Managing Cast and Machined Variations
SOLIDWORKS configurations provide a simple and efficient method of capturing the cast and machined variations of a part.
When working with the 3DEXPERIENCE 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.
In a scenario where the requirement is to treat cast and machined versions of a design as separate part numbers and have them revision controlled independently from one another, a derived part modeling methodology should be used. Using the derived part methodology, the part file for the cast version is represented by its own Physical Product, and any machined variations of the design are created by inserting the cast part file into them as the first feature. Each of the “machined” part files are then saved to the 3DEXPERIENCE 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.
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.
Taking this approach, the fully detailed folded version will always be shown when viewing the part using any of the 3DEXPERIENCE 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.
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.
Even though a weldment model could technically be described as an assembly, working within a multibody part allows for easy manipulation of multiple pieces and minimizes complex file relationships. Specialized weldment commands also automate common functions of working with structural members and frames.
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.
With the Create derived configurations 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.
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
Therefore, the part will be represented in the 3DEXPERIENCE 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.
Both the "As Welded" and "As Machined" configurations will now be represented in the 3DEXPERIENCE platform by unique Physical Products.
Working with Toolbox
The SOLIDWORKS Toolbox Library offers three different user settings for the creation of component sizes:
- Create Configurations
- Create Parts
- 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.
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.
To avoid any unexpected complications, it's recommended to not disable the 3DEXPERIENCE add-in or change the Files setting in Toolbox Settings.
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 SolidPractices guide.
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.
It is recommended that any configurations created to represent de-featured or simplified variations of a part are created as Representation configurations, and that the configuration representing the fully-detailed model is nominated to be the Physical Product configuration.
The part file will be represented in the 3DEXPERIENCE 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.
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