Day 12 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2026 EDITION – Slotted Screwdriver (Hybrid Design)

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 #12 of the 2026 Revised version of the course.

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Transcript

Welcome to Day 12 of Learn Fusion in 30 Days. Today, you’ll create a flathead screwdriver as you learn the 3-point arc command, circular pattern, and more. Let’s get started!

Start a new design file by choosing the Hybrid Design intent and save your design.

Use Hybrid because our screwdriver contains one part for the plastic handle and one part for the metal shank.

Create a new component for each part. Activate New Component from the toolbar.

Set the type to Part, as this represents a single manufacturable object. Stick with a standard component and ensure you uncheck External. This creates an ‘internal’ component that lives only inside this Hybrid design file.

Name this first component “Handle” and click OK.

This handle component serves as a container for everything related to the handle part.

Press Spacebar to repeat New Component and set this one to the Part Type as well. Name it Shank.

Before you click OK, clear out the parent selector. Select the top-level or ‘root’ component to ensure both components are nested at the same hierarchical level in the Browser.

Very important: Remember to keep a close eye on which component you have ‘active’ in the Browser. The radio button icon next to the component name indicates the active one.

Hover over the Handle component and click the radio button to activate it.

Press “C” for Circle and select the XZ origin plane to sketch the handle as if it were lying on a table.

Start at the center origin and define the diameter as 28mm before pressing Enter.

Press “E” to activate Extrude.

Define the length of the handle as 100mm. Click OK to save the Extrude.

To create the grip cutouts, start a new sketch on the back side of the cylinder. Rotate your model, right-click on the back face, and select Create Sketch.

Activate the Circle tool again.

Start the center circle anywhere on the edge of the existing cylinder. This automatically applies a coincident constraint.

Define the diameter as 6mm and press Enter.

Notice the circle stays constrained to the edge of the existing circle.

Click out in space to clear any selections.

Activate the Horizontal constraint. Select the origin and the center of the circle. This forces it to remain in position and fully defines the sketch.

Let’s cut half of this circle out of the existing cylinder. Press “E” to activate Extrude and select the right half of the circle.

Drag the blue directional arrow into the existing 3D body to cut away material. Define the distance as -75mm and click OK.

This represents the first groove on the handle. As a best practice, keep your sketches simple and manageable. Pattern the feature instead of sketching 5 more circles.

Activate the Rectangular Pattern tool in the toolbar and switch to the Circular type.

Very important, be sure to activate the Solid pattern tool and not the sketch pattern tool.

Set the Object Type to Features. This allows you to select the Extrude in the parametric timeline as the object to pattern.

Switch to the Axis selector. Because you started the handle from the center origin, you can leverage the center Y-axis that runs through the cylinder.

Very important: Our Handle component includes its own origin. Toggle open the origin folder and select the correct Y-axis nested in this part. This ensures the part never loses reference.

Leave the distribution set to “Full” and define the quantity as 6. Change the “Compute Type” to “Optimized” to ensure the fastest processing, and click OK to save it.

Before we round over the sharp edges, add the thumb rest on the front of the handle.

The YZ origin plane splits the handle down the middle. Right-click on the YZ plane in the Browser and select Create Sketch. This allows you to sketch the side profile and revolve it around the center axis later.

To sketch the 3-point arc at the top edge, use the Intersect command first to reference the existing edge.

Activate the Intersect tool.

Select the 3D body, ensure you check Projection Link, and click OK. Remember, this creates purple geometry where our active sketch intersects the existing 3D body. This edge will automatically adapt if you change the size of the handle.

Activate the 3-point arc command from the Create menu within the Arc flyout menu.

The 3-point arc requires you to define the starting point, the end point, and the radius of the arc.

Click to place the starting point anywhere on the projected line, and click again to place the end point.

Click a third time to place the radius.

Let’s now activate the Sketch Dimension tool to dimension the arc.

Select the corner projected edge and then the start of the arc. Click to place the dimension and define it as 3mm.

With the dimension tool still active, select the arc and define the radius as 13mm.

Notice the sketch is not yet fully defined, as the center point can still move freely.

Add a final dimension between the corner projected edge and the center point. Click to place the dimension to the left and define it as 9mm. This fully defines the sketch and prevents the arc from moving.

Activate the Revolve tool from the Solid tab. Revolve automatically selects the single sketch profile.

For the axis, select the Y-axis nested inside the Handle component, as this runs directly down the center of the handle.

The operation defaults to cut since it detects the 3D body. Click OK to save it.

Throughout the design process, you will often want to alter dimensions. Intentionally built parametric designs allow you to simply edit sketches or features to change the dimensions, without breaking the design.

Double-click the third sketch in the timeline and double-click the radius dimension to edit it. Change this to 14mm and press Enter.

Double-click the 9mm dimension and change it to 11mm. This makes the thumb rest more shallow. Once complete, select Finish Sketch to exit the sketch.

It’s a best practice to keep Fillets at the end of your timeline. This optimizes processing performance and prevents “lost references” or broken geometry that can occur at the edges.

Let’s first add the cutout for the shank.

Press “C” to activate Circle and select the front face of the handle to start the sketch.

Start at the center origin and define the circle as 7mm before pressing Enter.

Press “E” to activate Extrude and extrude this to a depth of -50mm. The minus symbol ensures this cuts into the handle 3D body.

Before proceeding, take a minute to rename your sketches in the Browser. Click once to select a sketch and a second time to edit the name.

Make the names descriptive of the task or design feature. This best practice pays dividends when you reopen old files or continue to work on multi-part designs.

Now, activate the Fillet command to round the sharp edges.

Select the two edges of our thumb rest and define this as 5mm.

Add a new selection set and select the front edge. Define this as 1.5mm.

Add a third selection set and select the back six edges of the handle. Once selected, define this radius as 10mm to create a large rounded end.

Click OK to save these Fillets.

Here’s a pro tip: when applying many different fillet radii, break them into two separate Fillet commands. This often helps the fillets compute better and makes them more manageable.

Activate Fillet again. In this case, you can select the long edges in a single click since the previous fillet connects the edges. Select all six long edges and define the radius as 2mm.

Add a new selection set and select the arc and short outer edge. Repeat this for the remaining five cutouts.

Define this fillet radius as 1mm and click OK.

This completes the handle. Click Home to reset the view.

Very important: remember to activate the Shank component before creating the shank. This ensures the sketches and bodies nest inside the correct part. You can also close the Origin and Sketches folders of the handle component.

Don’t forget, on Day 11, you turned off “Active Component Visibility” so each component remains opaque.

To create the Shank, you could technically Extrude the existing face of the circle. However, if you reference a face directly and then significantly modify or delete the original geometry, the dependent feature often loses its anchor. This results in errors and broken links in your timeline.

View the model from the Front position to right-click on the circular face and select Create Sketch.

Activate the Intersect tool.

Once active, select the inside circular face and click OK. This ensures the geometry of our shank always matches the handle cutout.

Activate Extrude and define the distance as 150mm.

As a best practice, always test your parametric designs as you go. Activate the handle component and edit the fourth sketch, which contains the shank cutout. Double-click the dimensions to edit and enter a new value.

When you select Finish Sketch, the shank automatically adapts in size. Again, you could achieve this by extruding that face; however, the Intersect command builds in more intelligence and ensures you never lose the reference.

Press Undo until you return to the 7mm diameter.

Let’s finish the design with the screwdriver tip. Create a new component for the Tip, which allows you to reuse the handle and shank for different designs.

Here’s a pro tip: Right-click the top-level or “Root” component and select New Component. This method remains the preferred choice as it automatically selects the root component as the parent, saving you a few seconds each time.

Set this one to the Part Type as well. 

Name this component “Tip” and click OK. Double-check that the Tip component is active in the Browser.

This time, reference the existing face to create the 3D body without a sketch. Press “E” for Extrude and select the end of the shank. Define the distance as 10mm.

The downside is that you only have an Extrude in your timeline without a sketch to alter. However, this works fine for simple use cases.

Toggle open the Origin folder for the Tip component. Right-click the YZ plane, as it runs down the middle, and select “Create Sketch.”

Again, use the Intersect tool to reference the existing edges.

Activate the 3-point arc tool. Start the first point near the front edge. For the second point, click where it snaps to the top purple edge. Click anywhere to place the third point.

The first endpoint can still move freely. Activate the vertical constraint and select the endpoint and the top edge. This forces it to remain on the front edge.

Activate Sketch Dimension. Select the center point and the first endpoint of the arc. Click to place the dimension and define it as 0.5mm.

Add a dimension between the corner edge and the second point of the arc. Define this as 9mm.

Lastly, add an 18mm radius dimension to the arc.

If you hide the Tip body, you will see that you need to fully close the sketch profile. Activate Line and sketch a line between the corner edge and the start of the arc.

Press “E” for the Extrude command and turn the 3D body back on. Since you sketched in the exact middle, change the Direction to Symmetric. Let’s build intelligence into the model in case the shank and tip diameter change. Update the “Extent Type” to “All.” This ensures the tool always cuts all the way through the existing 3D body.

Click OK to save the Extrude.

Let’s now mirror this to the other side. Activate the Solid mirror tool. Use the Features Object Type and select the Extrude in the timeline.

Switch to the Mirror Plane selector and select the XY origin plane inside the Tip component. Once again, use the Optimized option for the fastest performance and click OK.

The screwdriver model offers a fun opportunity to experiment with appearances. Have fun trying different plastic appearances on the handle, and remember you can apply appearances to individual faces.

Great job completing the screwdriver! I’ll see you on Day 13, where you’ll take a close look at why fully defining your sketches is so important.