Designing 90° Sheet Metal HVAC Duct in SOLIDWORKS – Part 2 of 4

Article by James Swackhammer, last updated on January 20, 2019

Welcome to Designing 90° Sheet Metal HVAC Duct in SOLIDWORKS – Part 2. In the previous part we had created the basic model for the duct, the required sizes are set with a basic sketch, and a circular profile sweep was used to create the model. In this second part we’re going to cut a small slit, for future reasons, and then split the part into 7 individual bodies.

PART 2: How to split the part into separate bodies

Let’s jump into this head first:

  • Start a sketch on the top plane. Here I’m going to convert the first sketch’s construction arc and then join the points together to form a full circle.
  • With the sketch still open, I’m going to do a mid-plane cut extrude 0.005″. This puts the much needed slit in for the conversion into sheet metal, which will be shown in a later article.
  • I converted the arc for design intent, now when I change the size of the duct, the extrude cut will change along with it.
Applying a circular cut for sheet metal flattening

Applying a circular cut for sheet metal flattening

  • This next sketch is a little more complex but first, I need to create a different plane. I pre-select the top plane and went to “Reference Plane” to add in a new plane.
  • My second reference is the face of the inlet. My reference plane snapped to the perpendicular relation, so I changed it to parallel because I want to sketch above, but have this plane linked to the size.
Adding a reference plane

Adding a reference plane

With the new plane created I will now start my sketch:

  • What I like to do once I start my sketch is hid the plane. Again, I’m going to use my first sketch and reuse geometry.
  • I bilaterally offset the lines that are not construction lines past the geometry in both directions.
  • Next, I do a Ctrl + A to select all and make those construction lines.
  • I can now connect each points with a regular line.
Creating split lines

Creating split lines

Now that we have this sketch completed we can move into our “Split” command. This is located under the “Direct Editing” tab, or you can use the search bar to locate it. The “Split” command will take our single body part and split into the amount of bodies we want. The amount of bodies depends on the sketch we create and the selections we select.

  • With the sketch pre-selected I will click “Split”, I will also select the duct body from the graphics area.
  • I can now click the “Cut Part” button. Just below that I will select all 7 parts and click “Auto Assign Names” and accept the command.
Split Body

Split Body

You’ll notice that I now have 7 different bodies in the bodies box. Each can now be modified individually or saved out. Follow this series to the next article where we save out the parts and convert to sheet metal.

Subscribe to our blog for the next article to learn how to save the bodies and convert them into the desired thickness of sheet metal gauge.

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James Swackhammer

James is a SOLIDWORKS Technical Support Application Expert based in the Javelin Oakville head office

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