A solid-based approach to model speakers with SolidWorks

The purpose of this tutorial is to model a pair of speakers. Given the shape of this device illustrated on the cover, one could come with several techniques in order to model it using CAD features. Here is one possible way to model a speaker in SolidWorks, which involves interesting solid features available in SolidWorks.

If we were to position the speaker such as the one on the left-hand side of the image above, we could come up with an easy way to model the speaker's body. Indeed, we would have to draw two horizontal rectangular profiles, add volume and remove some for the speaker's drivers.
But hey, what if we want to model the speaker in its natural position, like the one on the right-hand side?

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Firstly, open a new part by going to File > New > Part…. Start a new sketch on the right plane by selecting it and clicking on the Sketch icon:

In the Sketch tab, find the Line tool:

Then add those four lines. Add dimensions using the Smart Dimension tool.

Notice that the lines are starting at the origin. Use a Parallel relation on the two oblique lines in order to avoid the need to insert another angle dimension.
Exit the sketch. Extrude it 85 mm across the right plane by selecting the Mid Plane option.

Start another sketch on the front plane. Add a rectangle to the sketch (you can find this tool next to the line's). Select its lower edge and, while holding Shift, select the origin. You can now set a Midpoint relation between the rectangle's edge and the origin point. Add the following dimensions to the sketch and exit.

In the Features tab, locate the Curves icon. Look for the Project Curve tool.

Project the sketch on the rear face:

In the Features tab again, find the Lofted Boss/Base tool. Select the curve we just created, as well as the front face. Uncheck the Merge resultbox, we want two separate bodies here!

Remove the first body by going to Insert > Features > Delete Body….

This body was indeed merely a support for the previous lofted feature.

Add 10 mm Fillets on the edges running from the front to the rear of the speaker:

The shape should now remind you of something. Locate the Chamfer tool under the Fillet tool and add 1.5 mm chamfers around the front face.

We now wish to cut some volume for the speaker drivers. To do so, we need to perform a revolution of a certain profile. The axis is inclined though, this makes the operation less manageable.

For now, hide the speaker's body. Add a new sketch in the now empty screen.

Start by the lines, add the Spline and the Arc in a second time. Use Vertical relations to manage the latter. The sketch should be fully defined.
Revolve this profile with respect to the horizontal line.
Show the main body. Start a new sketch on its front face (simply click on its face and on the Sketch icon).

The intersection of both construction lines is the center of the speaker driver.
Here comes an interesting feature of SolidWorks. Go to Insert > Features > Move/Copy…. This tool allows you to specify, among other things, Mates between bodies. Select the revolved body and make its circular face coincident with the main body’s front face. Then make the intersection of the two construction lines above and the outer edge of the revolved body Concentric.

That’s it! The second body is at the right place.
Add a new median plane ( Features tab, under Reference Geometry) between the top and the bottom faces by selecting these two faces:

This plane will be useful to mirror the revolved body.

Find the Mirror tool in the Features tab and mirror the body (if you struggle to select the relevant body, right-click on the model and go to Select Other).

Now the finishing move: go to Insert > Features > Combine…. Check the Subtract operation. As Main Body, select the first main body, and combine the two others.

By going to Curves > Split Line, you can split the resulting body with a circle around the speaker drivers to add brighter appearance like so:

.
The speaker is now finished!

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