Prevent External References Between Components in an Assembly

External references, also known as in-context references, are created when a SOLIDWORKS sketch or feature utilizes reference geometry outside of the part that it was created within. This can help define the design intent while allowing for flexibility if and when models need updating. A common use case for this is lining up fastener hole positions from one component to another. In this case, if the hole positions on the “original” part are updated, the hole positions on the dependent component will reflect the change too.

However, sometimes the creation of external references can become a burden when there are too many interconnected references spanning across numerous parts in a large assembly. In assemblies with hundreds or thousands of components, external references can be hard to keep track of and may lead to performance degradation. Keep reading to learn how to prevent in-context references.

Using No External References Mode

When editing a part inside of an assembly, there is an option in the upper left corner of the interface called No External References. When this option is selected and is shown as dark grey, any actions that would otherwise generate permanent in-context references are treated like a one-time copy. Ultimately, any external reference that would be created is automatically broken.

Activating No External References mode

Creating Hole Wizard Holes Without External References

In the screenshot below, the Cover component needs holes added that will line up with the existing Guard component in the assembly. When editing the Cover part in the context of the assembly, the Hole Wizard hole positions can be placed at the center of the existing holes on the Guard part. After applying the Hole Wizard feature, the holes line up perfectly.

Creating Hole Wizard holes with the No External References option

Investigating Other Affected Components

Let’s look inside the Cover part in its own window. In the image below, we can see the Hole Wizard sketch that was just created. Remember that while the sketch points currently line up with the holes, they are not permanently locked.

From this point on, if the original Guard component design is modified, resulting in the hole locations moving, these points will not update. Additionally, the sketch points being blue tells us that they are underdefined. This means I could easily drag and drop and move these points accidentally, and the original alignment would be lost.

Undefined sketch points in the Cover part

Fully Defining the Incomplete References

At this point, it is a good idea to use Fully Define Sketch to define the hole positions numerically, as shown below. Fully Define Sketch assigns dimensions and relations to any sketch entities that are underdefined. After running the command, their positions are locked in place so they can’t be accidentally moved. The important distinction here is that these sketch entities are no longer connected externally to the Guard component and will not update when changes are made there.

Fully defining the sketch

Other Uses for No External References

Following a similar workflow, you could use No External Reference mode with commands like Convert Entities or Offset Entities to create one-time transfers or copies of geometry from one part to another within an assembly, while avoiding permanent external reference links between the files.

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