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External References Options

Specifies how part, assembly, and drawing files with external references are opened and managed.

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 will be opened for read-only access by default.
Don’t prompt to save read-only referenced documents (discard changes) Specifies that when a parent document is saved or closed, no attempt will be made to save its read-only, referenced documents.
Allow multiple contexts for parts when editing in assembly You can create 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 part that is derived from another document (such as a base part, derived component part, part with a cavity feature, and so on.)

Prompt

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

All

Opens all of the externally referenced documents.

None

Does not open any of the externally referenced documents. External references may be shown as out of context until you open the externally referenced documents.

Changed Only

Opens only the externally referenced documents that have changed since the last time you opened the original document.
Search file locations for external references Specifies that SOLIDWORKS should search the Referenced Documents list of folders in Tools > Options > File Locations. When cleared, the list is ignored.
Update out-of-date linked design tables to Determines what happens to linked values and parameters if the model and the design table are out-of-sync.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

The software prompts you when you open a document with a design table that is out-of-sync with the model.

Model

The design table updates with the model's values.

Excel File

The model updates with the design table's values.

Assemblies

Automatically generate names for referenced geometry When this option is off, you can mate to parts for which you have read-only access because you are using the internal face IDs of the parts. Unless you will use component replacement, leave this option off, especially in a multi-user environment.

When this option is on, you automatically create surface identifiers (for example: Face1, Face2) at the time you mate the part, therefore you need write access to the part, in most cases. Turn this option on if you intend to do component replacement using the same surface identifiers, remembering that you need write access to the parts you are using. (Rename the corresponding edges and/or faces on the replacement component to match the edge/face names on the original part.)
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 filename of the component.
Do not create references external to the model Select this option to not create external references when designing in the context of an assembly. No in-place mate is created when you create a new component. Also, external references are not created when you reference the geometry of other components, such as when you use Convert Entities or Offset Entities, or extrude Up to Vertex of another component.
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. Clear this option if you want to hide the indicators (x).


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Web Help Content Version: SOLIDWORKS 2016 SP05

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