Trouble with the Curve? Not Anymore! How to Drive your SolidWorks Assembly Pattern with a Curve.
Have you ever experienced that SolidWorks moment when you’d like to see a part feature available in an assembly? Patterning is one such wish I’ve had and recently revisited when a customer asked me about creating a Curve Driven Pattern in an assembly.
Now, some users may spout off a quick ‘No’ to such a question, but those of us that spend our 20 hours of screen time per day torn between the rigors of supreme CAD functions and Call of Duty while consuming excessive amounts of energy drinks and cold pizza may have found a beacon of hope in the Feature Driven Component Pattern command.
So how does one achieve such magnificence in their SolidWorks Assembly? Well, to be honest, it does require a little massaging from an underlying Part level Curve Driven Pattern Feature, but there are multiple ways this could be tackled.
Let’s use this conveyor example to show a few options. In this example, I want to pattern a Sub-Assembly that contains the leg and a foot plate part. My goal is to use a curve to pattern this Sub-Assembly around the curved conveyor rail within this Top Level Assembly.
Exhibit A: Curve Driven Pattern in the Curved Rail part.
One way to do this is to create a Curve Driven Pattern in the Rail part. This can be something that may really exist in the part or may be a dummy feature that we fill in later using the power of feature order. Here I’ve established a curve for my pattern associated to the curved rail, and patterned a simple hole. Think of it as: wherever there is a hole, there will be a leg assembly aligned to that hole. Now if you don’t need a hole in the rail, you could follow the Curve Driven Pattern feature up with some type of feature that will remove or fill in the holes (Extrude-Boss, Delete Face, etc.).
Back to the main assembly. Use the Feature Driven Component Pattern command to pattern the Sub-Assembly and your driving feature is the Curve Pattern from the Rail Part. Done!
Exhibit B: Curve Driven Pattern in the Leg Part. Similar to exhibit A, here we are going to pattern the leg along a curve. In the leg part, capture the curve needed as a sketch (you may want to edit in context and Convert Entities from the Rail part or use a sketch you’ve drawn at the assembly level). Now use that sketch in the leg part to do a Curve Driven Pattern of the body. Again, we probably don’t want the actual body instances left in the leg model, so you could follow that pattern feature with a Delete Bodies Feature that will remove all the instances created from the pattern.
Again, back to the main assembly. Feature Driven Component Pattern the Sub-Assembly needed and use the Curve Pattern from the Leg part as your driving feature. Done!
More flavors of these methods could be used as well. You could also use this for other patterns not available like Fill, Sketch, and Table.
I hope this was helpful, but if you’re still thoroughly confused due to a buzz from your favorite energy drink, you can check out this little video I put together showing Exhibits A and B. Enjoy!
***
Brian VanderPloeg is an Applications Engineer at Fisher/Unitech, a SolidWorks Value Added Reseller with locations across the Midwestern and Northeastern United States. He is a regular contributor to the Fisher/Unitech blog.
Want to try out SolidWorks? You can request a free SolidWorks trial on our website.
Want to see how SolidWorks can help you win new business and get to market faster? Request a SolidWorks demo today.
Fisher Unitech is improving manufacturing in America by delivering, supporting and training customers on the best product development software and additive and subtractive manufacturing solutions available. The company delivers 3D software and hardware, which enable customers to design, validate and manage innovative products from prototyping to manufacturing. With more than 17 office locations throughout the Midwest, Mid-Atlantic, and New England. For more information, visit www. FisherUnitech.com.