When working with an assembly that utilizes the SOLIDWORKS top down assembly design approach it is good practice to lock the external references for a design that is ready for release.
This will help to ensure the design does not change unless the external references are unlocked first. Locking external references will also increase rebuild performance of an assembly. This is because SOLIDWORKS needs to keep track of any references applied in the assembly and if a rebuild is applied to a part that is referenced by other parts this will in turn cause the referenced parts to rebuild.
In this tech tip I will show you how to lock an external reference in this simple garden light design:
What is an External Reference?
External references are created when a part is built while in the assembly environment. Using existing geometry of another part to help create a new part will generate an external reference, for instance a sketch entity could be created by offsetting an edge of an existing part, or a feature is extruded up to an existing part’s face as shown in the image below:
Parts that have external references are denoted within the FeatureManager Design Tree with the ‘->’ symbol as shown in the figure below. The feature that was created with the reference and the overall part icon will both display the symbol. A part may also have multiple features with external references.
How to Lock an External Reference
- Open your top down assembly document that contains parts with external references.
- To lock an external reference Right-click on the Part (or Feature in a Part document) with the external reference (denoted by the ‘->’ suffix in the FeatureManager Design Tree).
- Select External References from the shortcut menu.
- In the related dialog box the external references will be listed for each feature of the component, in this example an Extrude feature is present as shown in the figure below.
- To lock the external references pick the Lock All button in the dialog.
- SOLIDWORKS will warn you that you will not be able to modify the reference in the part while it is locked, pick OK on the dialog.
- The part (or feature) will now be listed as locked in the dialog. Select OK to close the dialog.
- In the Assembly FeatureManager Design Tree a locked symbol ‘->*’ will now be displayed as a suffix of the part name to denote that the reference is locked. If you need to add more references to the part you can unlock it using the same procedure.
Learn more about SOLIDWORKS Assemblies
Attend our live online SOLIDWORKS Assembly Modeling training course to learn more about external references and working more productively.
Get Certified SOLIDWORKS Services from Javelin
Javelin Experts can help you to: