1.5: Midterm Project - Advanced Solid Modeling

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Introduction

An HVAC duct is used to circulate air in a building. This module shows the steps to create an HVAC duct by using advanced solid modeling features in Fusion 360 as shown in Figure \(\PageIndex{1}\).

finished HVAC duct — Figure \(\PageIndex{1}\): HVAC duct that will be created in this module.

finished HVAC duct orthagonal views — Figure \(\PageIndex{1}\): HVAC duct that will be created in this module.

Steps to create the HVAC duct

This section lists the steps needed to create an HVAC duct as shown in Figure \(\PageIndex{1}\).

Step 1 - Sketch the front face

Draw a “center rectangle” 75 millimeters (mm) in length and 35 mm width on the front plane as shown in Figure \(\PageIndex{2}\). The center of this rectangle is at the origin.

Sketch front face — Figure \(\PageIndex{2}\): Initial sketch of the front face.

Step 2 - Create an offset plane

Create an offset plane from the bottom plane. This new plane is offset 100 mm away from the bottom plane as shown in Figure \(\PageIndex{3}\).

Create offset plane — Figure \(\PageIndex{3}\): Creating offset plane from the bottom plane.

Step 3 - Create a circle on the offset plane

Create a circle of diameter 50 mm. The center of this circle is 100 mm away from the origin on this new plane as shown in Figure \(\PageIndex{4}\).

Create circle on the offset plane — Figure \(\PageIndex{4}\): Circle on the offset plane.

Step 4 - Create a parallel plane to the right plane

Create a plane that is parallel to the right plane and coincides with the origin and the center point of the rectangle created in step 1. This plane is in the blue color as is shown in Figure \(\PageIndex{5}\).

Create parallel plane — Figure \(\PageIndex{5}\): Parallel plane created in step 4.

Step 5 - Sketch a spline

On the plane created in the previous step, sketch a spline as shown in Figure \(\PageIndex{6}\). The choice of the curve is up to the designer, the only restriction is that is must be as smooth as possible and must join the center of the circle to the center of the rectangle.

Sketch spline — Figure \(\PageIndex{6}\): Sketch the spline.

Step 6 - Create the Loft

Under the Create menu, select the “Loft” command and a dialog box will open up. As shown in Figure \(\PageIndex{7}\), under the profiles section, select the rectangle and the circle. To guide the loft profile, select the centerline as the spline you have already created in step 5. Once the profile is created, select OK in the dialog box.

Create loft — Figure \(\PageIndex{7}\): Create the Loft.

Step 7 - Create the Shell

Use the Shell command to hollow out the body created in the last step. Select the two faces (rectangle and circle) and select the thickness as 5 mm as shown in Figure \(\PageIndex{8}\). Remember to save your work.

Create shell — Figure \(\PageIndex{8}\): Create the Shell.