| Rev # | Date | Description |
|---|---|---|
| 1.0 | Dec 2024 | Document created. |
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 that are on 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 3DEXPERIENCE 2025x GA and SOLIDWORKS 2025 SP0. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.
Acknowledgments
This document was authored by PLM Group and reviewed by Dassault Systèmes SolidWorks Corporation.
Preface:
3D Product Architect is a role that lets you create or modify multi-CAD and multi-discipline product structures without the use of SOLIDWORKS. The primary apps in this role are the Product Structure Editor and 3D Compose. With these apps, you can digitally mockup a new design or propose changes to an existing design on the web, reducing design iterations. Design changes are accelerated by making review cycles available to more people in the product development process through use of the similar app called the Product Structure Explorer. The Product Structure Explorer is available in the Collaborative Industry Innovator (CSV). Fundamentally, 3D Product Architect lets you form a collection of components into a structure to define a product for varying purposes. Then you can interact with the design department to adjust the specifications that define the various components.
The architect on the 3DEXPERIENCE platform can not only mockup the design, but watch it evolve as the designers evolve the mockup into a real product with precise assembly of the various pieces.
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Prior Knowledge
To get the most out of this SolidPractice guide, you should have knowledge in the following areas:
An understanding of core 3DEXPERIENCE principles (Dashboards, Apps & Widgets, Collaborative Spaces, Bookmarks)
Experience creating assemblies in SOLIDWORKS and saving them to a collaborative space on the 3DEXPERIENCE platform
A general understanding of how the structure of an assembly created in SOLIDWORKS is presented on the 3DEXPERIENCE platform using the Product Explorer app
How to open and edit an assembly stored in a collaborative space on the 3DEXPERIENCE platform and in SOLIDWORKS
How to use mates to control the degrees of freedom in an assembly
Getting Started
Any user with the 3D Product Architect role and a web browser can use the apps in this role to do the following:
Create new structures from existing components that are already saved to the platform.
Establish entirely new component structures that are empty at the time of creation and where the 3D content can be added later in the project.
This role enables more stakeholders within a company to connect with the product-development process because SOLIDWORKS is not required to create and maintain assembly structures.
Note: Users who do not have the 3D Product Architect role can access and view the assembly structures created by a user who has the 3D Product Architect role. Also, opening the structures in a CAD application like SOLIDWORKS does not require the SOLIDWORKS user to have the 3D Product Architect role.
Main Apps: 3D Product Structure Editor and 3D Compose
Among the apps that are included in the 3D Product Architect role, the Product Structure Editor and 3D Compose apps represent the core capabilities of the role.
Product Structure Editor: This app lets you create and edit the structure of the product. The default view of the structure is a tree list with different columns that can be changed according to preferences. You can also view the assembly as a diagram, which provides a more visual way to explore the content of a structure and how it is organized.
3D Compose: This app lets you view and interrogate a product structure, as well as manipulate the position of the components.
When adding the Product Structure app to a dashboard, the 3D Compose app is also added by default. The two apps can be used independently of one another, however.
Setup
When the 3D Product Architect role is assigned to you, you can add the apps in the role to a dashboard. Create a new dashboard, expand the Roles and Apps menu under the Compass and drag the Product Structure Editor into a dashboard tab. This creates two widgets, one for the Product Structure Editor app and another for the 3D Compose app.
If needed, you can also add a new tab containing a Bookmark Editor widget to make it easier to browse for content using the Bookmark folders.
Selected Use Cases
The use cases in this document are scenarios where using the 3D Product Architect role provides benefits for the following groups:
CAD users
Users who do not have access to CAD
Technical professionals and nontechnical professionals taking part in the product-development process
The use cases represent most of the scenarios for which you will want to use the 3D Product Architect role. There might be other uses cases not covered in this document, and there may be some overlap in specific areas of the use cases. But these selected use cases are different enough so that each can stand on its own.
Note: The use cases are meant to be read in the order they are presented in this document. You might find references to tools and techniques that are introduced in an earlier use case. Each use case showcases different techniques that are useful to everyone using the 3D Product Architect role. Even if a use case does not seem to apply to you, we encourage you to read all use cases.
Before creating anything, it is worth checking:
Which Collaborative Space will the content you create be stored in?
You can create components that reference content in any collaborative space you have access to and move content to different collaborative spaces later if needed, without breaking references. However, we recommend considering the location of the new content you create.
Make sure that the Product Structure Editor widget uses the correct credentials and collaborative space. You need to have at least Author credentials to create content on the 3DEXPERIENCE platform. Talk to your Platform Administrator if you do not have the necessary credentials for doing your work task.
What CAD format should I select when I create a new top-level item?
SOLIDWORKS CAD Format
Choose this format if you intend to edit the assembly later in SOLIDWORKS by adding or removing components, or adding mates and assembly features.
If your workflow is largely SOLIDWORKS based, this is the CAD format you should choose.
3DEXPERIENCE CAD Format
Choose this format if you intend to work on the Assembly later in an xApp like xDesign, or a CATIA-based app like Assembly Design.
Choose this format if you intend to utilize advanced filtering options.
Choose this format if you are planning to include the assembly in ENOVIA Variant/Option management.
The 3DEXPERIENCE CAD format allows limited edits from within SOLIDWORKS, such as adding or removing components under the 3DEXPERIENCE item. However, the geometry itself cannot be modified within SOLIDWORKS.
In SOLIDWORKS you can still include a 3DEXPERIENCE CAD-format assembly as a subassembly in a SOLIDWORKS assembly.
Other CAD formats. Choose these if you intend to create structures that are later going to be opened in programs such as Inventor, NX, or Creo.
Tip: The Administrator can change the order of the CAD formats that is shown in the New Product menu. In the Platform Management Dashboard under CAD collaboration, select Common settings > CAD sequencing for CAD template.
Considerations when opening an existing SOLIDWORKS assembly in 3D Product Architect
With 3D Product Architect, you can detach components from SOLIDWORKS assemblies that are In Work in the same way that you can mark a component in an assembly opened in SOLIDWORKS and remove it from there.
If the component you are removing has an external reference to another component in the assembly you are removing it from, this might lead to errors in Feature Manager in the SOLIDWORKS assembly. These errors are not visible in 3D Product Architect.
If you detach a component, you cannot undo the detachment. You can, however, use the history of the assembly to review what component got removed in order to get it back again. Using maturity states or change actions could help avoid this situation.
About the overarching scenario for the use cases and the 3D models
We are using as an example an imaginary company that delivers equipment for physical working spaces for use in workshops and manufacturing companies. They deliver systems of chairs, worktables, drawers and shelves and they tailor the delivery for each customer. As there are differences between the different customers in terms of the type and amount of needed equipment, as well as area and shape of the available space, our company needs a way to create new constellations of existing products for each new project.
We chose these particular product examples because we expect the reader to be familiar with the function of the products. This makes it easier to follow and understand the use cases, and learn to use the tools in the 3D Product Architect role.
For clarity, these are the various products in use in the cases – either inserted in the case or visible in the images:
| Chair | Single seat, no back rest | |
|---|---|---|
| Worktable | Worktable for a single person | |
| Space Divider | Mobile wall for dividing a room and providing basic noise dampening | |
| Server Rack Cabinet | For rack-mounted technical equipment | |
| Power outlet | For table mounting | |
| Drawer | Low drawer for hand tools and other equipment | |
| Office Lamp | Lamp for ceiling mount | |
| Laptop | Portable PC |
Use Case 1: Mockup
Anyone with at least Author access to a collaborative space containing physical products can use the 3D Product Architect role to create a new product structure based on components stored on their tenant. This means you can create new products consisting of CAD models made earlier without using a CAD program.
There are several reasons why you might want to create a mockup:
To establish a Bill of Materials (BOM) early in a process
To be able to create a quote
To show a prospective customer what is included in a delivery
To show a customer the difference between product options
To visualize in 3D what a delivery will look like early in a project
This role can be a powerful tool for those who do not use CAD software. Creating a new structure by reusing content in the 3D library does not require the use of traditional CAD software such as SOLIDWORKS.
The mockup process using 3D Product Architect often starts with creating a new top-level physical product. Then you create instances of additional components under this physical product. You can also create sublevels.
You can also insert some components as placeholders. Inserting placeholders can, for example, show that a CAD designer will add geometry to the node later using SOLIDWORKS or another CAD program supported by the 3DEXPERIENCE platform.
Use Case Example
Use Product Structure Editor to create a new product. In this example, we are selecting Start a New Activity > New Product.
In the New Product dialog box, enter a title and template for a new physical product, and credentials to access the template.
In this example, we are selecting SOLIDWORKS from the Template list. The template determines the CAD format and cannot be changed later (see page 8 “What CAD format should I select when I create a new top-level item). Any SOLIDWORKS templates uploaded to your tenant appear in this list. The credentials you enter must give at least Author rights to the collaborative space where you plan to store the content. In this case, we are also adding details such as a description under Show More.
Click Create. In the Product Structure Editor, a new top-level assembly is created, ready for component insertion. The 3D Compose application is automatically activated on the right side of the window when you add the Product Structure Editor widget to the dashboard.
Inserting components. You can insert components using the Action Bar under Edit or by dragging them from another application such as the Bookmark Editor. Ensure you place the component under the correct top-level assembly node. Since Product Structure Editor lets you view multiple structures simultaneously, verifying the correct node helps maintain accuracy.
Dragging and dropping a component. When you drag and drop a component onto a physical product, a confirmation message prompts you to verify the action.
Click Copy to confirm. The component is now inserted under the top-level assembly. This is the first component containing geometry, so the 3D Compose application displays a preview of the assembly.
Insert additional components by dragging them from the Bookmark Editor application and dropping them onto the top-level item. These components are placed under the same physical product, with their origin aligned to the origin of the top-level item. Inserting components this way might cause components to overlap, as shown in the following image.
Inserting components this way modifies the SOLIDWORKS file, however. To avoid unintended changes, consider inserting only released physical products under the top-level item. If you need additional subassembly levels, you can create them by first inserting other physical products. This scenario is covered in Use Case 2. If you mistakenly insert a physical product, you can detach it by right-clicking and selecting Detach, allowing for reinsertion as needed.
Insert a new instance of the table. To add another instance of an existing product within the same structure, you can use Copy and Paste from the Edit tab in the Action Bar or simply use the keyboard shortcuts CTRL + C and CTRL + V. Select the product to copy, click Copy, then choose the target item and click Paste to insert the product under it.
Tip: Using Copy and Paste in Product Structure Editor does not duplicate the product. It creates a new instance of it.
The assembly now has two instances of the same product in the same location. Although this does not impact the BOM of the assembly, you might need to move the components to a different location. For details on adjusting the position of a product, see Use Case 2.
Anyone with access to the new top-level assembly can do the following:
Open the assembly in SOLIDWORKS.
Use mates to make sure the components are positioned correctly.
Ensure that degrees of freedom and other design requirements are respected.
Preparations for exporting the product structure as a CSV file. Everything visible in the structure displayed in Product Structure Editor is included in the exported CSV file. You can select what columns to include when you export to a CSV file in step 14. To select the columns:
Right-click the column.
Select Tree List View Options.
From the list of available columns, select the column to include.
Hiding columns. To hide a column, right-click it and select Hide Column. To hide the Position Matrix, Type, or Lock columns, right-click any column, select Tree List View Options, and then hide any of the three columns.
button. The three columns will now be hidden, and the settings will apply only to this widget on the current dashboard tab.
Tip: Columns can be repositioned by dragging their titles to new locations.
The product structure can be expanded so that all levels are visible. To expand a product structure:
Select the top-level item in the structure.
On the Action Bar, click View > Expand All.
Displaying Thumbnail images in the structure. Enable thumbnails by right-clicking a column title and clicking Display thumbnails. Click the image icon on the top (1), then choose Pin Left (2) on the Display Thumbnails entry so that the column containing thumbnails is pinned to the left.
Click Close to go back to the structure. The thumbnails are now visible in the structure and pinned to the left.
Printing to PDF. On the Action Bar, click Tools > Print. This will produce a preview of the document, which you can then print to a PDF file.
The menu choice for printing to a PDF file might differ across different devices, but it is typically called Microsoft Print to PDF or Save to PDF. In this example, by clicking Print, you will be prompted to choose a location to save the PDF. This location will be outside your 3DEXPERIENCE platform, allowing it to be used in other contexts such as in a quote for a customer.
Exporting the structure. Once all components have been inserted, the structure can be exported as a CSV file if needed to be included in a quote. Alternatively, content can be directly shared by inviting customers to your tenant, allowing them to use either their own license or yours.
To export the structure to a CSV file, select Tools > Export. The CSV file format can be edited in applications such as Microsoft Excel.
The new physical product can be previewed by anyone with who can see the content of the Collaborative Space the product is stored in (see “What Collaborative Space will the content you create be stored in?”). It can be opened using a viewer app like 3DPlay. It is not needed to have 3D Product Architect role to view the product. It is also possible to open it in SOLIDWORKS and continue working on it there.
An alternative way of exporting the structure is to print to a PDF file using Tools > Print. A PDF created like this will include the thumbnails of the items in the structure, which adds clarity to the list of items. First, ensure that the thumbnail images are visible in the structure. To learn more about thumbnails, see step 12.
Use Case 2: Temporary Design
A CAD designer can use 3D Product Architect to quickly start a new assembly without opening SOLIDWORKS. Later in the process, the assembly and its components can be opened in SOLIDWORKS to mate components together, insert fasteners, and reuse the file for any downstream purpose, such as creating drawings.
This lets you:
Create new products on any device that has a web browser, including a tablet.
Visualize new products in context.
Decide the hierarchical structure of the assembly.
Recognize the need for additional components that are not modeled yet, which can be inserted temporarily using virtual components as placeholders.
Tip: If the intention of creating the physical product is purely to sketch something that can be abandoned later, consider setting the Maturity State of the product to Private. In this maturity state, only the owner of the product can see the physical product, as well as any Administrator. Set it back to In Work whenever the idea phase is done, and work is starting on the physical product.
In this use case, you will accomplish the following:
Create a new assembly with Product Structure Editor.
Work under a bookmark on Product Structure Editor.
Add existing items to the assembly.
Modify an existing assembly.
Remove and replace components.
Position components in the 3D Compose app.
Open the model in SOLIDWORKS to add mates.
Create a drawing in SOLIDWORKS.
Working under a bookmark can be useful when adding new physical products in a structure. It will ensure that the new physical products are visible in that bookmark, which makes it easier to find components later.
Use Case Example
Close any open products. If another product is open, the new product will appear alongside it, which is not what we want in this example. Close the product either by right-clicking the top-level item and selecting Close, or by going to the View tab on the Action Bar and clicking Close.
Create a product with a SOLIDWORKS CAD format. Under Start a New Activity on the Home Screen, select New Product. A name and description are assigned to the new product.
Working under a bookmark. Organizing the product under a bookmark makes it easier to locate later by browsing. On the Action Bar, select Work under Bookmark. In the Work under Bookmark dialog box, select the bookmark and click Set.
button becomes activated. To stop adding items to the bookmark, click the button and select Unset.
Inserting an existing product: worktable. To insert an existing product under the top level in the Product Structure Explorer:
Select the top-level item.
On the Action Bar, click Insert Existing.
To find a product, use the search box. For this example, search for “table.” The search results appear in Tile View, displaying thumbnails to help you find the right product.
Click the worktable product and click OK.
As this is the first product containing geometry, a preview of the product is displayed in the 3D Compose app. To view all geometry in the 3D Compose app, go to the Action Bar, click the View tab, and click Reframe.
Tip: If the wrong product is inserted, it can be detached from the structure by right-clicking and selecting Detach. This action closes the inserted product, allowing for the insertion of another.
Inserting another product: chair. Using steps 4a through e, insert a chair. By selecting the top-level item first, you place the chair under it. In the preview, you can see that the chair is resting on the same top plane as the worktable.
Tip: The products are modeled in SOLIDWORKS, where all geometry is positioned to rest on the top plane. In this case, the top plane represents the factory floor. 3D Product Architect respects the orientation and position relative to the coordinate system in the SOLIDWORKS file, which helps you accurately position it in 3D Compose later.
The chair is inserted with respect to its origin.
Moving the chair into position. To move the chair to a different position:
Click the chair seat. Although the chair seat is highlighted, the orange selection indicator shows that you are moving the entire chair assembly as a single item.
In the pop-up menu, click Move. This will display the Robot on the selected geometry. You can drag and drop the Robot on top of something else in the same assembly to move from that location. Moving the Robot to a different item will move that item, however.
When the Robot is positioned, do one of the following:
In the Translation text box, select a direction and type in a distance to move the chair accurately in that direction (see the image after step d).
Move the assembly by dragging the mouse over the ruler to snap to whole numbers during movement.
Tip: You can move just the chair seat if the SOLIDWORKS assembly is in a maturity state that allows changes, such as In Work. However, the position will be reset the next time the file is opened in SOLIDWORKS. The mates will recalculate the position, which will reset the position matrix in 3D Compose.
Click Save to store the new position.
Because the chair is in the Released state, attempting to move the chair seat triggers the following error message:
Rotating the chair. In the Robot, in the Rotation V: box, enter -30. Then click Save. The chair rotates -30 degrees on the Y (V) axis.
Copying the worktable to insert new instances of it. This process creates multiple instances of products. It does not duplicate them. To make a copy of the table:
In Product Structure Editor, select the worktable.
Press CTRL + C.
Click the top-level item and press CTRL + V.
In the confirmation message, click Copy. The table now occupies the same space as the previous one.
Moving the worktable. To move the copied worktable out of the way:
In Product Structure Editor, hide the first instance by right-clicking a row and click Hide in 3D. Hiding it ensures that you move the correct instance.
In the Robot, in the Rotation V: box, enter 180.
Click Save. The worktable rotates 180 degrees on the Y (V) axis so that it faces the other table.
Moving and rotating the chair. Repeat steps 9a through c to choose a suitable location for the chair.
Creating a new subassembly of the worktables and chairs. Now that you have two opposing tables with chairs, group them in a subassembly for easier replication. To create a subassembly:
On the Action Bar, select the top-level item and click New Product.
For this example, select the SOLIDWORKS Assembly template.
In the Title box, type “Table and chair group.”
Click Create.
Inserting the worktables and chairs into the subassembly. To insert the worktables and chairs into the subassembly:
Select the two tables and chairs by pressing Shift while clicking anywhere on the product row in the structure.
Drag the selected items into the subassembly you created.
In the confirmation window, click Move.
Now the assembly looks like this:
Creating copies of the subassembly. In this example, we will create four more instances of the Table and chair group. To create more instances of the subassembly:
Select the Table and chair group.
Press CTRL + C.
Click the top-level item and press CTRL + V.
In the confirmation message, click Copy.
Use the Robot to move the copied subassembly to a new location and press Save to confirm the move.
Repeat steps c through e until you have five instances total.
Detaching instances from structures. In this example, we need four instances, not five. To detach an instance from the structure:
In Product Structure Editor, select the instance in the middle.
Right-click it and select Detach. This removes the instance from the structure.
The subassembly now looks like this:
Inserting a small drawer from Bookmark Editor.
We now want to insert a new product. A small drawer can be inserted by browsing to the product in Bookmark Editor and dragging it into the structure. The new product will then be placed in the origin and is visible together with the rest of the products in the structure. You might want to move the new product to the right location using the Robot before proceeding.
Tip: Consider adding a Bookmark Editor widget to the same tab as the 3D Product Architect app. It is easier to insert products if they are placed in Bookmarks.
A new instance of the drawer can be inserted using Copy and Paste. The drawer can then be positioned as needed by clicking it and selecting Move. Then use the Robot to move it to a new location and press Save to confirm the move
Inserting an additional product under an existing subassembly. Inserting an existing product under a subassembly instantiates it under all occurrences of that subassembly. When moving or rotating the inserted product, the same relative position will be applied to all subassembly instances.
In this example, a power outlet is inserted from Bookmark Editor (see step 15) and then dragged onto the table and chair subassembly in Product Structure Editor. The power outlet is then instantiated across all subassemblies. One instance is positioned to rest on top of a table, and all other instances automatically follow the same position matrix.
Inserting a new product. Insert a space divider between the worktables using Bookmark Editor (see step 15). One new instance of the space divider is created and can be positioned as necessary using the Robot.
Repositioning components using the Position Matrix. The Position Matrix column indicates if a physical product has been moved or not. It will display an icon if the component is moved or rotated. Right-clicking the Position Matrix icon of a moved part allows copying its position. This position can then be reused by pasting it onto another component.
Tip: If the Position Matrix column is not visible, you can display it. To display a hidden column, right-click any column title, select Tree List View Options, and then find the column in the list.
In the following steps, we will reuse the position matrix of the last-placed instance of the Table and chair group subassembly and use it to position a space divider.Copying the space divider. A new instance of the space divider can be inserted by selecting it, pressing CTRL + C, selecting the top item, and pressing CTRL + V. This instance can then be positioned near the end of the last worktable.
Repositioning the copied space divider using the Position Matrix from the Table and Chair Group subassembly. The Position Matrix icon is right-clicked on the Table and chair group subassembly and Copy Position is selected.
and select Paste position.
Inserting additional products. Now insert a shelf, server cabinet, and high drawer by dragging their physical products from Bookmark Editor.
Reposition the products using the 3D Grid. The 3D Grid can simplify positioning. To reposition the products using the 3D Grid:
In the 3D Compose app, go to the Action Bar and select the Tools tab.
Click 3D Grid.
To adjust the grid settings, such as pitch, go to the Action Bar of the 3D Compose app and select Preferences.
Opening the file in SOLIDWORKS and adding mates. Now you can open the file in SOLIDWORKS and add mates that accurately connect components and manage their degrees of freedom. The positions that were applied in 3D Compose are respected in SOLIDWORKS.
Tip: If SOLIDWORKS is open in another window and you are logged into the same tenant, you do not need to open the file in SOLIDWORKS separately. You can drag the top item directly from Product Structure Editor in the web browser into SOLIDWORKS.
Use Case 3: Project Kick-Off
You can start a new project by creating a structure and organizing the assembly into subassemblies and components. You and your team can create the geometry in the different files later. In this use case, you will accomplish the following:
Add new products.
Add new parts.
Change the structure.
Insert a new product under multiple parents.
Add an Enterprise Item Number to components.
Open the physical products in SOLIDWORKS to add geometry and mates.
Use Case Example
In this use case example, you will create a structure consisting of empty CAD models.
Create the top-level physical product by going to Start a new activity and choosing New Product.
In the New Product dialog box, enter a title, template, and credentials. In this example, select a SOLIDWORKS template and any collaborative space. Enter credentials that ensure Author access rights at the minimum.
Click Show More to expand the dialog box and add a description for the new product.
Click Create to create the product.
Insert a new part under the top-level physical product.
Select the top-level physical product.
Tip: If you do not select the top-level product before creating the part, the new part becomes a new top-level item, separate from the original product.In the Action Bar, click the Edit tab.
Expand the New Product menu and click New Part.
In the New Part dialog box, enter details for the new part, including a name. In this example, select the same collaborative space and credentials you entered in step 2. Then click the Create button.
Create a physical product as a subassembly under the top level.
Select the top-level assembly so that the new product is placed under it.
Go to Start a new activity and choose New Product.
In the New Product dialog box, enter a title, template, and credentials. In this example, select a SOLIDWORKS template and any collaborative space. Enter credentials that ensure Author access rights at the minimum.
Click Create to create the product. The new product appears under the top-level product.
Repeat step 5 to create two more parts under the top-level product.
You can delete physical products or parts that you do not need. In the previous step, you created a part that you do not need. To delete one of the new parts, go to the Action Bar and select Lifecycle > Delete. You cannot undo this action.
Note: Deleting content requires certain rights. Also, your administrator might have applied tenant settings that prevent you from deleting content. If you cannot delete a product or part, speak to your administrator.
In our example, the project now looks like this:
You can reorder the structure by moving a part to a different location at the same assembly level. Reorder the structure to control the assembly order and the BOM layout. To move a part:
Drag New Part below New Product until a brown line with a dot appears.
Drop New Part below New Product.
In the Reorder message, click Reorder.
The part is now under New Product.
You can restructure the assembly by dragging New Part 2 to a subassembly level under New Product. When restructuring this way by dragging a component to another component, this is called a move operation in Product Structure Editor. It should not be confused with changing the position of a product in the 3D Compose app.
In this example, we drag New Part 2 and drop it onto New Product, then click Move in the confirmation window. New Part 2 is now beneath New Product.
Making a new part under New Product. Create an additional new part under New Product. In this example, this part is called New Part 3.
Create two copies of the New Product subassembly.
Select New Product and press CTRL + C.
Select the top-level item and press CTRL + V.
In the confirmation dialog box, click Copy.
Repeat steps a through c to create another copy.
Now you have three instances of the subassembly. The instance Title column shows that the title of each instance has a number appended to it.
Insert a new product under all subassemblies simultaneously.
You might need to create an item to use in multiple places in the structure. This can be a physical component like a mounting bracket, or a reference component to indicate a BOM item with no CAD model, such as packaging or a product manual. When creating a product or part, you can opt to insert an instance of it under several levels at once.
Note: A part cannot be inserted under another part.
To insert a new part under all subassemblies simultaneously:Select the top node New Project and one of the New Product nodes.
On the Action Bar, click the Edit tab.
Expand the New Product menu and click New Part.
In the confirmation box, click OK.
dialog box, enter details for the new part. In this example, name the part Extra Part. Select the same SOLIDWORKS template, collaborative space, and credentials you entered in step 2.
Click the Create button. The message "Object Successfully Inserted" appears.
The part appears in the selected nodes in the structure, which is the top level and the subassembly. Because the subassembly has three instances, the part appears in each instance of the subassembly.
Add an Enterprise Item Number to all components.
Now that you have set up a structure, now is a good time to add Enterprise Item Numbers to the components.
In the Product Structure Editor app, select all components by right-clicking the top item and selecting Expand All.
Note: To select a component, it must be visible in the structure with its parent expanded.
Select all components in the structure by clicking the top left check box or by pressing CTRL + A.
On the Action Bar, click the Edit tab.
In the Edit tab, click Set Enterprise Item Number.
In this case, six objects appear in the Enterprise Item Number generator. It does not display each instance of each component individually.
Click the top left check box to select all components.
Click the plus sign on the top right to generate numbers for the selected components.
In the confirmation box, click OK. The Enterprise Item Number generator previews the six unique numbers it selected for these components.
Click Set to apply the Enterprise Item Number assignments.
Now when you display the Enterprise Item Number column in Product Structure Editor, it shows the numbers assigned to the components. Each instance of the same component has the same number.
Configure SOLIDWORKS to open components that do not contain geometry.
Now you can open the assembly in SOLIDWORKS and start adding content to the files. In this example, none of the components contain geometry. Before attempting to open the assembly in SOLIDWORKS, ensure the platform settings let you open components with no geometry.
Note: Changing platform settings as described below can only be done by the Administrator of the tenant.Go to Platform Management Dashboard > Content > CAD Collaboration > SOLIDWORKS > Settings > Open.
Ensure the setting Filter 3DEXPERIENCE Engineering items with no geometry is set to one of the Off options.
This setting affects how SOLIDWORKS interprets physical products created outside of SOLIDWORKS when opening them.
The options are:
Always Off (Default): Opens physical products containing no geometry.
Always On: Does not open physical products containing geometry.
Default Off (user control): Opens physical products containing no geometry unless you disable it from the SOLIDWORKS MySession app.
Default On (user control): Does not open physical products containing geometry unless you enable it from the SOLIDWORKS MySession app.
Open the assembly in SOLIDWORKS.
Once you open the structure in SOLIDWORKS, SOLIDWORKS becomes the CAD master and controls the content. However, you can still change the structure in Product Structure Editor.
Rename the components in SOLIDWORKS.
When Autonaming for SOLIDWORKS is enabled in the Platform Management dashboard (speak with the tenant administrator to set this up), you can rename the component titles to match their filenames. Renaming them ensures that the assembly created in 3D Product Architect follows the SOLIDWORKS file-naming conventions. Renaming the components is not necessary but is a good idea.Enable Autonaming. For instructions, see the SolidPractice “Naming Strategies for SOLIDWORKS Parts, Assemblies, and Drawings.”
Right-click a component and select Rename Title.
In the Rename Title dialog box, select Reset Title to Filename.
Click OK.
Save the file to the platform.
For each component, repeat steps a through e.
Use Case 4: Multi-CAD
In this use case, you will update the structure built in Use Case 2 to support multiple CAD formats. The use case addresses the following topics:
Prerequisites for multi-CAD
3DEXPERIENCE native format
Inserting products created in different CAD software
Working on a multi-CAD product in SOLIDWORKS
Use Case Example
First, we will ensure that the 3DEXPERIENCE platform is correctly configured to operate in a multi-CAD environment. Then we will insert the structure from Use Case 2 and work on it in SOLIDWORKS.
Note: Changing platform settings as described in this use case can only be done by the Administrator of the tenant.
Each connected CAD software has unique settings. Go to the Platform Management dashboard’s CAD Collaboration section. Review the settings for your particular CAD software. Please see the 3DEXPERIENCE User Assistance for information for your CAD software.
Create conversion rules in Derived Format Management. These rules enable all connected CAD software to generate multi-CAD graphical presentations of CAD objects when you save in SOLIDWORKS. It saves the graphical presentations to the cloud. This step is needed in order to see the preview of 3D files in the viewer apps in a 3DEXPERIENCE dashboard, such as 3DPlay.
In Platform Management Dashboard > Content > Collaborative Space Configuration Center > Derived Format Management, click Conversion Rules.
Click the plus sign.
In the New Conversion Rule dialog box, enter the rule parameters in the following image.
Click OK to create the rule.
In Derived Format Management, click the plus sign again.
In the New Conversion Rule dialog box, enter the rule parameters in the following image.
Click OK to create the rule.
Create a top-level node for a multi-CAD assembly in the native 3DEXPERIENCE CAD format.
We will start by creating a new product in the 3DEXPERIENCE native format. Go to the Home Screen, and select New Product. In the New Product dialog box, click the arrow and select 3DEXPERIENCE – Default product. Enter a Title and Credentials. Then click Create.
column in Product Structure Editor shows that the format is 3DEXPERIENCE. Hovering over this icon displays the CAD name.
Insert the SOLIDWORKS assembly from Use Case 2 in the new top-level product.
Use 3DSearch to locate the assembly. In this case, we can search for the string “Case 2” in the search box on the top of the screen:
Drag the assembly from the 3DSearch result list and drop it into the top-level product. When the plus-sign indicator labeled Insert appears, the assembly is added to the current assembly, instead of opening as a separate instance.
The Title column shows that the product is multi-CAD level. The CAD Format column shows the difference in formats between the top level and the subassembly.
Insert 3DEXPERIENCE CATIA native components into the product.
Components created in CAD systems other than SOLIDWORKS can also be inserted into the structure. In this case, an office light and a laptop, modeled using 3DEXPERIENCE CATIA, are added to the product.
We will add two office lamps, either by searching for the 3D model or dragging it in form a Bookmark. The lamps are positioned using the Robot tool for precise placement. See Use Case 2 for instructions on using the Robot.
Add 3DEXPERIENCE CATIA components inside a SOLIDWORKS assembly.
Insert an instance of a laptop modeled with 3DEXPERIENCE CATIA into one of the subassemblies and onto a desk. This can be done by dragging a physical product from a Bookmark or a search result. By including the laptop in the SOLIDWORKS subassembly with instantiated desks, it instantiates across each table group.
We are using Snap to Object to position the laptop on the desk. The Snap to Object function allows you to quickly align components by selecting a face on one object and dragging it to a corresponding face on another object, making them coincident. As shown in the image below, activate Snap to Object from the toolbar, select the bottom surface of the laptop and drag it to the top surface of the desk to snap it into place.
Use the Robot tool to finalize the laptop’s positioning within the subassembly as shown in Use Case 2. Because the laptop was inserted to the subassembly level in step 6, its new placement is automatically replicated across all instances of the desk.
Review the assembly in SOLIDWORKS. If needed, you can open the assembly to observe its behavior in SOLIDWORKS. Right-click the top-level structure and select Open with > SOLIDWORKS Connected.
The structure can be opened in any 3DEXPERIENCE-connected CAD application with this method.
The entire assembly opens in SOLIDWORKS, with the top-level and other non-native components treated as imported items. You cannot modify imported items directly. However, these components still appear in the SOLIDWORKS FeatureManager Design Tree and are represented graphically in the software.
Use Case 5: Large Assemblies
You can work with large assemblies with different components created in different CAD applications. Create the top-level assembly with 3D Product Architect applications and subassemblies in SOLIDWORKS or other connected CAD applications. This approach ensures that the top-level assembly uses a 3DEXPERIENCE native format and can later be opened and modified in CATIA applications, such as Assembly Design.
This use case includes the following topics:
Settings for large assemblies
Working on large assemblies
Reordering items in the structure
Use Case Example
Select settings that help with large assemblies.
In 3D Compose, click the cloud icon.
In Edit preferences, activate Automatically reload recents from last session to prevent large assemblies from loading automatically when you open the website.
In Geometry Quality, select Optimized to improve performance when working with larger assemblies.
Click Save.
Create a new base product for a large assembly and insert components into it.
In this example, the finalized multi-CAD assembly from Use Case 4 will be applied multiple times within a factory layout using applications in 3D Product Architect. In this example, another engineer has already modeled the factory layout in CATIA.Use Product Structure Explorer to create a new base assembly with a 3DEXPERIENCE native CAD format as done in Use Case 4. This assembly will serve as the base model for the factory layout.
Add the factory layout model. To add the factory layout model described in step 2 into the current assembly, use 3DSearch to locate it and drag it into the open assembly in Product Structure Editor.
The layout model is a part, not an assembly. All components will therefore be inserted under the base assembly created in step 2, and not under this model.
Tip: If you need to transform the product created in 3DEXPERIENCE CATIA into a native CAD part, you can use the Product to Part command in Product Structure Explorer to do so.
Insert an instance of the multi-CAD assembly into the top level of the factory layout being developed. Use Snap to Object function, as described in the previous section, to initially insert the assembly onto the floor. Afterwards, position the assembly correctly within the layout using the Robot tool as described earlier.
Copy the instanced assembly within the assembly.
Copy the assembly into the three rooms shown in the image in the previous step using the CTRL + C and CTRL + V shortcuts as described in the first Use Case. Then position the assemblies as you wish in the rooms by using Robot like in earlier Use Cases.Once the three rooms are created, you can see that the wireframe structure, designed to facilitate positioning, is causing the 3D Compose application to process more slowly. To improve performance, temporarily disable the wireframe by turning off the wires in the View Modes menu, as shown in the following image.
Add the rest of the components.
Using Product Architect applications, insert new instances of the assembly to the other rooms of the factory model. Refer to the first Use Case for guidance on inserting components. This will grow the size of the assembly by a bit. Some extra assemblies were also added to this example case as can be seen from the following image.
Reorganize the design tree.
After copying and pasting assembly instances in earlier steps, the assemblies might not be organized correctly in the design tree according to the factory layout, as can be seen in the following image.
Restructuring of the product tree is done by using the Reorder function to arrange the rooms in the proper order in the top-level assembly. As shown in the following image, select the top-level assembly and activate the Reorder function.
Change the order of the items by selecting the row of the item you want to reorder, then use the arrows on the right side of the Tree Reordering-dialog, to change the order of that component. To confirm the reorder, press the OK button.
Open the large assembly in a connected CAD software.
As demonstrated in previous examples, you can open this assembly in any CAD application connected to the 3DEXPERIENCE platform, such as SOLIDWORKS.
General Recommendations
This section contains general advice about working with 3D Product Architect. Some of the advice is applicable to other roles and apps on the 3DEXPERIENCE platform.
Use Lock when you intend to make changes to a structure.
Whenever you intend to make changes to a document or a physical product on the 3DEXPERIENCE platform and you are working with others, consider using Lock. Enable it before you start making changes so that your team members can see that you are working on it. Then use Unlock when you are done making changes.
Change governance using Change Actions and Routes.
Change governance using Change Actions and Routes if the company prefers to have a planned and traceable approach to product development.
Use 6W tags to interrogate and analyze the structure.
You can use the 6w tags to interrogate and analyze the content of a structure. This can be useful to quickly get information on specific aspects of larger structures.
For example, you could use them to check if all components are Released. This can be achieved as shown in the following image. We click the 6w tag button first, then find the Maturity State tag group. If we expand the Options to the right of the tag group, we can click the palette icon and add colors to the tags in the tag group. In this case, blue signifies a Released product.
Use Relations to get an overview of the content.
In Product Structure Editor, you can select any component and click Tools > Relations to open the Relations app. This enables you to see the relations on this particular component, such as its parent and child components. It also lets you see if there are markups or bookmarks associated with the structure.
Multi-select objects to fill in attributes on more than one item.
You can multi-select more than one component at a time to make changes to its attributes. For example, you can add a common description text to three different components. In the following image, we select three components, right-click them and click Information. In the Information Panel, we can now change some of the attributes for all the three components at once. The components must have a Maturity State of In Work.
User Assistance
The 3DEXPERIENCE User Assistance website provides guidance for the use of various tools on the platform. Another place to find information on how to use 3D Product Architect is in the ENOVIA user forum.
Dassault Systèmes User Assistance
Help for 3D Product Architect can be found under the apps Product Structure Editor and 3D Compose.
Help in Product Structure Editor:
3DEXPERIENCE User Assistance R202Xx on the Cloud > Social and Collaborative > Multidiscipline Configured Product Development > Product Structure Editor
Help in 3D Compose:
3DEXPERIENCE User Assistance R202Xx on the Cloud > 3D Modeling > Mechanical Systems > 3D Compose
3DEXPERIENCE Platform
The ENOVIA User Community has a collection of user articles that show different aspects and techniques of the 3D Product Architect role, explained with text, images, and video.
Community: ENOVIA User Community > Wiki SectionYou can find tips listed by role at:
ENOVIA Expert Insights | Tips & Posts (Per Role) > Tips (Per Role) > 3D Product Architect (PAU)
You can find posts per role at:
ENOVIA Expert Insights | Tips & Posts (Per Role) > Posts (Per Role) > 3D Product Architect (PAU)
We hope that you find this document informational and useful. We request that you leave brief feedback about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from DS SOLIDWORKS Corp.
