration with Representation configurations.

  Recommended Strategies for Working with Part and Assembly Configurations

  Before starting any new design project, it is important to choose the right strategy for working with SOLIDWORKS configurations. Failure to plan ahead can result in many unwanted and unnecessary linked Physical Products being created when saving new parts and assemblies. The result of this can lead to an unnecessarily complex experience for both SOLIDWORKS and other 3DEXPERIENCE users, loss of revision and lifecycle flexibility, and at worse degraded SOLIDWORKS opening and saving performance due to the additional items and information being managed in session.

  Taking the right approach will enable you and your design teams to maximize the benefits of working in the 3DEXPERIENCE platform right from the start.

  Understanding the Impact of maintaining Multiple Physical Product Configurations per part and assembly file

  If a clearly defined single Physical Product configuration strategy for parts and assemblies is not put in place, then users can find themselves in the situation where multiple Physical Products are created for each file during the first save. Maintaining multiple Physical Product configurations per file can have several negative impacts on the user experience, and SOLIDWORKS performance.

  Multiple Physical Products representing one SOLIDWORKS part or assembly can make it difficult for users to easily identify which is the actual Physical Product that represents the engineering definition of the part or assembly file.

  Individual revision and lifecycle operations are applied to all the Physical Products related to a single part or assembly at the same time. It is not possible to have related Physical Products at different revisions or maturity states to one another.

  When opening or saving a SOLIDWORKS part or assembly that contains multiple Physical Product configurations, all of the attribute and lifecycle information for every Physical Product configuration is processed. This can negatively impact open and save performance in SOLIDWORKS.

  When a user deletes a Physical Product configuration from a part or assembly, this will cause issues if that configuration is externally referenced in other parts or assemblies. In some case, it may no longer be possible to save the file without either updating all external references, or removing the deleted Physical Product from all related product structures. (The latter can only be done using the Product Structure Editor or Engineering Release apps.)

  1. Prototype and Production Parts and Assemblies
  2. Recommended Strategy

  Parts and assemblies designed and developed in-house, and for production, should only have one SOLIDWORKS configuration update as a Physical Product. This nominated SOLIDWORKS configuration should be configured to contain any key SOLIDWORKS properties related to engineering and manufacture.

  The resulting Physical Product, in the 3DEXPERIENCE platform, will represent a single engineering definition for that part or assembly including the maturity state, Enterprise Item Number, plus any Physical Product specific attributes.

  

  To manage the two different configuration types, enable the following SOLIDWORKS option for all users:Update SOLIDWORKS files for compatibility with the 3DEXPERIENCE platform.

  EXPERIENCE users within an organization.

  If your company uses SOLIDWORKS 2024, use the Remove CAD Family option so that only one Physical Product configuration can exist per file. With this option set, additional SOLIDWORKS configurations will be automatically created as Representation configurations.

  : It is recommended that SOLIDWORKS part and assembly templates are updated with the CAD Family removed to make this the default behavior for every new part and assembly file.

  For companies using SOLIDWORKS 2023 or earlier, users must manually choose which SOLIDWORKS configuration to nominate as the Physical Product configuration. It is not possible for the platform administrator to configure their 3DEXPERIENCE platform to make this the default behavior. Therefore, it is important that users are well trained and have a complete understanding of the recommended strategies from this section of the guide.

  1. Saving Pre-existing SOLIDWORKS Designs to the 3DEXPERIENCE Platform
  EXPERIENCE platform, it is important to understand how configurations have been used in their parts and assemblies before any files are saved. Due to the versatility of configurations, it is common practice for design teams to treat configurations as individual part numbers. In that scenario, take time to carefully analyze the files and factored in to any migration project. (See the Working with Existing SOLIDWORKS Files page for details.)

  If you decide to maintain any part or assembly configurations as individually life-cycled engineering items, then those configurations must be split or saved into individual part and assembly files, with each file containing only one Physical Product configuration.

  NOTE: Saving configurations to individual files is a manual process that can be automated using a SOLIDWORKS macro.

  1. Summary

  Adopting the recommended SOLIDWORKS configuration strategy for prototype and production items will ensure that only one clearly defined Physical Product exists for each part and assembly in the 3DEXPERIENCE platform. This approach will enable you and your design teams to maximize the benefits of working in the 3DEXPERIENCE platform from the start.

  1. Standard Library and Purchased Parts and Assemblies
  2. Recommended Strategy

  Externally purchased parts and assemblies are typically managed in a library and are not modified or revised by the engineers who utilize them in their designs. When deciding which SOLIDWORKS configuration strategy to adopt for purchased parts, consider the following:

  • Part files with configurations that represent different size variations
    • If there are 20 or less configurations per part file, Physical Product configurations can be used without negatively affecting performance.
    • If there are more than 20 configurations per part file, the one Physical Product configuration per file strategy should be used to maximize performance. Each configuration needs to be saved to an individual part file.
      • In this scenario, Representation configurations must not be used to represent different size variations. Representation configurations are not saved to the 3DEXPERIENCE platform. Therefore, the size variation of the part will not be displayed in any of the 3DEXPERIENCE platform viewer apps.
  • Assembly files with configurations
    • For all assembly files, the one Physical Product configuration per file strategy should be to maximize performance. Each configuration needs to be saved to an individual assembly file.
  1. Summary

  When deciding on which configuration strategy to deploy for SOLIDWORKS library parts, using one strategy and avoiding a mix of single and multiple Physical Product configuration library parts will help you maintain a consistent user experience.

  Common Use Cases for SOLIDWORKS Configurations and Best Practices When Using the 3DEXPERIENCE Platform

  This section of the guide discusses common use cases for SOLIDWORKS part and assembly configurations and provides recommended best practices for each.

  Part Configuration Use Cases

  Part Configuration Use Cases
  Managing Cast and Machined versions of a part
  Sheet Metal - Flat and Folded States
  Weldments - As Machined and As Welded states
  Working with Toolbox
  Part Geometry Simplification

  1. Managing Cast and Machined Variations

  SOLIDWORKS configurations provide a simple and efficient method of capturing the cast and machined variations of a part.

  EXPERIENCE platform, the required strategy will depend on the lifecycle requirements of each variation.

  If the requirement is to treat both as one part number, then it's recommended that both the cast and machined variations are created as configurations in the same part file. This part file should contain only one Physical Product configuration. Any other variations of the part that are required to represent different machined states should be created as Representation configurations. During the first save to the 3DEXPERIENCE platform, the Physical Product configuration will generate the Physical Product that is used to represent the overall design including its lifecycle information. For example, maturity state, revision, and key attributes. Typically, the finished machined version of the part is nominated to be the Physical Product configuration.

  EXPERIENCE platform and represented by their own individual Physical Products which are revision controlled, independently. For information on how to work with derived parts in SOLIDWORKS, refer to the Derived Part section of the online help.
  1. Sheet Metal - Flat and Folded States

  When designing Sheet Metal parts in SOLIDWORKS, configurations are used to represent the folded and flattened states. The flattened state configuration represents the manufacturing definition of the finished part. For most companies both configurations will represent the same part and part number, therefore the one Physical Product configuration per file strategy should be applied. It is recommended that the folded configuration of part is defined as the Physical Product configuration, and the flattened configuration is defined as a Representation configuration.

  EXPERIENCE platform viewer apps. The flattened configuration is only used in SOLIDWORKS, by the designer, to create the necessary outputs for manufacture. For example, drawings and DXF files.

  In the scenario where multiple variations of the same sheet metal part need to be revision managed independently, with unique lifecycles, individual flat patterns, and part numbers, separate part files should be used to represent each variation. Each individual part file should contain one Physical Product configuration to represent the fully detailed part and a Representation configuration that represents the flattened state.

  1. Weldments - Welded and Machined States

  NOTE: Before using SOLIDWORKS weldments functionality with the 3DEXPERIENCE platform, it's recommended that users are familiar with the Weldments training course material.

  A weldment is an object made up of several parts welded together. In SOLIDWORKS, a weldment refers to a special type of part model containing multiple bodies which can be described with a cut list. Often times these bodies are welded together in production, such as structural members welded together to form a frame.

  

  Although primarily targeted for working with structural steel and aluminum, SOLIDWORKS weldments are also commonly used for modelling wood working projects and plastic extrusions.

  The default behavior when adding a weldment feature to a part model includes the creation of a derived configuration and configuration as follows

  The description is added to the active configuration.

  A derived configuration with the same name is added with the description .

  Additionally, any new top-level configurations created will automatically have a corresponding derived configuration.

  These configurations provide a means for representing the weldment as it will initially be welded and as it will be following post assembly machining operations.

  In the Weldments page of Document Properties, settings can be adjusted to modify how these configurations are created.

   setting activated, any subsequent top-level configurations will automatically have a corresponding "As Welded" derived configuration. Deactivating this setting will prevent the creation of additional configurations in the part.

  To set up your own standard for how weldment configurations are created, consider modifying these settings and save them to a part template.

  1. Recommendations for Using Weldment Configurations in Combination with the 3DEXPERIENCE Platform

  The default part template settings are configured so that configurations are automatically created to represent the model in an “As Welded” state and an “As Machined” state. Having a representation of both is the most common user requirement as these configurations provide an easy way to communication information about a weldment model in the different stages of the manufacturing process.

  When adding a weldment feature to a part, the configuration will automatically be created as a Physical Product configuration, and the configuration will be created as a Representation configuration.

  EXPERIENCE platform by the "As Machined" configuration only. The "As Welded" configuration will only be visible in SOLIDWORKS. This default behavior will meet the needs of the majority of users. If working this way, it’s recommended to remove the CAD Family from the part (if using SOLIDWORKS 2024), so that only one Physical Product configuration ever exists per weldment part file. That setting can be saved with your weldment part template. For more information on removing the CAD Family, refer to the Recommended Strategies for Working With Part and Assembly Configurations section of this guide.

  In the scenario where there is a business requirement to manage both the "As Welded" and "As Machined" configurations as independent items, with unique attributes and Enterprise Item Numbers, then both configurations must be created as Physical Product configurations. In this scenario, the "As Welded" configuration needs to be converted from a Representation configuration to a Physical Product configuration.

  EXPERIENCE platform by unique Physical Products.
  1. Working with Toolbox

  The SOLIDWORKS Toolbox Library offers three different user settings for the creation of component sizes:

  1. Create Configurations
  2. Create Parts
  3. Create Parts on Ctrl-Drag

  The Toolbox integration with the 3DEXPERIENCE platform only supports the Create Parts setting. This setting creates individual part files for each size. The Toolbox integration does not support managing Toolbox sizes as SOLIDWORKS configurations.

  1. Collaborative Designer for SOLIDWORKS

  To enforce the correct behavior, the system automatically activates the Create Parts setting when you install the Design with SOLIDWORKS app and activate the 3DEXPERIENCE add-in.

  EXPERIENCE add-in or change the Files setting in Toolbox Settings.
  1. 3DEXPERIENCE SOLIDWORKS

  Unlike SOLIDWORKS Desktop with Collaborative Designer for SOLIDWORKS, the SOLIDWORKS Connected app does not include the Files setting in Toolbox Settings. This is by design. The Create Parts setting is force-activated and cannot be changed.

  For detailed information related to working with Toolbox and the 3DEXPERIENCE platform, refer to the “Working with Toolbox” SolidPractice guide.

  1. Part Geometry Simplification

  There are many scenarios in which a fully featured part model is not required and may even have a negative impact on performance. For examples, large assembly designs and SOLIDWORKS Simulation studies. In these scenarios, configurations are the recommended method of controlling the level of detail in a part model. Configurations representing a de-featured version of a part are typically used to aid design in SOLIDWORKS and will not be related in any way to the final manufactured version.

  EXPERIENCE platform as one Physical Product that contains all of the information related to the design and its lifecycle (attributes, Enterprise Item Number, revision, maturity state). Maintaining one Physical Product configuration per part file reduces unnecessary complexity, as opposed to having multiple Physical Products represent one part.

  Another benefit of adopting this methodology are scenarios where parts are simplified to aid in large assembly design and visualization in SOLIDWORKS. SOLIDWORKS users get optimized performance when using simplified representations, and anyone viewing a complete assembly outside of SOLIDWORKS, in a 3DEXPERIENCE platform viewer app, will see the fully detailed models.

  Assembly Configuration Use Cases

  Assembly Configuration Use Cases
  Mirrored Components and Split Parts
  Alternate Component Positions
  Simplified Assemblies
  SpeedPak Configurations
  Display States

  1. 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.
   

  1. 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.

  

   

  

  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.

  
  1. 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.

  
  1. 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.

   

  
  1. 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.
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