Designing a 90° Sheet Metal HVAC Duct in SOLIDWORKS – Part 1 of 4

Article by James Swackhammer updated January 28, 2019


Designing and manufacturing a duct for a ventilation system is easy, right?

With this series I’m going to start with simple, but most commonly asked for in a HVAC system design, the 90° bend:

I’m going to break down the SOLIDWORKS creation process into these 4 parts:

  1. How to sketch and model the duct part (this post)
  2. How to separate into different separate bodies,
  3. How to save out the individual bodies and convert into sheet metal
  4. And finally, how to edit the parts to get a nice material-yield-friendly laser/plasma cut.

90 Degree Bends

PART 1: How to sketch and model the duct part

Starting with the basics and keeping the size simple, I’m going to make a large 48″ diameter duct, 96″ span in a 90° bend. I want  to have 7 individual parts that will be welded together after they have been laser cut and rolled (on the rolling machine).

  • On the top plane I will start my first sketch using the “3 Point Arc” start on the origin to create a quarter of a circle.
  • Starting with the end points I’m going to add a horizontal relation to one and a vertical to the other.
  • Next, I will draw my vertical line and horizontal line, making them equal with a dimension of 18″. This is my inlet and outlet.
  • Lastly, to fully define the sketch I will add in my dimension of 96″ from the lines I just created.
Duct Sketch

Duct Sketch

  • Here’s the tricky part- I will now change the arc into a construction line. I want to add 5 equal lines using the arc as a reference. Make sure that the end points of the 5 lines are coincident with the arc.
  • I will now use the “Swept Boss/Base” feature to sweep a 48″ circular profile along that path.
    • I’m going to use the thin feature to add in my thickness of 0.0359″ for 20 gauge material
Swept Boss/Base feature

Swept Boss/Base Thin Feature

  • Then I will add my material of ASTM A36.
Completed Duct Model

Completed Duct Model

We now have a duct that looks the part, so if you’re only doing a plant layout or just need a pretty picture, you can stop here.

Subscribe to our blog for the next article where we cut this model into usable parts.

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James Swackhammer

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