Best Practice Information
Domain and Role/Product
SOLIDWORKS Design Collaborative Designer for SOLIDWORKS SOLIDWORKS Design with Cloud Services
What's Covered? - Jump to each section using the Contents List in the top right!
- Prerequisite Learning
- Introduction to choosing the right approach for managing material finishes
- Defining the material finish of a component as a function of design, or of manufacturing.
- Use Case Example - Defining a Material Finish in SOLIDWORKS Design as a function of Design/Engineering
Revision History
| Rev # | Date | Description |
|---|---|---|
| 1.0 | Oct 2025 | Document created. |
Note
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Your Feedback Requested
We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.1. Prerequisite Learning
Before reading this guide, it is important that you are familiar with the following:
- Creating and utilizing SOLIDWORKS configurations in a design workflow
- The different item types created when saving SOLIDWORKS files to the 3DEXPERIENCE platform, and how they relate to SOLIDWORKS configurations.
For an in-depth explanation, please refer to the "Using SOLIDWORKS Configurations with the 3DEXPERIENCE Platform" SolidPractices guide.
2. Introduction – The Importance of Choosing the right approach for managing material finishes
SOLIDWORKS configurations are a common technique employed by designers and engineers to represent different material finishes that can be applied to a component during the final stages of manufacture.
SOLIDWORKS configurations provide a number of distinct benefits. Each one can have its own unique property information, including a part number that can be consumed in downstream manufacturing, geometry changes can be easily propagated to specific or all configurations, and all of the information is encapsulated in one part file. However, when adopting the 3DEXPERIENCE platform for managing your design to manufacturing process, modelling techniques that worked well with Windows file management are not necessarily the best techniques that will enable your business to take full advantage of the breadth of the 3DEXPERIENCE platform capabilities.
This guide will explain how to transition from using a configuration-based approach for capturing material finish information related to a design to choosing the right approach that will meet the needs of not just your design team, but also consider the needs of other departments within your company.
Defining the material finish of a component as a function of design, or of manufacturing
Where the material finish information related to a component is captured will vary from company to company. In small to medium-sized companies, it's common for it to be associated with the SOLIDWORKS model as a configuration that falls under the responsibility of the design or engineering teams.
In large manufacturing organizations, the material finish is often defined by the manufacturing department, especially where the finish is purely aesthetic and will not impact the performance of the product. The engineering team may have no involvement, and the choice of finishes may be governed by a marketing department working directly with manufacturing. In this scenario, the material finish information will appear in a manufacturing bill of materials but will not be defined on the related SOLIDWORKS model or drawing.
Adopting the 3DEXPERIENCE platform for managing design data, like any new business process change, offers an opportunity to enhance current working practices that take advantage of new capabilities.
The following use cases describe the recommended methodologies for defining multiple material finishes related to a single component.
3. Use Case – Defining Material Finish in SOLIDWORKS Design as a function of Design/Engineering
In situations where an accurate representation of material finish is required as a function of the design, it's common practice for designers and engineers to capture each finish as a SOLIDWORKS configuration.
However, creating multiple configurations and having each one represented by a Physical Product can lead to an unnecessarily complex experience for both SOLIDWORKS Design and other 3DEXPERIENCE users. The limitations include loss of revision and lifecycle flexibility, and at worst, degraded SOLIDWORKS opening and saving performance due to the additional items and information being managed in session.
When adopting the 3DEXPERIENCE platform, a different modelling approach is required. Instead of defining each material finish as a SOLIDWORKS configuration, a derived part should be used to represent each finish. A derived part can have its own unique item number and attribute information while maintaining a reference back to the main design. Each derived part will be represented in the 3DEXPERIENCE platform by a single Physical Product. Any geometry changes made to the main design will be propagated to the derived parts. Adopting a derived part modelling approach will maintain many of the advantages of using configurations, but importantly, provide greater flexibility for managing the overall design lifecycle in the 3DEXPERIENCE platform.
The following example describes the recommended modelling approach for defining a range of different colour finishes for a SOLIDWORKS part design. A simple aluminium alloy component is available in a range of coloured anodized finishes.
In this scenario, each colour variation of the component will require its own unique item number. Any geometry changes will be propagated to each of the different material finish variations of the design.
a) SOLIDWORKS System Options
Set the SOLIDWORKS 3DEXPERIENCE Integration option to Allow a single physical product in new parts and assemblies. This setting will ensure that each SOLIDWORKS file will be represented by only one physical product in the 3DEXPERIENCE platform.
Note: Having 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.b) Initial Component Design
A new Inlet Body component is designed and saved to the 3DEXPERIENCE platform.
A single Physical Product that represents the engineering definition is automatically created.
c) Creating a Material Finish Part
To create the first material finish variation of the component, a new part file is created.
Tip: By utilising the Create new on the 3DEXPERIENCE platform templates, a user can enter important attribute information at the time of a part or assembly creation. This can save time and effort later.
For the first save, a descriptive Title “Inlet Body – Blue Anodized” is used. This can be easily replaced later by an Item Number.
Next, the original Inlet Body part model is inserted into this new part using the Insert->Part command from the Insert pull-down menu in SOLIDWORKS Design. The Inlet Body part is now the first model feature in the Blue Anodized part.
The Inlet Body and the Blue Anodized parts are now linked by an external reference. Any geometry modifications to the Inlet Body part will be automatically propagated to the Blue Anodized part.
A new blue colour appearance is applied, and the part is saved to the 3DEXPERIENCE platform.
The SOLIDWORKS MySession task pane shows the Inlet Body referencing the Blue Anodized part.
d) Adding a Make From Relation
A user can create a specific 3DEXPERIENCE Platform relationship type that can be used to define that one part is made from another stock part. Adding a Make From relation highlights to other stakeholders in a company that one part is made specifically from another. In this example, the Inlet Body will be added to the “Make From” tab of the Blue Anodized part.
A Make from relationship can be defined in one of two ways: using the Engineering Release app (non-CAD users) or from the Information panel in SOLIDWORKS MySession. The Make From relation is defined in SOLIDWORKS by first selecting the component in the MySession Task Pane, followed by opening the MySession side panel and navigating to the Make From tab.
To add the relation, click on the add make from icon and search for the stock component, which in this case is the Inlet Body part. The Inlet Body part is now displayed on the Make Tab.
Opening the Inlet Body - Blue Anodized part in the 3DEXPERIENCE relations browser will now show that a Make From relationship type exists between it and the Inlet Body stock part.
Any additional material finishes of the Inlet Body can be defined by repeating the same steps of creating a new SOLIDWORKS part and inserting the stock Inlet Body part.
Viewing the relations of the Inlet Body part will group all of the referenced material finish parts under a Used to Make relationship type.
Note: When deleting a physical product with a Made From or Used to Make Relation, selecting the Include Structural Objects option will delete all of the related components. It is recommended that this option be left unchecked if you are unsure exactly what objects will be included in the delete.
e) Assigning an Item Number to a Material Finish Part
Each material finish part will typically need to be assigned its own unique part number. An Enterprise Item Number (EIN) is the primary Part/Item numbering solution in the 3DEXPERIENCE platform. The EIN offers a broad scope for configuration. For example, an EIN can be configured to contain attributes that include different counters linked to individual values.
To learn more about configuring and using Enterprise Item Numbers, please refer to the Attribute Driven Naming section of the Naming Strategies for SOLIDWORKS SolidPractices guide.
The EIN for each material finish part can be assigned either in SOLIDWORKS via the MySession Tools toolbar or by using the Engineering Release app (requires the Product Release Engineer Role) in a web dashboard.
To ensure that the EIN is highly visible to all users in both SOLIDWORKS and the web dashboard, the EIN can be configured to automatically populate the Title field of the physical product.
a. Set the option EIN Administration option Copy EIN to Title
b. In the SOLIDWORKS system options, configure the feature manager to display the EIN as the primary identifier
f) Copying An Existing Material Finish Part
Since the inlet body part in this use case can be supplied in multiple finishes, each one can be created directly from the blue anodized part.
There is no need to repeat the steps of creating each one as a new derived part. Instead, make a copy of the material finish part by using either the Save As New command in SOLIDWORKS MySession or the Duplicate command from the Bookmarks Editor web widget. There is no right or wrong here, but before deciding, it’s important to understand the impact of using either one.
Save As New – The resulting part and physical product does not contain the Make From part reference, in this example, the Inlet Body component. The Make From relation will need to be added to each new part using the MySession task pane.
Duplicate – The duplicate command is executed from the Bookmarks Editor widget. Both a CAD Family and a Physical product will be created. The CAD family object can be removed from the Bookmark. The duplicated Physical Product will include the Make From Physical Product.
g) Viewing the Related Make From Components in 3DEXPERIENCE Web Widgets
Bookmarks Editor
Make From relations can be viewed in the 3DEXPERIENCE Bookmarks Editor widget via the relations tab on the ENOVIA properties panel. In this example, the Blue Anodized physical product shows a "Make From" relation to the Inlet Body physical product.
The relations tab for the Inlet Body physical product shows a "Used to Make" relation listing all of the components that have been associated with it via the Make From tab.
Product Explorer
The related child components of the Inlet Body can be viewed in Product Explorer by RBM on the Title column and selecting "Show Relations."
4. Use Case - Managing Material Finish Variations of an Assembly
The 3DXPERIENCE platform methodology called branching is used to create physical products that represent different material finish variations of an assembly. Branching is similar to duplicating in 3DEXPERIENCE. Branching is the intended method for creating and managing design alternatives, whereas duplication is the intended method for managing the evolution of a product.
The following example will describe the recommended approach for creating a new material finish variation of an assembly using a branching methodology. The Branch command allows a user to make a new copy of the Nozzle assembly while maintaining a link back to the original assembly.
In the previous use case, multiple material finish variations of an anodized Inlet body part were created from the stock inlet body part. The same principle can be applied to an assembly scenario, too. In this example, the Inlet Body part is a key component in a Water Jet Nozzle assembly. The water jet nozzle assembly can be supplied with any of the colour variations available for the inlet body. Each colour variation of the assembly can have its own Enterprise Item Number.
Creating a new branch assembly
Prior to creating any material finish variations, a stock version of the water jet nozzle assembly has been created.
This stock assembly represents the functional design regardless of colour finish information. Any new colour variations will be branched from this assembly.
To create a new branch, first, the stock Water Jet Nozzle assembly is opened in SOLIDWORKS Design from the 3DEXPERIENCE platform. The Branch command is then selected from the Lifecycle toolbar on the MySession Task Pane.
In the New Branch dialogue, an action can be specified for each node in the product structure. In this example, the stock Inlet Body part will be replaced with the Green Anodized material finish version. The action for the top-level assembly is set to Branch, and a new Title is added. The action type for all of the remaining items is set to Reuse. Since there is no option in the Branch command to replace items, the replacement of the Inlet Body with a chosen colour variation will be done using the SOLIDWORKS Replace in Assembly command afterwards.
When the Branch button at the bottom of the dialogue is selected, a new physical Product is created. The existing stock Water jet Nozzle assembly remains open in SOLIDWORKS Design, and the new branch assembly has been created in the database, but has not been automatically opened.
Next, the new branch assembly is opened in SOLIDWORKS Design. It is still referencing the stock Inlet Body part. The SOLIDWORKS Replace Component command is used to replace the stock inlet body with the green anodized material finish version.
The assembly is saved back to the 3DEXPERIENCE platform to apply the changes.
The Revisions command from the Lifecycle toolbar in MySession will display graphically which assembly the Green material variation of the Nozzle assembly has been branched from, plus any other branched variations.
5. Summary
The use cases outlined in this guide explain how to transition from using a configuration-based approach for capturing material finish information related to a design. The use cases are intended for design teams who have a need to capture the information as part of the design in SOLIDWORKS.
Adopting the 3DEXPERIENCE platform for managing design data, like any new business process change, offers an opportunity to enhance current working practices that take advantage of new capabilities. Therefore, before deciding on whether to use this approach or continue using SOLIDWORKS configurations, it is important to consider whether or not there is value in capturing the material information during the SOLIDWORKS modelling process. Instead, consider whether the information could be defined further downstream as a part of the manufacturing bill of materials.
Your Feedback Requested
We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.