An alternative way to model a speaker with SolidWorks

Want to read this tutorial offline ?

Get this tutorial as a PDF file you can freely read and learn from without an internet connexion.

The purpose of this tutorial is, as the title suggests, to model a speaker. Given the shape of this device that you can observe on the cover, one could propose a straightforward technique in order to achieve its modelization. However I chose to give you a different method here, somewhat less obvious, which involves interesting features available in SolidWorks.

As an exercise, try to imagine the path you would take to model such a speaker…

Done already? To give you an insight about how we are going to proceed, here is a little picture:

The speaker’s position on the left-hand side illustrates the straightforward way. One has to draw two horizontal profiles, add volume and remove some for the speaker drivers.
But hey, what if we want to model the speaker in its natural position, like the one on the right-hand side?

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 first 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.
Exit the sketch. Extrude it from 85 mm across the right plane by selecting the Mid Plane option.

On the front plane, start another sketch. Add a rectangle (the icon is not that far from the line’s own icon). Select its lower edge and, by holding Shift, select the origin. You can now set a Midpoint relation. Add the dimensions to the sketch and exit.

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

Project the sketch on the rear face:

Still on the Features tab, find the Lofted Boss/Base tool. Select the curve we just created, as well as the front face. Do not merge!

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

This body was merely a support for the lofted feature we created.

Add 10 mm Fillets:

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 body. Add a new sketch in the henceforth empty screen.

Start by the lines, add the Spline and the Arc in a second time. Use Vertical relations to manage the latter.
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 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 edge of the revolved surface 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:

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.

You may want to split the resulting body around the speaker drivers like so:

By going to Curves > Split Line.
The speaker is now done!