The following use case describes the recommended workflow for designing a new component in xShape in the context of an assembly created in SOLIDWORKS. The internal components for a new gaming controller design have been positioned in a SOLIDWORKS assembly. xShape will be used to design the external shape of the gaming controller.
Although xShape is the xApp used in this example, the methodology is the same for all of the other xApps for example xDesign or xSheet Metal.
1.Saving the SOLIDWORKS Assembly to the 3DEXPERIENCE Platform
A new SOLIDWORKS assembly design is saved to a collaborative space on the 3DEXPERIENCE platform using the Save to 3DEXPERIENCE command.
During the save process ExactGeometry representations of each component are automatically generated. ExactGeometry representations are necessary to be able to visualize and reference the geometry of SOLIDWORKS components in the SOLIDWORKS browser based design apps. The time necessary to generate ExactGeometry can be longer than the save to 3DEXPERIENCE process, especially when the geometry is complex, or when the assembly contains a high number of components. The ExactGeometry generation process can be monitored using the Convert Status column in the MySession task pane. Successful creation of ExactGeometry for each SOLIDWORKS component is represented by a green circle with a white check mark.
The geometry of a SOLIDWORKS component will not be visible when opened in a xApp until the ExactGeometry representation has been generated.
2. Opening the SOLIDWORKS assembly in xShape
Using the Open command, design data (physical products) originating from SOLIDWORKS can be opened in an xApp in the same way as a 3DEXPERIENCE native design.
After the Gaming Controller is opened in xShape, the Design Manager displays a red SW icon for the top-level assembly and its components to signify that they originated from SOLIDWORKS.
3. Creating and Inserting a new component in xShape
With the Gaming Controller assembly loaded in xShape an existing xApp authored component can be inserted into the assembly, or a new component can be created in context of the assembly. In this use case a new component to represent the gaming controller shape is created in context using the Insert New Component command.
After the new component has been created in the assembly, xShape design features can be used to generate the desired geometry in context of the SOLIDWORKS design.
Saving the assembly in xShape will update the SOLIDWORKS assembly.
4. Propagating the Modifications Made in xShape to SOLIDWORKS
The process of propagating the changes made in xShape back to SOLIDWORKS will depend on the status of the local working folder. Let’s look at a couple of scenarios.
Original Files Deleted from the Local Working Folder:
If the SOLIDWORKS assembly and its components were deleted from the local working folder since it was last opened in SOLIDWORKS, opening the assembly after the save in xShape will result in the latest modified files being downloaded to the local working folder including the new shape Controller component.
The Controller Shape component created in xShape is downloaded and converted to a SOLIDWORKS part in exactly the same way as the mounting bracket component in use case 1. One point to note is that the SOLIDWORKS assembly will have a MySession status “File is modified by synchronization since last open from 3DEXPERIENCE” indicated by the orange triangle. This is because the native SOLIDWORKS assembly file contained within its physical product was not updated by xShape. The SOLIDWORKS assembly file can be updated by re-saving it to the 3DEXPERIENCE platform.
Original Files still Reside in Local Working Folder:
When the SOLIDWORKS assembly file and components still reside in the local working folder (have not been deleted) then the MySession status column is automatically refreshed after opening the assembly. In this scenario the top-level assembly has a status icon showing that a newer version is available on the 3DEXPERIENCE platform. Hovering the cursor over the icon displays a tooltip that describes the modification.
The MySession Reload from Server command is used to propagate the modifications made to the assembly in xShape to the assembly now open in the SOLIDWORKS session and local working folder.
When reloading an updated component, the same three options described in use case 1 are presented.
Reloading the selected file only will reload the assembly including any modifications to the structure, in this case the new controller shape component.
After the reload the SOLIDWORKS assembly will have a MySession status “File is modified by synchronization since last open from 3DEXPERIENCE” signified by the orange triangle. The assembly file can be updated by saving it back to the 3DEXPERIENCE platform using the Save to 3DEXPERIENCE command, as discussed in the previous section.
Important Note: When saving a modified 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. This is the same process that is described in step one of this use case when saving SOLIDWORKS design data to the 3DEXPERIENCE platform. The generation of ExactGeometry 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. The convert status of the component will show an orange clock face to signify that the ExactGeometry is still being processed.
When the exact geometry creation process has completed successfully, the convert status will automatically update to display a black circle. The component can be now be updated using the Reload from Server command. The graphics body will be automatically replaced by the BREP geometry during the reload.
The green circle/white check mark status represents a successful conversion of SOLIDWORKS geometry. The black circle signifies that ExactGeometry has been successfully generated for a component authored in an xApp.
5. Modify the Assembly in SOLIDWORKS
Any modifications to an assembly containing 3DEXPERIENCE native components can be easily propagated back to the 3DEXPERIENCE platform. In this example a modification to the position joystick component was required. The change in position has resulted in the base of the component interfering with the external casing that was created using xShape.
A modification to the overall shape is now required to accommodate the new Joystick position. This must be done in the original authoring app xShape. First however, the SOLIDWORKS assembly must be saved to the 3DEXPERIENCE platform to capture the new joystick position.
Important Note: When making modifications to the geometry of SOLIDWORKS components, monitor the Conversion Status in the MySession task pane column after saving to the 3DEXPERIENCE platform. As explained in step 1, only components with an up-to-date conversion status will be visible within xApps and 3DEXPERIENCE platform viewer apps.
6. Update the Assembly in xShape
Modifications made to the assembly design in SOLIDWORKS are propagated to a cloud design app one of two ways. If the assembly was not open in an xApp session when it was saved in SOLIDWORKS. The next time it is opened in an xApp the assembly will automatically update to reflect the modification last saved from SOLIDWORKS.
If the assembly was already open in an xApp the Global Refresh command can be used to update all of the object currently loaded in session
After the assembly design is refreshed the new position of the Joystick component is updated to reflect the change made in SOLIDWORKS.
The controller shape component can now be modified using the sub division modelling tools in xShape to take account for the new Joystick position. When the changes are complete, the component is then saved.
The saved modifications from xShape are propagated back to SOLIDWORKS by repeating the reload from server workflow outlined in Step 4.
Before reloading any component or assembly in SOLIDWORKS, always remember to check that the exact geometry conversion status of the last saved items is up to date as shown in the Convert Status column by refreshing the MySession information. When saving components with complex geometry the conversion can take a few minutes to complete.
Reload the changes when conversion is marked as up to date.
Note: When reloading an assembly, choosing the option to Reload file and references will not only reload the assembly, but will also reload any modified components.
The reload operation updates the assembly loaded in session with the modifications made to the Controller Shape component.
Summary
Although this use case demonstrates designing in context of a SOLIDWORK assembly using xShape, the same workflow is applicable when working with the other xApps for example xDesign and xSheet Metal.
