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:
- How to sketch and model the duct part (this post)
- How to separate into different separate bodies,
- How to save out the individual bodies and convert into sheet metal
- And finally, how to edit the parts to get a nice material-yield-friendly laser/plasma cut.
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.
- 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
- Then I will add my material of ASTM A36.
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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