External references are one of the benefits of using assemblies to design in SOLIDWORKS. Understanding them and the available options will improve efficiency and reduce frustration. This article describes the definitions and options available for external references.
In a top-down design, where a part’s features are created using geometry in an assembly external references are created in order to track the dependency or linkage of the part and assembly’s geometries. Changes made to the geometry of a referenced document will update and change the geometry in the dependent document, if the external reference is in-context.
An external reference can be recognized if your part file or subassembly file includes the symbol -> next to the features or file names in the feature manager tree. An example of this behavior can be seen below.
In this particular case Part A has an external reference in Sketch4 to an assembly file. To view, lock, unlock, or break a file’s external references, right click on a feature or file name with an external reference symbol ->, and select List External Refs…, which brings up the External References For dialog box.
An example of the External References For dialog box can be seen below.
Locking external references on a component prevents the existing references from updating and new references cannot be added to the component. If an external reference is locked, the feature name or part name will be followed by ->*. The following image is an example of a part’s feature manager tree with locked external references.
Once external references are broken, the external references cannot be restored, which means the references are forever broken. Breaking external references on a component prevents the existing references from updating, but new references can be added to the component. If an external reference is broken, the feature name or part name will be followed by ->x in the feature manager tree. An example of an external reference icon can be seen below.
The External References For dialog box also shows columns for the Feature, Data, Status, Referenced Entity, and Feature’s Component of the External References. The Feature lists each in-context item, such as sketches and features, in the selected part. The Data describes the type of data used to create the item, such as a converting an edge/face, or offsetting a sketch entity, and so on. The Referenced Entity defines the actual item being used, and the name of the document that contains the item. If the Referenced Entity is located in a different component in an assembly, the Feature’s Component of the External References column shows the name of the component in which the affected feature exists.
There are several statuses that are available for an External Reference. An in context status shows the feature is solved and up to date. An out of context status describes the feature is not solved or up to date because the update path is not available. An out of context reference is followed by ->? in the feature manager tree. An example of an out of context reference icon in a feature manager tree can be seen below.
The out of context reference can be solved and updated by opening the assembly that contains the update path. A dangling status describes a situation where the referenced entity has been changed such that the reference is invalidated. An example of a dangling external reference can be seen, when an extrusion to a surface is made and that surface is deleted from the referenced component.
There are some exceptions for External References. For instance, a component cannot have an external reference to itself. Also, one instance of a part cannot be used to reference a feature on another instance of the same part, even if instances are in different configurations. Furthermore, a part cannot be replaced with another part created by deriving the second part from the first.