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!

• Fundamentals of Toolbox management using 3DEXPERIENCE
• Platform administrator settings
• Saving existing assemblies referencing Toolbox parts
• Inserting Toolbox parts
• Toolbox Physical Product characteristics
• Attribute mapping for Toolbox Physical Product
• Opening Toolbox parts 

• FAQs

   

Revision History

日本語版は QA00000125578 からダウンロードできます。

中文版可从 QA00000125578 下载。 

Note
All SolidPractices are written as guidelines. You are recommended to use these documents only after properly evaluating your requirements. The distribution of this document is limited to Dassault Systèmes SOLIDWORKS employees, resellers, and customers that are on active subscriptions. This document may not be posted on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SOLIDWORKS Corporation.

This document was updated using the SOLIDWORKS Design app (user-license version) from 3DEXPERIENCE Cloud platform R2026x FD02. The content also applies to Design with SOLIDWORKS app, used with the device-license version of SOLIDWORKS Design 2026 SP02.

For simplicity, 3DEXPERIENCE Cloud platform is referred to as 3DEXPERIENCE in the subsequent sections of this document.

If you have questions or need assistance in understanding the content, get in touch with your designated reseller.

1) Preface

For companies that use SOLIDWORKS Toolbox in their assemblies, easy access and management of Toolbox parts are essential. This document addresses those requirements, and explores the tools and methods that are available for SOLIDWORKS Toolbox management using 3DEXPERIENCE. Configuring or customizing SOLIDWORKS Toolbox library is not covered in this document - a separate document called ‘Setting up SOLIDWORKS Toolbox’ is available on this topic.

References:

1. 3DEXPERIENCE User Assistance

• Installation and Setup > Social and Collaborative > Multidiscipline Configured Product Development (Collaborative Design) > Design with SOLIDWORKS > Configuring Attributes > Configuring Standard Libraries Management

2. SOLIDWORKS Help > Toolbox

• SOLIDWORKS Toolbox Overview > Installation and Configuration > Configuring Toolbox > Toolbox - 3DEXPERIENCE
• Toolbox Components in the 3DEXPERIENCE Platform
• Saving Existing Toolbox Components
• Saving New Toolbox Components

2) Fundamentals

a) Prerequisites

i) In SOLIDWORKS Design

Toolbox management using 3DEXPERIENCE only works from SOLIDWORKS assembly files, and with the following local settings activated:

• Add-ins –

  • SOLIDWORKS Toolbox Library

  • SOLIDWORKS Toolbox Utilities

  • 3DEXPERIENCE (in SOLIDWORKS Design device-license version when Design with SOLIDWORKS app is installed)

• System Options –

  Hole Wizard/Toolbox > Make this folder the default search location for Toolbox components.

   

  

ii) On 3DEXPERIENCE 

The following target collaborative space must be accessible:

Collaborative Spaces Configuration Center > Standard Libraries Management > ToolBox settings. 

By default, this is set to Common Space. To use a different collaborative space, its visibility must be set to Public.  

b) Workflow

Toolbox parts saved to 3DEXPERIENCE by one user become available for re-use by other users without any duplication, and from any SOLIDWORKS client computer connected to the same platform. To manage Toolbox parts using 3DEXPERIENCE, you can -

• Open an existing local assembly referencing Toolbox parts, and save to 3DEXPERIENCE.

• Insert new Toolbox parts in an assembly from the Design Library task pane tab, and save to 3DEXPERIENCE. 

For both the scenarios, the system automatically enforces the following when you save the assembly to 3DEXPERIENCE:

• For a new size / configuration, saves a new part with a single Physical Product to the target collaborative space. 

• Sets the Physical Product’s maturity state to In Work or Released, as per the ToolBox settings on 3DEXPERIENCE.

• For a size / configuration that already exists on 3DEXPERIENCE, retrieves the part from 3DEXPERIENCE and synchronizes locally.

Note: Toolbox management using 3DEXPERIENCE only supports the Create Parts option that generates individual parts for the sizes / configurations.

c) Design with SOLIDWORKS

Design with SOLIDWORKS is the 3DEXPERIENCE connector app for SOLIDWORKS Design device-license version. When you install this app, it enforces the following User Settings for Files in the Toolbox Setup utility:

1. Activates Create Parts
2. Assigns the following file path in the Create parts in this folder field - 

%LocalAppData%\\DassaultSystemes\\CATTemp\\ENOUSWC\\Resources\\[tenant ID]\\Toolbox

This is the Toolbox local cache folder. In this folder, the app generates *.sldprt files and 3DEXPERIENCE cache files (i.e. *.v6 and *.srv.v6) for each of the sizes / configurations saved to 3DEXPERIENCE.

These cache files are essential for the Toolbox *.sldprt files to synchronize with 3DEXPERIENCE. The cache files are hidden by default, so only visible with the relevant folder option enabled.

New Toolbox parts inserted into an assembly do not create the cache files until you save the assembly to 3DEXPERIENCE.

In the Toolbox Setup utility (SOLIDWORKS Design device-license version), the other two User Settings for Files are not supported for Toolbox management using 3DEXPERIENCE:

Create Configurations

Create Parts on Ctrl-Drag

Do not change User Settings to either of these two options as this will not work with 3DEXPERIENCE. This will also prompt the following message when you attempt to use a Toolbox part:

⚠️ Note: After you install the Design with SOLIDWORKS app on a computer, do not disable the 3DEXPERIENCE add-in if you intend to use Toolbox parts.  

If you do so by mistake, and then insert any new Toolbox parts into an assembly, those will continue to be referenced from the Toolbox local cache folder as per the file path for Create parts in this folder. To rectify the references for those components, simply save the assembly locally, make sure that 3DEXPERIENCE add-in is active for Start Up, close SOLIDWORKS, and relaunch it from the app in 3DEXPERIENCE Compass. Then save the assembly to 3DEXPERIENCE.    

Also, do not change the User Settings for Files in the Toolbox Setup utility, to either of the two options below.

If you do so by mistake while the 3DEXPERIENCE add-in is disabled (also by mistake),

➡️  and then insert new Toolbox parts into an assembly, 

➡️  then save the assembly to 3DEXPERIENCE by activating the 3DEXPERIENCE add-in within the same SOLIDWORKS session,

↪️ follow the additional steps below to rectify the Toolbox parts references for the assembly:

1. Make sure that 3DEXPERIENCE add-in is active for Start Up, 
2. Delete the assembly and Toolbox parts from the 3DEXPERIENCE files on This PC tab of the task pane, 
3. Close SOLIDWORKS and relaunch it from the app in 3DEXPERIENCE Compass,
4. Open the assembly from 3DEXPERIENCE and save it back,
5. Search for and delete any unwanted duplicates of Toolbox parts from 3DEXPERIENCE, that have been created as a result of the unsupported workflow.

d) SOLIDWORKS Design User-License Version

The SOLIDWORKS Design app in the 3DEXPERIENCE Compass is the user-license version. This app is less susceptible to user errors compared to the device-license version, because -

1. It does not have the Files option in User Settings of the Toolbox Setup utility.  

   

The Create Parts option is hardcoded within the app, which uses the same Toolbox local cache folder as the Design with SOLIDWORKS app.  

2. The 3DEXPERIENCE add-in is not available in the Add-Ins list. This is also hardcoded within the app in online mode.

3) Platform Administrator Settings for Toolbox Components

a) Target Collaborative Space and Maturity State

The platform administrator can designate a target collaborative space for Toolbox parts. They can also set the initial maturity state to either In Work or Released. This maturity state setting applies to the Toolbox parts that are saved to the target collaborative space for the first time after the setting is deployed.

These settings are available in the ToolBox settings section of the Standard Libraries Management widget of Collaborative Spaces Configuration Center.  

Out-Of-The-Box (OOTB) values for these settings are –

Collaborative Space = Common Space 

State = RELEASED 

As mentioned in section 2)a)ii), to designate a collaborative space other than Common Space, you must set its visibility to Public. 

The values set in ToolBox settings only affect the Toolbox parts that you upload after you define those values. As an example, consider an assembly that you previously saved to 3DEXPERIENCE with Toolbox parts saved to Common Space as Released. 

Then in ToolBox settings, you designate a different value for Collaborative Space and set State to IN_WORK. 

If you then open the assembly in SOLIDWORKS from 3DEXPERIENCE -     

1. The previously saved Toolbox parts will still be in Common Space as Released. This will still be the case even if you clear local cache for both the assembly and the Toolbox parts. Any subsequent save command on the assembly will not change this.

2. When you insert new Toolbox parts in the same assembly, only the new Toolbox parts will be uploaded to the new collaborative space as In Work, as per your latest values in ToolBox settings.

3. You have the flexibility to move the previously uploaded Toolbox parts from Common Space to another collaborative space, e.g. as per the latest Collaborative Space value in ToolBox settings.

b) Toolbox Resources

As a platform administrator, you can deploy a specific Toolbox library database to all the SOLIDWORKS users accessing the same platform from different machines. This Toolbox option is available in the Resources section of the following page:

Collaborative Spaces Configuration Center > CAD Collaboration > SOLIDWORKS > Settings  

This additional setting is targeted for customized Toolbox libraries. If you use the default Toolbox library from SOLIDWORKS installation, you do not need to deploy this setting. 

To use this option, first package your Toolbox library database using the Toolbox Setup utility from SOLIDWORKS. To launch this utility, go to System Options > Hole Wizard/Toolbox, and click Configure. Or, from Design Library task pane tab, click Configure Toolbox. 

⚠️ Note: Before packaging your Toolbox library database, make sure to Save any customizations done to the library using the Toolbox Setup utility (see SolidPractices document ‘Setting up SOLIDWORKS Toolbox’ for details).   

To package your Toolbox library database -    

1. Go to section 6. 3DEXPERIENCE, and export the Toolbox library database as a zip file to a local folder using the Save command.   

2. After the save is successful, click OK and close the Toolbox Setup utility.

   

Once the Toolbox library database zip file is ready, go back to the Resources section on the platform, and click the Browse files button for the Toolbox option to locate the zip file from your local machine. 

Then click the Upload a Toolbox resource file (.zip) button to upload the file to the platform. 

Once successfully uploaded, Deploy Status updates accordingly. For a successfully uploaded Toolbox library database, 3DEXPERIENCE creates a corresponding XCADResource object, with Name attribute = SW-Toolbox-Database. 

⚠️ Important: Before packaging your Toolbox library database using the Toolbox Setup utility from SOLIDWORKS, make sure to choose a compatible collaborative space in your MySession Credentials. The content of the chosen collaborative space must be visible to all the users. 
 

By default, the Common Space collaborative space is compatible for this. If you choose a different collaborative space in your MySession Credentials, make sure to set its visibility to Public first before you package your Toolbox library database. 

After successfully uploading the Toolbox library database to 3DEXPERIENCE, search for XCADResource in 3DSearch, and make sure that the corresponding object is created in Common Space or in a Public collaborative space.

If the XCADResource object for your Toolbox library database gets created in an unintended / incompatible collaborative space, you can still correct it with either of the following actions:

1. Set the visibility of the collaborative space to Public.

Or,

2. Move the XCADResource object to the intended / compatible collaborative space using a web app, e.g. Collaborative Lifecycle. 

   

To remove a Toolbox library database file from 3DEXPERIENCE, simply delete the XCADResource object using a web app, e.g. Collaborative Lifecycle.

Users do not need to manually download a deployed Toolbox library database from 3DEXPERIENCE to SOLIDWORKS client computers. When each user launches SOLIDWORKS from the same platform, the Toolbox library database gets automatically downloaded to the following folder location on their machine, and gets synchronized with their SOLIDWORKS installation.

%LocalAppData%\\DassaultSystemes\\CATTemp\\ENOUSWC\\Resources\\[tenant ID]\\ToolboxDatabase

The manual download option is also available with the Download the current Toolbox resource file button.

4) Saving Existing Assemblies Referencing Toolbox Parts

a) From SOLIDWORKS Session

When you open an existing assembly that references a Toolbox part, regardless of the Toolbox User Settings originally used in SOLIDWORKS Design device-license version Toolbox Setup utility, the Create Parts option takes effect. Then saving the assembly to 3DEXPERIENCE from SOLIDWORKS session follows the process below:

When save to 3DEXPERIENCE is complete –

1. The Toolbox part status synchronizes with 3DEXPERIENCE, and MySession task pane tab displays the latest attributes, e.g. Maturity State, Collaborative Space etc.
2. Toolbox local cache folder contains the Toolbox part and its 3DEXPERIENCE cache files.  

For any reason, if MySession is not connected to 3DEXPERIENCE when you open an assembly in SOLIDWORKS, any referenced Toolbox parts will appear as File has not yet been saved into 3DEXPERIENCE.

After MySession connects to 3DEXPERIENCE, and then you save the assembly to 3DEXPERIENCE, the Save to 3DEXPERIENCE dialog box will show the Toolbox parts as already saved to the target collaborative space with Not modified status. The app uses the original process for new or existing Toolbox parts to establish this status. This completes the client-server synchronization for those Toolbox parts, even if you cancel the assembly save at this point.  

b) Using Batch Save

When saving SOLIDWORKS assemblies to 3DEXPERIENCE using the Batch Save to 3DEXPERIENCE tool, follow the guidelines documented in the SolidPractices guide Moving SOLIDWORKS Files to the 3DEXPERIENCE Platform. 

Batch Save to 3DEXPERIENCE tool does not work the same way as saving to 3DEXPERIENCE from an active SOLIDWORKS session. It is important that you complete the file preparation correctly before using this tool.    

For an existing local assembly that references a Toolbox part, the Batch Save to 3DEXPERIENCE tool follows the process below: 

(1) Toolbox part inserted into assembly using SOLIDWORKS Design device-license version without the Design with SOLIDWORKS app installed, and with the Create Configurations option in Toolbox Setup utility.

(2)  Assembly packaged using Pack and Go, and with the Include Toolbox components option activated. 

(3) Toolbox part inserted into assembly using SOLIDWORKS Design device-license version with the Design with SOLIDWORKS app installed, or using SOLIDWORKS Design user-license app.  

If the Toolbox part referenced in your assembly does not already exist on 3DEXPERIENCE, follow the recommendations below for scenarios (1) and (2) from the process chart:

(1) After using Batch Save to 3DEXPERIENCE, open the assembly in SOLIDWORKS from 3DEXPERIENCE, and save back to 3DEXPERIENCE.

(2) Do not activate the Include Toolbox components option if you package the assembly using Pack and Go. If you have already done so, do not save the Pack and Go folder using Batch Save to 3DEXPERIENCE. Instead, package a new Pack and Go folder without the Include Toolbox components option activated, then save the new folder using Batch Save to 3DEXPERIENCE.     

⚠️ Note: Using Batch Save to 3DEXPERIENCE, if you by mistake save a local assembly folder that also includes its referenced Toolbox parts, follow the steps below to rectify the assembly structure on 3DEXPERIENCE:

1. Delete the assembly file set including Toolbox parts from the 3DEXPERIENCE files on This PC tab of the task pane (MySession local cache).

2. Open the assembly from 3DEXPERIENCE, Lock it and save it back.

3. Search for and delete the unwanted duplicates of Toolbox parts from 3DEXPERIENCE, that have been created as a result of the unsupported workflow. 

5) Inserting Toolbox Parts

To insert Toolbox parts into an assembly, use the Design Library task pane tab to drag and drop from the Toolbox folder. This is the only supported workflow. 

Do not use any other workflows (e.g. Insert Components command).

When you insert a Toolbox part into an assembly from the Design Library task pane tab, the system follows the same process described in section 4)a).

6) Toolbox Physical Product Characteristics

a) Maturity State

With the appropriate credentials, the platform administrator can change the maturity state of existing Toolbox Physical Products as per the Maturity Graph applied for Engineering Definition.

For more details on this, see the following topics in 3DEXPERIENCE User Assistance guide: 

1. Collaborative > Structured Collaboration & Collaborative Content > Collaborative Lifecycle Web App > Changing the Maturity of Objects

• Installation and Setup > 3DEXPERIENCE Platform > 3DEXPERIENCE Platform Administration > 3DSpace > Collaborative Spaces Control Center > Configuring Content for the 3DEXPERIENCE Platform > Configuring Maturity Graphs.

The platform administrator can also use the Default · Administrator credentials for this.
 

b) Enterprise Item Number

You can assign Enterprise Item Numbers (EIN) to Toolbox Physical Products that are in In Work maturity state.

You can also customize your assembly Tree Display to show EIN as the Primary name for the components. 

 The Primary name also appears in the Component Name column of MySession.

⚠️ Note: The Primary name from assembly Tree Display does not affect the Physical Product title.

The platform administrator can also deploy the Copy Enterprise Item Number to Title of a Product rule for all Physical Product. This rule is listed in –

Collaborative Spaces Configuration Center > Engineering Definition > Enterprise Item Number : Admin Configuration. 

With this rule deployed to 3DEXPERIENCE, when you add an EIN to a Toolbox Physical Product, or edit an existing EIN, the EIN appears as the Physical Product’s title. Refresh MySession to update the Title column.   

⚠️ Note:

(i) This only applies to EINs added or edited after the rule is deployed.

(ii) If you then Clear the EIN value from a Physical Product, it still retains the copied EIN as its title, until you manually change the title.

c) Local Modification

After you save a Toolbox part to 3DEXPERIENCE for the first time, you can no longer save any local modifications to it from SOLIDWORKS back to 3DEXPERIENCE. This includes adding, removing, or modifying any Custom or Configuration Properties, or performing any SOLIDWORKS commands that trigger a local modification.

After you insert a new Toolbox part into an assembly from the Design Library task pane, you can open it in a separate window using the Open Part command from the assembly design tree. This opens the part file from the Toolbox local cache folder. You can then add, remove, or modify this part’s Custom or Configuration Properties, and save it back locally to the Toolbox local cache folder. Saving the assembly to 3DEXPERIENCE then also saves those Toolbox local modifications. These operations are only supported for a new Toolbox part that has not yet been saved to 3DEXPERIENCE. 
 

d) Delete

You can delete existing Toolbox parts from a collaborative space. 

1. If a Toolbox part maturity state is In Work, you can delete it as the Leader of the collaborative space.
2. If it is in Released maturity state, the platform administrator can delete it with the Default · Administrator credentials. Alternatively, they can demote the maturity state to In Work first, and then a Leader of the collaborative space can delete it.   

For more details on delete permissions with different responsibilities, see the following topic in 3DEXPERIENCE User Assistance guide: 

3DEXPERIENCE > 3DEXPERIENCE Platform > Collaborating in 3DEXPERIENCE > Controlling Access to Content in Collaborative Spaces > Baseline Responsibilities. 

Note: For Toolbox parts, changing the maturity state, moving to a different collaborative space, or deleting those affect all the users accessing the same platform. Only a designated Toolbox administrator should perform these activities when necessary, and with caution.

7) Attribute Mapping for Toolbox Physical Product

When deploying attribute mapping, follow the guidelines documented in the SolidPractices guide Attribute Mapping for SOLIDWORKS®.
 

a) CAD Attribute to Product Attribute Mapping

For Toolbox Physical Products, CAD attribute (SOLIDWORKS) to Product attribute (3DEXPERIENCE) mapping is available to new parts only, i.e. you can add or modify an attribute in SOLIDWORKS Configuration Properties only before a Toolbox part is saved to 3DEXPERIENCE for the first time [see section 6)c)]. 

You can follow any of the methods below to add or modify an attribute in Toolbox part Configuration Properties before saving to 3DEXPERIENCE for the first time with an assembly.

(1) From a SOLIDWORKS session:

1. Insert a new Toolbox part into an assembly from the Design Library task pane. 
2. Open the Toolbox part in a separate window using the Open Part command from the assembly design tree (the part opens from Toolbox local cache folder). 

3. Add the attribute in Toolbox part Configuration Properties. 

4. Save the Toolbox part locally back to Toolbox local cache folder. 

5. Save the assembly to 3DEXPERIENCE.

(2) From Toolbox library:

1. Launch Toolbox Setup utility.
2. In tab 2 - Customize Hardware, select the Toolbox Standards as needed. 
3. In the Custom Properties panel, click Add new Custom Property.

4. In the Custom Properties Definition dialog box, add the attribute title in the Name field with the following settings – 
   • Check the box for Add as configuration specific property 
   • Check the box for Show in PropertyManager
   • Property Type = Textbox
   • Overall default value = The attribute value.

5. In the Custom Properties panel, check the box for the added attribute value to Apply Custom Property to current tree selection.
6. Click Save and close Toolbox Setup utility.

7. Insert a new Toolbox part into an assembly from the Design Library task pane tab.

8. Save the assembly to 3DEXPERIENCE.

See SolidPractices document Setting up SOLIDWORKS Toolbox for more details on how to configure / customize a Toolbox library. 

b) Product Attribute to CAD Attribute Mapping

For a Product attribute to CAD attribute mapping deployed on 3DEXPERIENCE, you can add the attribute to a Toolbox part Configuration Properties from a SOLIDWORKS session, before saving it to 3DEXPERIENCE for the first time. For this, follow the method below.

1. Insert a new Toolbox part into an assembly from the Design Library task pane.
2. Open the Toolbox part in a separate window using the Open Part command from the assembly design tree (the part opens from Toolbox local cache folder). 
3. Add the deployed attribute to the Toolbox part Configuration Properties, from the ----PLM Attributes---- list in the Property Name drop down menu. 

4. Save the Toolbox part locally back to Toolbox local cache folder.

5. Save the assembly to 3DEXPERIENCE.

   

You can add or modify this attribute value only from the Physical Product Properties, with the appropriate credentials used in the editing app (e.g. Side Panel accessed from MySession Action Bar). For example, as Leader of the target collaborative space for Toolbox parts, you cannot add or modify this attribute value if the Physical Product is in Released state. But, as Owner the collaborative space, you can.   

This is governed by the same rules for authoring content in collaborative spaces, described in 3DEXPERIENCE User Assistance guide - Baseline Responsibilities.

After you add or modify the attribute value in the Physical Product Properties, the mapped value appears in the Toolbox part Configuration Properties without triggering any local modifications.

8) Opening Toolbox Parts

• As mentioned in section 2)c), when you open an assembly referencing Toolbox parts, the Toolbox part files are either created or downloaded to the Toolbox local cache folder. Toolbox management using 3DEXPERIENCE does not support Toolbox parts referencing from your local work folder (MySession local cache).
   
• You can search for Toolbox parts using 3DSearch. However, the Open or drag operations into an assembly, or as a part, from 3DSearch results are not supported. These will return the following message:

You can insert Toolbox parts into an assembly only from the Design Library task pane tab, even if those are already saved to 3DEXPERIENCE.

• Toolbox management on 3DEXPERIENCE only works from an assembly environment, see section 2)a). If you open a Toolbox part on its own using the drag operation from the Design Library task pane tab, it opens from the local Toolbox library location without following the Create Parts rule. This workflow is not supported for Toolbox management on 3DEXPERIENCE. Do not save a Toolbox part to 3DEXPERIENCE on its own as an individual part.

9) Assemblies Last Saved Before R2021x FD04

You may have existing assemblies referencing older version Toolbox parts that were last saved to 3DEXPERIENCE before R2021x FD04. Simply open those assemblies in SOLIDWORKS, and save back to 3DEXPERIENCE. The app maintains the Where used references of the Toolbox parts.

10) Additional Recommendations

• If you install the Design with SOLIDWORKS app, do not disable the following option in SOLIDWORKS Design device-license version:

  System Options > Hole Wizard/Toolbox > Make this folder the default search location for Toolbox components. 
  
  In SOLIDWORKS Design user-license apps (that include the Toolbox add-in), this option is active by default and cannot be disabled. 

• Do not attempt to revise Toolbox parts - it is not supported.

• Do not create duplicates of Toolbox Physical Products using a web app (e.g. Collaborative Lifecycle) as those duplicates are not supported for Toolbox management on 3DEXPERIENCE. When you drag and drop a duplicate of a Toolbox Physical Product from 3DSearch into a SOLIDWORKS assembly, the part is downloaded to your local work folder (MySession local cache) instead of the Toolbox local cache folder.

   

11) FAQs

Q.1. Can I add the default PLM attributes (e.g. Maturity State, Rev etc.) to Toolbox part Configuration Properties?
Answer: Yes, although not necessary. And, only before saving a Toolbox part to 3DEXPERIENCE for the first time. Same method from section 7)b) applies.

Q.2. Is it possible to add default PLM attributes to local Toolbox library database using the Toolbox Setup utility?
Answer: Yes, and only before saving a Toolbox part to 3DEXPERIENCE for the first time. See From Toolbox library. In the Custom Properties Definition dialog box, add the Property Name value (e.g. Enterprise Item Number) to the Name field, and the Value / Text Expression syntax (e.g. \\\$PLMPRP:"EnterpriseExtension.V_PartNumber") to the Overall default value field.    

Q.3. Is it possible to apply the Auto-name setting from the platform to Toolbox parts?
Answer: No. The Auto-name setting does not apply to SOLIDWORKS Toolbox parts. 

Q.4. Is it possible to assign user defined titles to Toolbox parts? 
Answer: Yes, from the File Name: field in the Configure Component PropertyManager when you insert a new Toolbox part into an assembly. By default, this field populates a value based on properties such as standard, specification, type, size, length etc. You can modify this value before clicking OK. Use this only for new Toolbox parts, before saving first time to 3DEXPERIENCE. 

Q.5. Can I modify the title attribute of Toolbox Physical Products using web apps?
Answer: Yes, using compatible web apps, e.g. Collaborative Lifecyle. This is governed by Baseline Responsibilities for authoring content, see sections 6)d) and 7)b). Make sure to delete existing files from Toolbox local cache folder before opening any assemblies, that reference those Toolbox parts, from 3DEXPERIENCE.

Q.6. Why can I not change maturity state or modify custom attribute values of some old Toolbox parts that I saved to 3DEXPERIENCE in the past?
Answer: These enhanced capabilities were released in 3DEXPERIENCE R2023x FD01 (February 2023). Any Toolbox parts saved to 3DEXPERIENCE before this do not support these enhanced capabilities. 

Q.7. With major version upgrades to SOLIDWORKS Design, how do I upgrade versions of existing Toolbox parts on 3DEXPERIENCE? 
Answer: There is no need to upgrade versions of existing Toolbox parts on 3DEXPERIENCE. If you need to upgrade versions of the referenced assembly files, simply open those from 3DEXPERIENCE and save back. This does not affect the referenced Toolbox parts.

Your Feedback Requested
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.​​​​​​​​​​​​​​