Problem

External references are a key benefit of designing assemblies in SOLIDWORKS. Understanding them and their options can improve efficiency and reduce frustration. This article explains how to access external references and their statuses. In top-down design, part features are created from assembly geometry. External references track the relationship between the part and assembly. When an in-context reference exists, changes to the referenced geometry update the dependent document.

An external reference is indicated by the arrow -> symbol next to a feature or file name in the FeatureManager design tree. An example is shown below.

In this case, the part has a Cut Extrude with an external reference to an assembly file. 

Accessing External References

To access External References, right-click on the feature or file name with an external reference symbol -> and select "External References" to bring up the External References window.

An example of the External References window can be seen below. 

The External References window includes columns for Feature Name, Status, Referenced Entity, and Type. Feature Name lists in-context items, such as sketches and features, in the selected part. Referenced Entity identifies the referenced item and the document containing it. If the item is in another assembly component, Feature’s Component shows the component containing the affected feature. Type describes the type of data used to create the reference, such as a converted edge, face, sketch entity, or body.

External Reference Statuses 

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 indicates that the feature is not solved or up to date because the update path is not available. An out-of-context reference is followed by an arrow with a question mark symbol 
->? 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. The dangling reference is similar to an out-of-context symbol but is yellow, as shown below.

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.

For information on Breaking or Locking External References, review these articles:

How to Break External References in SOLIDWORKS

How to Lock External References in SOLIDWORKS

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.