Learn Autodesk Fusion in 30 Days (formerly called ‘Fusion 360’) is the most popular Fusion course online and was first launched in 2019. Since then, we have launched a revised 2023-24 version, and we are now releasing a fully updated and improved 2026 version.
This is Day #9 of the 2026 Revised version of the course.
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Transcript
Welcome to Day 9 of Learn Fusion in 30 Days. Today, you’ll create the shape of an LED lightbulb while learning to use Fusion’s primitive tools and the easy way to create this smooth transition. Let’s get started!
Start with a new Part Design file and save your design.
Today, we’ll focus on the overall visual appearance without considering the manufacturing or other aspects of a real light bulb.
There will be times you’ll need to quickly create a 3D model for rendering or communication purposes, versus 3D printing or manufacturing.
Instead of starting with a new sketch, activate the Cylinder primitive from the Create menu of the Solid tab.
Notice it prompts us to select an origin plane or planar face. Select the bottom XY origin plane, as we’ll create the stem of the light bulb as if it were sitting upright.
Select the origin point as the start of the cylinder and define the width as 35mm.
Click to place the diameter and notice the Cylinder dialog appears, allowing you to define the overall height or change the width.
Primitive shapes streamline the design process by combining sketching and 3D volume creation into a single, automated step. However, primitives present some drawbacks, including potential reference and parametric issues.
As a best practice, use Fusion’s primitive shapes when working on small or quick models, such as this visualization. For more complex models, particularly ones that need to be fully parametric, utilize fully defined sketches and modeling features instead.
Define the height of the cylinder as 40mm before clicking OK.
To create the sphere on top, we’ll want a reference line to snap to. We’ll once again use the Intersect tool.
In the Browser, toggle open the Origin folder. Right-click on the XZ origin plane and select Create Sketch. We’re choosing this plane because it slices our model down the middle, allowing us to create points on each edge of the cylinder.
Press “S” to open the shortcuts menu, type “Intersect,” and click to activate it.
Select the topmost edge. Make sure you check the projection link before clicking OK. This ensures the projected edges update if the cylinder size changes.
Notice the two purple corner points. These represent the exact points where our sketch intersects the edges of the cylinder.
We can now reference these two points, knowing they will always represent the exact edges.
Let’s connect the two dots with a standard line. Activate Line, click the purple intersected point on the left, and then click the point on the right.
To create a starting point for the center of the sphere, add a 20mm vertical line.
Press ESC to exit the existing line and press the spacebar to reactivate Line.
Zoom in on the model and start the line where it snaps to the midpoint. Notice that a triangle glyph appears at the midpoint or exact center of the line.
Define the length as 20mm and click to place the line where it snaps vertically along the Z-axis.
An automatic perpendicular constraint applies to the corner.
Press ESC to clear the line command.
Since these two lines only serve as references for the sphere, hold down the Shift key and select both lines. Select the Construction option in the Sketch Palette.
While not required, this best practice of creating dashed reference geometry will help you avoid issues in more complex models.
We can now activate the Sphere primitive from the Create menu of the Solid tab.
Start by selecting the end of the construction line, which serves as the center of the sphere.
Define the width as 63mm. Notice Fusion defaults to the Cut operation since it detects the cylinder. Switch the operation to “Join” so the sphere joins the existing cylinder, and click OK to save it.
Notice you created the basic shape with a single sketch and two primitives.
Let’s now use Fillet to add material to the inside edge. As a general rule, fillets remove material from outer edges and add material to inner or adjacent edges.
Activate Fillet and select the edge where the two shapes meet. Drag the blue directional arrow to experiment with the appearance.
Define the fillet radius as 45mm.
As you learned on Day 8 with the doorstop, add a new selection set in the Fillet dialog. This allows you to select the bottom of the cylinder and define a separate fillet radius of 4mm.
Before we add the thread, let’s add some appearances.
Press the shortcut “A” for Appearance.
Fusion offers several LED appearances that represent real light when viewed in the Render Workspace.
Search for LED in the appearance dialog and download the appearance, if needed.
If you drag and drop the appearance, it applies to the whole body. First, select the upper part of the light bulb. Notice the area highlights in blue.
This enables you to drop the LED appearance inside the highlighted area, applying it only to the top.
Search for “Plastic Glossy Grey” to apply to the bottom.
After you download the appearance, drag and drop it onto the bottom part of the lightbulb.
Notice the warning message. Fusion asks if you want to keep or remove the LED appearance we already applied.
Select Keep.
In the Appearance dialog, find the grey plastic located within the “In this design” section. Here, you can edit the appearances further. Right-click on the appearance and select “edit.”
Click and drag the color picker to choose a different shade of grey.
Let’s now create the bottom cylinder where the thread will go.
Activate the Cylinder primitive again.
Zoom in and select the bottom face of the existing cylinder. Click to start at the center origin.
Define the diameter as 25mm and click to place the cylinder.
The height will be 19mm.
Very important: If you leave this set to Join, the cylinder inherits the plastic material. Change the operation to ‘New Body’ so we can apply a metal appearance to a separate 3D body.
Fusion’s thread tool does not offer the Edison Screw type that a typical light bulb would have. Instead, you can create custom threads using the Coil tool.
Activate the Coil primitive from the Create menu.
Start the coil primitive by selecting the bottom of the recent cylinder.
Click the center origin to start and define the diameter as 25mm. After you press Enter, notice the Coil dialog appears.
The coil tool offers many different Type options, each of which allows you to define the coil in different ways.
We know the height of our cylinder and that we want the thread to go around 4 to 5 times, so select “Revolution and Height.”
Remember, our goal with this model is to make it visually look ‘good enough’. Through some trial and error, I found the following settings that visually mimic an Edison screw.
Take some time to experiment and let me know in the comments if you find a better way!
The key takeaway here is recognizing that the coil tool can help you create custom threads.
Start by setting the section—or the size of our circle—to 2.5mm.
Set the Revolutions to 4.5 times.
Set the height to -18mm. The negative is necessary to drive the coil upward.
Leave the angle set to 0.
Use the default circular profile and on-center section.
Lastly, set the operation to Cut this out of the existing cylinder, and click OK to save the coil.
Before we finish this with fillets, add the beveled edge to the bottom. Activate Chamfer form the Modify menu and select the bottom edge.
Define the Chamfer as 3.5mm and click OK. This helps make the thread more realistic at the start.
Activate the Fillet tool and select all of the sharp edges. There will be three different edges to select.
Set this fillet to 1mm; this creates a rounded profile that closely mimics the look of authentic Edison thread.
Click OK to save the fillet.
Now add the electrical foot contact to the bottom of the bulb.
Use the Cylinder command once again. Start on the bottom planar surface and select the origin point.
Click the edge of the existing cylinder to create a matching diameter of 18mm. Set the height to 2mm.
Before you click OK, make sure the operation is set to “New Body,” allowing you to apply a different appearance.
Activate Chamfer one last time and apply a 2mm chamfer to the bottom-most edge.
Experiment and have some fun by applying a metal appearance to the thread and a different appearance to the foot contact.
Great job completing the light bulb! I’ll see you on Day 10, where we’ll reinforce all the skills you’ve learned so far to make a 3D printable phone case.