Spiralling Features in Autodesk Fusion

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Equation-based spirals

The first method of creating spirals, and in fact all types of equation-based curve geometry is the free plug-in "Equation Driven Curve" by CodeReclaimers. Once also available on the Autodesk Apps, the download of this tool seems to be unavailable at the moment, but you can get it from the tip Curves in Fusion. Copy/install the plugin into the ApplicationPlugins subfolder (see the Readme file). Enable it in the Fusion Add-ins dialog (Shift+S) and start it with the function "Equation Driven Curve" in the Sketch environment. The resulting geometry is a spline, with a number of computed control points. Using this plugin, you can create a spiral or helix or any other mathematical curve as a Fusion sketch geometry.

The control expression/equation for a spiral is e.g.:

x(t) = 0.05 * t * sin(t)
y(t) = 0.05 * t * cos(t)
z(t) = 0

But you can also create logarithmic spirals (see below), Archimedean spirals, 3D helices and other types of "spiral" geometry.

Coil-derived spirals

Another approach for creating spirals and helices is the Coil tool. This functions directly creates a 3D coil (helix) with no sketches or other construction geometry. But you can the project one of the edges of this 3D geometry back to a 2D or 3D sketch curve. So this constitutes the reverse of the usual modelling approach in Fusion.

So how to proceed:

Use the ribbon SOLID > CREATE > Coil to start creating a 3D helix object.
To create a 2D spiral, select Spiral as the coil Type, set the desired inner diameter.
Change the cross-section shape to "Triangular (inner)" and the section position to "Outside". This will adjust the inner edge of the resulting Triangular coil to match the desired dimensions.
Enter the remaining information about the coil/helix. Helices can be defined by setting the revolutions and height, revolutions and pitch or height and pitch, for 2D spirals only by the number of revolutions and "threads" pitch. When finished, click OK to create the coil/helix body.

Now you are ready to backtrack the model. Start a new Sketch and:

If you want to create a 3D helix, enable 3D Sketch (the last option) in the Sketch palette.
Go to SKETCH > CREATE > Project / Include > Include 3D Geometry.
Select the sketch plane and select the inner edge to create a 2D or 3D sketch object.
Click OK and click the "Finish Sketch" button to end the sketch.

Now you have a sketch depending on the source 3D model. The spiral sketch object is purple, indicating that it is formed by projecting a reference. Follow the steps below to remove this reference and allow the helix body to be unlinked and removed:

Turn off the visibility of the 3D helix body.
Right click on the sketch spiral in the viewer or on the timeline and select "Edit Sketch".
Click on the reference glyph.
Press the Delete button on your keyboard or select Delete from the circular context menu.

The sketch spiral is now detached. It is displayed in blue and its control points are shown. You can now freely remove the forming helix body.

By any of these workflows you will obtain a spiral sketch which can be used for any other modeling operation in Autodesk Fusion.

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(Source article: How do I create a 3D helix or 2D spiral sketch in Fusion?)