The following use case describes the recommended workflow for taking a component created in one of the xApps, and adding features to it in SOLIDWORKS. This example will be based around a motorcycle fuel tank concept design created in xShape. After the fuel tank concept has been completed in xShape it is opened in SOLIDWORKS where features are added to create the detail engineering design.

1.Create the new fuel tank design in xShape

A new motorcycle fuel tank design concept is created using the browser-based design app xShape and saved to a collaborative space. 

Important Note: As explained in the previous two use cases, when saving a component in xShape (or another cloud design app), immediately after the save operation has completed an exact geometry representation is generated asynchronously in the background on the cloud server. The generation of exact geometry in most cases is instantaneous, but for components with complex geometry it can take a few minutes or more. If the native 3DEXPERIENCE component is opened in SOLIDWORKS before the exact geometry has been generated it will be represented by a faceted graphics body in place of the ExactGeometry.

2. The fuel tank design concept is opened in SOLIDWORKS as a native 3DEXPERIENCE component

The Open command in SOLIDWORKS is designed to only work with parts and assemblies authored in SOLIDWORKS. Therefore, any Physical Products created using an xApp will not appear when searching or browsing Bookmarks in the Open command.

Instead, components authored in an xApp are opened in one of two ways. Drag and drop from the xShape window into SOLIDWORKS. 

 Or drag and drop from 3DSearch or Bookmark Editor in the MySession tab in SOLIDWORKS.

During the open process a CATPart file representing the xShape component is automatically downloaded the local working folder and converted to a SOLIDWORKS part file. The resulting part file is automatically oriented with Z-up to match the orientation in xShape. 

It is important to understand that the part file generated during the open operation is intended only as a temporary file. If the part is closed and then deleted from the PC via the 3DEXPERIENCE Files on this PC tab, the next time it is opened another brand-new part file will be created to represent it. If any SOLIDWORKS features are added to the part, when a user attempts to save the part back to the 3DEXPERIENCE platform the save will be blocked with the status “Incompatible geometry detected”. 

In this case the blocking of the save avoids a user getting into a situation where the SOLIDWORKS features will be lost following the deletion of the local file. The recommended workflow for adding SOLIDWORKS features is to first create a derived part from the native 3DEXPERIENCE component. 

3. Creating a Derived Part from the native 3DEXPERIENCE Fuel Tank component

In step 1, xShape was used to create the overall shape of the fuel tank. Next, SOLIDWORKS will be used to continue with the detail design, adding the necessary geometry required to turn the initial concept into a manufacturable component. To ensure that any SOLIDWORKS features can be saved back to the 3DEXPERIENCE platform, first a derived part must be created from the native 3DEXPERIENCE fuel tank component. Any SOLIDWORKS features are then created in the derived part file, and not in the temporary part file of the native 3DEXPERIENCE component.

There are a few ways that the derived part can be created. If the native 3DEXPERIENCE component is open in the SOLIDWORKS session an alternative method would be to create a new part, and then use the insert part command to insert the xShape fuel tank as a derived part, achieving a similar result.

It’s recommended that when creating the derived part that a SOLIDWORKS part template with Z-up orientation is used. Using a template with Z-up orientation will ensure that the derived part model is oriented with same way as the original xShape fuel tank model.

For more information on templates and model orientation please refer to the SOLIDWORKS set up section of this guide.

After inserting the xShape design, the new SOLIDWORKS part file can be saved both locally and to the 3DEXPERIENCE platform. The feature manager design tree will show the native 3DEXPERIENCE component as the first feature displayed with a physical product icon. The physical product icon signifies that the fuel tank is a native 3DEXPERIENCE component.

The MySession task pane will show that the new part file is referencing the native 3DEXPERIENCE Fuel Tank model.

The visual appearance of the inserted model is governed by the appearance settings of the SOLIDWORKS part template used. The colour and other visual properties of the new part can be set using the display manager.

Tip: When saving the new part file for the first time its good practice to use a different file name and title to the one used for the native 3DEXPERIENCE component. This will avoid any potential confusion in future when searching in the 3DEXPERIENCE platform for either one of the components. In this example the new part file is saved with the Title and file name “Fuel Tank – SW” to signify that it is the SOLIDWORKS native part related to the fuel tank design.

4. Add detail features in SOLIDWORKS

After the native xShape design has been inserted, the new SOLIDWORKS part file with respect to adding geometry can be treated like any other. In this example additional features are added to develop the engineering design of the motorcycle fuel tank. To be able to save the changes back to the 3DEXPERIENCE platform, the component must be locked to the user making the changes. When working on designs with other colleagues its recommended that the component is locked before making any changes. Locking a component will signify to other users on the 3DEXPERIENCE platform that its actively being worked on.

Summary

This use case highlights the recommended workflow for starting a component design using xShape, opening it in SOLIDWORKS, and adding detail features. Although xShape was used, the workflow is the same when any of the other SOLIDWORKS browser-based design apps for example xDesign or xSheet Metal.

In a real-world scenario, there will be times when the initial concept design needs to be modified at a later stage whilst ensuring the changes are propagated back to SOLIDWORKS. This is possible today by following the modification and update workflow explained in use case 2. However, in the current release of the SOLIDWORKS browser-based design apps, 2025x GA the original face IDs are not maintained when the local file representing the native 3DEXPERIENCE component is updated in SOLIDWORKS. The result can lead to failed features and dangling references on the derived SOLIDWORKS model. The intention is to support the maintaining of face IDs in a future release. Until this is implemented it is recommended that to avoid rework, any additional modelling using SOLIDWORKS is postponed until the design of the native 3DEXPERIENCE component is mature and unlikely to change.