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! 

• Preface 
• Cut List Fundamentals in SOLIDWORKS Design
• Engineering Items on the 3DEXPERIENCE Platform
• Saving Weldment parts to the 3DEXPERIENCE Platform
• Publishing a Cut List
• Enriching Cut List Items

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, VARs, and customers who are on an 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 version SOLIDWORKS 2025 SP04. If you have questions or need assistance in understanding the content, please contact your designated reseller.

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1. Prerequisite Learning

Before reading this guide, you must be familiar with the following:

• Creating and editing Weldment models in SOLIDWORKS Design
• Storing SOLIDWORKS designs in a collaborative space on the 3DEXPERIENCE platform
• Saving to and Opening SOLIDWORKS Designs from the 3DEXPERIENCE Platform

2. Preface

Weldment design in SOLIDWORKS is about more than creating geometry. It is about ensuring that structural members, cuts, and raw material details flow seamlessly into manufacturing. By managing weldment structures and their cut lists on the 3DEXPERIENCE platform, designers gain a direct link from design intent to production execution.
 

Working with Multiple Bodies in a Part

In the SOLIDWORKS Design part environment, it is possible to model several solid bodies within a single file. This approach is commonly used for weldments, where structural members, plates, or tubes are created directly as bodies. It removes the need to manage mates as in a traditional assembly, and it simplifies updates since all related members exist in one file.

This method is especially effective when:

• Structural members are cut from raw stock such as beams, tubes, or plates.
• A design contains complex geometry that must be divided into multiple pieces.
• Frequent modifications are expected, since changes can be managed without external references.

The result is faster iteration, a more compact file structure, and clearer design intent compared with building full assemblies from individual parts.
 

From Design to Manufacturing with Cut Lists

Once the geometry is complete, it must be prepared for production. The Cut List feature in SOLIDWORKS Design organizes bodies within a weldment part. It identifies groups of identical members, applies properties such as material and length, and creates a cut list table for communication with downstream teams.

Key aspects include:

• Grouping bodies with the same dimensions and properties.
• Capturing manufacturing data such as description, finish, and cut length.

• Providing output through the cut list table, which functions as the bill of materials for multibody weldment parts

   

3. Cut List Fundamentals in SOLIDWORKS Design

The Cut List in SOLIDWORKS Design provides the link between a weldment design and the manufacturing process. Its functional intent is to act as the bill of materials for multibody weldment parts. Instead of manually collecting data for each body, the cut list automatically organizes and communicates what is required for production.
 

Purpose of a Cut List

The cut list groups similar bodies created in a part file and enables metadata to be attached for downstream use. Identical items, such as structural members of the same length and profile, are combined into one entry. This provides:

• Clear communication of manufacturing needs
• Reduction of duplication by grouping topologically similar bodies
• A place to apply additional properties like material, description, and finish
   

Types of Cut List Members

Within a cut list, SOLIDWORKS Design recognizes three main types of members:

• Structural Members : Bodies created using Structure System commands. These represent standard profiles such as tubes, beams, or channels cut to length and welded together.
• Sheet Metal Members : Bodies created using Sheet Metal commands. These are flat or bent plates used in welded designs, with automatic attributes such as bounding box dimensions, thickness, and bend information.
• Generic Members : Bodies created with general modelling features such as Extrude, Revolve, or Insert Part. These do not generate specialized attributes automatically and often require manual property definition.

Cut List Properties

Each type of cut list member carries its own properties. For example, structural members include length, angle details, and cut length, while sheet metal members include bounding box dimensions, thickness, and bend parameters. Generic members usually only carry basic attributes such as material and quantity, with additional details added manually if required.
 

These properties appear on cut list items under the Cut List Folder in the FeatureManager design tree. Within each folder, all bodies that share identical geometry and orientation are grouped, ensuring accurate reporting for manufacturing. The Cut List Folder is automatically created when the Weldment feature is enabled or when bodies are generated using Structure System or Sheet Metal commands.

4. Engineering Items on the Platform

In the 3DEXPERIENCE platform, design data from SOLIDWORKS is translated into objects that follow the platform’s data model. At the core of this model is the concept of the Engineering Item.

Engineering Item

An Engineering Item represents the designed specification of a product. It captures the engineer’s design intent rather than the physical object itself. This definition provides a digital reference that can be connected to processes and consumed by downstream teams.
 

Physical Product 

A Physical Product is a subtype of Engineering Item that represents the tangible, real-world counterpart of the design. It can exist as a single part or as an assembly, and may also include associated objects related to parts and assemblies.

Physical Products have several default behaviors:

• They can reference other Physical Products as child items
• They carry properties that define their role in the product structure
• They can be managed through maturity states and lifecycles on the platform
   

Part Physical Product  

Within the Physical Product category, the Part Physical Product subtype is most closely aligned with SOLIDWORKS Design data. By default, a SOLIDWORKS part saved to the platform is represented as a Part Physical Product.

• A Part Physical Product defines a single part with no child references
• It is suited to simple, single-body designs
• Multibody parts may also be saved as a Part Physical Product if specific conditions are not satisfied
   

Relevance for Weldments and Cut Lists

The way a SOLIDWORKS Design file maps into the platform has a direct impact on how weldment structures and their cut lists are represented. If a file is stored as a Part Physical Product, it remains a standalone item. If it is stored as a Physical Product Assembly, the structure within the weldment can be represented as child items.

5. Saving Weldment Parts to the 3DEXPERIENCE Platform

When a SOLIDWORKS Design part file is saved to the 3DEXPERIENCE platform, it is normally represented as a single Part Physical Product. This default behavior works for simple parts but does not properly reflect the structure of weldments. Weldments contain multiple members that behave like child items, so the correct representation on the platform is a Weldment Structure.

Default Mapping vs Weldment Structure

• Default behavior: A SOLIDWORKS Design part saved without weldment intent becomes a Part Physical Product on the platform. It is treated as a single object with no children.

• Weldment behavior: A part that contains a weldment feature and meets specific criteria is treated as a Physical Product Assembly. This allows the platform to manage it with a product structure that can later expose cut list members as child items.

  

   

This distinction ensures that although the model is authored in the SOLIDWORKS Design part environment, its lifecycle and structure are managed correctly as an assembly on the platform.
 

Prerequisites for a Weldment Assembly

For a multibody SOLIDWORKS part to be saved as a Weldment Structure on the platform, the following conditions must all be satisfied at the first save:

1. The part contains a Weldment feature

2. The file is saved using the New Configuration Manager

3. The file is identified as a Single Physical Product (one part number)

Only when these conditions are met does the part map to the correct Weldment Structure data model.
 

Recovery if Conditions Are Not Met

Not every multibody design is intended to be an assembly, and in many cases, a multibody part will save as a Part Physical Product. Once a part is saved as a Part Physical Product, it cannot be directly converted into an assembly on the platform. Two common recovery scenarios exist:

1. The file was saved without a Weldment feature

   1. With the file opened in a SOLIDWORKS session, go to Insert > Weldment > Weldment to add the weldment feature.

      

       

   2. From the top menu, select File > Save As New. This creates a new platform object that is recognized as a Weldment Structure instead of reusing the old Part Physical Product definition
       

2. The file was saved without a Single Physical Product definition.

   1. With the file opened in a SOLIDWORKS session, go to the Configuration Manager tab. 

      

       

   2. Right-click on the CAD Family and select Remove CAD Family
   3. From the top menu, select File > Save As New. This creates a new 3DEXPERIENCE platform object that is recognized as a Weldment Structure instead of reusing the old Part Physical Product definition

A weldment part must behave as a Single Physical Product at the moment of its first save to the 3DEXPERIENCE platform.
If the SOLIDWORKS system option was previously set to: Allow multiple physical products in new parts and assemblies.

Once the file is saved in this incorrect data model, changing the setting later does not update the already-saved platform object, which is why recovery is required.

How to ensure all future Weldment parts are saved with the correct data model

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. 
 

These recovery paths ensure that weldment data is stored with the correct structure and can later support the publishing of cut list items.

Recommended Practice: Create weldment templates that already include the Weldment feature, the single physical product definition, and a predefined Cut List ID setup. This ensures that from the very first save, the file aligns with the correct data model on the platform, reducing errors and avoiding the need for recovery steps later.

6. Publishing a Cut List 

Publishing the cut list exposes each cut list member as a child Engineering Item on the platform. Without publishing, the weldment appears as a single line item. With publishing, the platform shows the weldment as a product structure with child items that correspond to the cut list members.
 

Prerequisites

• The part must be saved so it maps as a weldment assembly on the platform
• Generate Cut List IDs must be enabled and calculated in SOLIDWORKS Design

Cut List IDs ensure that each body can be uniquely identified. They are automatically built from body geometry and metadata once the option is enabled.
 

Cut List ID Configuration

Cut List IDs are defined in Tools > Options > Document Properties > Weldments. By standard configuration, SOLIDWORKS Design uses the following properties when generating IDs:

• Structural Members: Description, Material, Length, Angle1, Angle2, Angle Direction, Angle Rotation
• Sheet Metal Members: Description, Material, Bounding Box Length, Bounding Box Width, Sheet Metal Thickness, Bounding Box Area, Bend Count, Bend Radius
• Generic Members: Description and Material

For structural and sheet metal members, these properties are usually sufficient to ensure uniqueness. For generic members, however, the minimal set of description and material often does not guarantee traceability. In such cases, an additional property such as a part number can be added to the ID definition so that repeated use of the same body type is always recognized correctly.

Recommended Practice: 
Establish a company-wide standard for Cut List ID definitions. Consistent rules prevent conflicts when sharing or reusing cut list items across projects.

Publish cut lists only once the design has reached a stable stage. Publishing too early can lead to redundant updates and confusion if production teams begin planning from items that are later changed.

Publishing the Cut List

Publishing can be performed directly at the time of first save of the geometry, or it can be published even after it has been saved to the 3DEXPERIENCE platform:

1. Open the weldment part in SOLIDWORKS Design.
2. Ensure that "Generate Cut List IDs" is enabled from the options menu.
3. Select File > Save to 3DEXPERIENCE
4. It might prompt you to lock your component if you had already saved the file to the 3DEXPERIENCE platform before.

5. In the Save dialogue, check the option Publish Cut List.

    

6. Complete the save

This creates the parent weldment item and child items for each cut list member in the product structure. Identical members share the same Cut List ID, so they are grouped consistently in BOM contexts while still being visible as individual instances in the structure.

3DEXPERIENCE Platform Representation

In SOLIDWORKS Design, cut lists group identical bodies in folders. The number of displayed items, therefore, reflects the number of groups, not the total number of bodies. On the platform, everybody is represented as an instance within the product structure. Bodies with the same Cut List ID are grouped for BOM accuracy but still shown individually as instances, ensuring both reuse and visibility.

7. Enriching Cut List Items

Once a cut list is published to the platform, each member is treated as an Engineering Item. This makes them accessible outside the SOLIDWORKS environment for collaboration, downstream use, and additional data management.
 

Limitations of Traditional Methods

In traditional workflows, cut lists remain confined to drawings or exported spreadsheets. Manufacturing teams rely on these static files, and every design change requires manual export and re-import. This breaks the digital thread and prevents the reuse of information. Metadata such as NC programs, DXF files, or raw material specifications must be maintained by the design engineer within the SOLIDWORKS file, creating bottlenecks.
 

Value of Publishing to the Platform

On the platform, published cut list items are recognized as Engineering Items. Each structural, sheet metal, or generic member becomes a managed object within the product structure. This enables:

• Assigning Enterprise Item Numbers (EINs) for traceability across design, procurement, and production

• Adding attachments such as DXF files, NC programs, or specifications directly to cut list items 

   

• Mapping custom properties relevant to a specific industry or company standard

• Collaborating through comments, classifications, and lifecycle controls without needing to open the SOLIDWORKS file

   

This separation allows responsibilities to be distributed. Production teams can add information to cut list items without depending on design engineers to embed everything in CAD.

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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.