How to Use Assembly Feature Propagation in SOLIDWORKS
SolidProfessor - Sam Sanchez | April 13, 2016 | Comment
When working in SOLIDWORKS, it is important to keep your design intent in mind when adding features to your models. SOLIDWORKS lets you add features to your models at both the part and assembly levels using assembly feature propagation.
In the video tutorial above, we have a mount part, which is part of a major assembly. The part requires holes in the tabs of its brackets to allow other components to be attached to it.
We could add an extruded cut, however none of the other parts in the assembly will share that hole.
Since this hole feature we need will affect more features than just the mount, we can save time and incorporate better design intent by creating the extruded cut as an assembly feature instead.
In the assembly, we can sketch a circle and then add dimensions and relations to fully define the sketch on the face depicted below.
We can exit the sketch and then launch the extruded cut assembly feature from the “Assembly Features” dropdown menu on the command manager.
We will make this a “Through All” cut and select “All components,” under “Featured Scope” to cut through all components. When I click the green checkmark, you can see the results.
Although this looks like what we wanted in the assembly, there is no cut in the part file. This is because the feature was added at the assembly level and not the part level. In fact, none of the parts contain the cut.
Using Assembly Feature Propagation Between Parts and Assemblies
This could cause some problems down the line; say someone sent one of these parts in an email to a supplier to get a quote and the part didn’t contain the cutout.
To fix this, we must go back to the assembly and edit the cut extrude feature. Notice that in the feature scope there’s an option to propagate the feature to parts.
We’ll check the box to activate it and click the green checkmark.
In the assembly it looks like nothing has changed, but now when we open one of the parts, we can see the cut extrude feature has been added there as well.
Notice the files now contain external references, indicated by the arrow.
The cut extrude feature at the part level is now parametrically linked to the feature that was created in the assembly. If we change the dimension on the assembly, it updates at the part level as well.
The option to propagate to the part is also available for other assembly features, such as fillets.
You can learn more about the new capabilities in SOLIDWORKS 2016 by signing up for a free membership.
About the Author
Sam Sanchez is an Applications Engineer with SolidProfessor and a CSWP. Sanchez is an alumni of UC San Diego, and in her free time enjoys 3D printing and hanging out with her dog Ruby. You can see more training videos on a wide range of CAD, CAM & BIM topics at www.solidprofessor.com.
- 3D Shape Basics in Fusion 360
- Fusion 360 Sketch Basics
- Running a Parametric Study and Analysis in SOLIDWORKS to Create a Flow Simulation Project
- Calculating External Flow around a Sphere in SOLIDWORKS
- How to Add Heat Sources in SOLIDWORKS
- Working with Macros in SOLIDWORKS Electrical
- Creating Locations in SOLIDWORKS Electrical
- Linking Sketch Blocks in SOLIDWORKS
- Inserting Fluid Subdomains in SOLIDWORKS
- Inserting a Porous Region and Running an Analysis in SOLIDWORKS