External References Options

You can specify options to open and manage part, assembly, and drawing files that have external references.

To open this dialog box:

Click Options or Tools > Options and click External References.

Reset Restores factory defaults for all system options or only for options on this page.
Open referenced documents with read-only access Specifies that all referenced documents open for read-only access by default.
Don’t prompt to save read-only referenced documents (discard changes) Specifies that when you save or close a parent document, you are not prompted to save the read-only, referenced documents.
Allow multiple contexts for parts when editing in assembly Allows the creation of external references to a single part from more than one assembly context. However, any individual feature or sketch within the assembly may only have one external reference.
Load referenced documents Specifies whether to load the referenced documents when you open a document with external references.

Prompt

Asks about loading externally referenced documents each time you open a document with external references.

All

Loads all of the externally referenced documents.

None

Does not load the externally referenced documents. External references may show as out-of-context until you open the externally referenced documents.

Changed Only

Loads only the externally referenced documents that changed since the last time that you opened the original document.
When you select All, None, or Changed Only, a message is added to the dismissed messages list.

To view the dismissed message, click Tools > Options and click Messages/Errors/Warnings. Under Dismissed messages, you see the One or more features in this part are based on other documents. If those... message.

If you check the message to show it again, Load referenced documents changes to Prompt. You must reopen system options to see the change.

Load documents in memory only Loads referenced documents in memory only, rather than opening the documents in separate windows. You can keep references up-to-date without opening windows for the documents. Use this option when you open an assembly containing many component parts that have external references.

Available when you select Prompt, All, or Changed Only for Load referenced documents.

Search external references in

Reference Documents specified in File Location Searches for missing referenced documents in the Referenced Documents folders specified in System Options > File Locations.
Otherwise, the standard recursive search routine is used.
Include sub-folders Searches subfolders of the Referenced Documents folders.
Exclude active folders and recent save locations Blocks the software from searching open folders and folders where you recently saved items.
Go To Reference Documents Opens the System Options - File Locations dialog box.
Update out-of-date linked design tables to Determines what happens to linked values and parameters if the model and the design table are out-of-sync.

Prompt

Asks about updating values between the design table and the model.

Model

Updates the design table with the values from the model.

Excel File

Updates the model with the values from the design table.
When you select Model or Excel File, a message is added to the dismissed messages list.

To view the dismissed message, click Tools > Options and click Messages/Errors/Warnings. Under Dismissed messages, you see the Document contains an externally linked design table that has changed... message.

If you check the message to show it again, Update out-of-date linked design tables to changes to Prompt. You must reopen system options to see the change.

Assemblies

Automatically generate names for referenced geometry

Automatically creates surface identifiers when you mate parts, which usually requires write access to the parts. Use this option when you replace components using the same surface identifiers, remembering that you need write access to the parts that you use. You can rename the corresponding edges and faces on the replacement component to match the edge and face names on the original part. Update out-of-date linked design tables to

Unless you use component replacement, leave this option off, especially in a multi-user environment.

When you clear this option, you can mate to parts for which you have read-only access because the internal face IDs of the parts are used.

Update component names when documents are replaced Clear this option only if you use the Component Properties dialog box to assign a component name in the FeatureManager design tree that is different from the file name of the component.
Allow creation of references external to the model Permits the creation of external references when designing in the context of an assembly.
Reference Component Type

Any Component

Creates an external reference to any component.

Only Envelope Component

Creates an external reference only to envelope components.
In the context of

Top level assembly

Creates an external reference to components in the top-level assembly.

Same subassembly

Creates external references only to components in the same subassembly.

Show "x" in feature tree for broken external references Flags items that have broken external references with an indicator (x) in the FeatureManager design tree.
Force referenced document to save to current major version For assemblies and drawings, saves the model and all references in the current version of the SOLIDWORKS software.

When you clear this option, only modified documents save in the current version.