Create a Hex Nut in Fusion 360 with Midplanes and Mirror

Kevin Kennedy: Welcome to Day 6 of Learn Fusion in 30 Days. Today, you’ll create a hex nut as you learn to create faster with Midplanes and Mirrors.

I’ll also show you a pro trick when using the thread tool. Let’s get started! Start with a new Part Design file and save your design.

Start a new sketch on the XY origin plane, imagining the hex nut lying on a table. During the first 5 days, you used rectangles and lines to create sketches. The Create menu of the Sketch tab offers many other sketch objects to

help you create geometric shapes. Activate the Circumscribed Polygon tool; it quickly creates the 6-sided polygon for the hex nut.

Click the center origin to start. As you drag your mouse cursor away, define the length and the number of sides. Type 10mm for the first input to set half the overall length.

Press the Tab key to switch inputs and enter 6 for the second input to represent a 6-sided polygon. Click to place the polygon, without worrying about its orientation.

The sketch is not yet fully defined. Activate the Horizontal sketch constraint from the toolbar and select the top edge of the polygon.

This forces the edge to remain horizontal. The Browser should now display a red lock icon on the sketch, indicating you have fully defined the geometry.

The hex nut will now only change shape if you edit this sketch and modify the 10mm dimension. Press “E” to activate the Extrude tool and view the model from the Home position.

Define the Extrude distance as 10mm to set the total thickness of the hex nut. With a simple sketch and an extrude, you have created the overall shape of the hex nut.

You will now add chamfered edges to one side, which you will later mirror to the other. Fusion includes a Chamfer tool; however, the tool does not allow you to apply

the chamfer in a circular manner. You can solve this with a simple triangle sketch that you will revolve around the center axis.

Start a new sketch on the XZ origin plane. Open the Origin folder in the Browser, right-click the XZ plane, and select Create Sketch.

Choose the XZ plane because it slices the 3D body down the middle at one of the vertices. You must choose the correct plane here, or you will not get the same

results when you revolve the triangle. To sketch the triangle, snap to the corner edge of the 3D body. You can achieve this in two main ways.

One option involves sketching the first line of the triangle and then using a Coincident constraint to force it to the corner edge. The other option utilizes the Intersect command.

Remember, on day 4, you used Intersect to create a point on each sketch profile for the Loft rails. Activate Intersect and select the upper-right corner.

I will change the perspective so you can better see which corner intersects the active sketch plane. Keep the ‘Projection link’ checked; this ensures the point automatically updates if

you change the size of the polygon sketch. You now have the purple Intersected point for reference. Use the “Look At” button in the Sketch Palette to look directly at the sketch.

Let’s also hide the Body in the browser so it’s easier to see the sketch Activate Line from the toolbar and click to start the line at the purple point. Define the length as 1.5mm and click to snap the line straight

down when you see the vertical glyph representing the vertical constraint. With the Line tool still active, sketch the rest of the triangle without adding dimensions.

Click to place the second line, then click the starting point again. It’s okay for the triangle to be an irregular shape. We’re going to use sketch constraints to fully define it.

Start by activating the Horizontal sketch constraint. Select the top line to force it to stay horizontal, ensuring it always matches the top edge of the 3D body.

As you learn to fully define sketches, clear out any sketch tools with the ESC key and click and drag the sketch geometry to find the moving objects. Notice the upper-left corner of the triangle still moves freely.

We’ll want to restrict these degrees of freedom to fully define the sketch. As discussed on Day 5 during the ice cube tray lesson, use constraints over dimensions where appropriate in Fusion.

In this sketch, set the top line equal in size to the right line. Very important - make sure you click in space to deselect anything after you drag sketch objects around.

Otherwise, sketch constraints may appear to be grayed out based on your selection. Activate the Equal constraint from the toolbar and select both the top and right lines.

The selection order does not matter because the right line already has a dimension; the underdefined object will always inherit the size of the defined one.

Verify that all sketch objects appear black and fully defined, and check for the red lock icon in the Browser. While we’re here, it’s best practice to rename your sketches

and bodies in the Browser. Clear any active commands with the ESC key, click once to select a browser object, and click again to edit the name.

Take a minute to rename the two sketches and the 3D body. While this may seem unnecessary for simple models, this habit will pay dividends when you work on complex projects.

Turn the 3D body back on in the Browser and verify that your sketch profile aligns with a vertex of the polygon. Activate Revolve from the Solid toolbar.

The tool should automatically select the profile since only one exists. If it does not, use this pro tip to select the sketch: notice that the mouse cursor often prefers the outer faces of the 3D body.

If you click and hold over the sketch profile, Fusion provides a selection menu, allowing you to select objects hidden behind others. Click to select the profile.

Use the Z-axis as the revolve axis. Switch to the Axis selector and select the Z-axis in the Browser. The Revolve tool automatically changes the Operation to “Cut” because

it detects the existing 3D body. The red graphic on the model also indicates that this profile will cut away from the body.

Ensure you change your operation to Cut before selecting OK. Most Hex Nuts are symmetrical, so let’s mirror this over to the other side. To mirror, you need a plane or axis that slices the model in half.

Since none of the origin planes align with this, head to the Construct menu and activate the Midplane option. Midplane makes it incredibly easy to create a plane directly in the

middle of two selected objects. Select the top face of the hex nut, use the ViewCube to tilt the model, and then select the bottom face.

This creates a plane directly in the middle. Click OK to save the midplane. Activate the Mirror command from the Create menu of the Solid tab.

Remember, Fusion also has a mirror command in the sketch environment, so ensure you activate the Solid mirror. Similar to the Rectangular Patterns you created on Days 1 and 5, the

Mirror tool allows you to mirror bodies, faces, and features. Choose the Features option, which allows you to select the Revolve in the Timeline. Switch to the Mirror Plane selector and select the midplane construction plane.

Similar to the Rectangular Pattern ice cube cutouts from Day 5, you have compute type options. Choose the Optimized option for the fastest performance; I will place notes

on these options in the video description. Finish the model by adding the threaded hole. We’re done using our Midplane.

Turn off the Midplane by selecting it and pressing the shortcut “V” for View to hide the object. You can also right-click the object and select Hide.

It’s now time to finish the model with the threaded hole. One best practice in Fusion - and most parametric CAD programs - involves keeping mirrored geometry at the end of your timeline.

This ensures better performance and helps you avoid dependency issues. In this case, click and drag the timeline marker back before the Mirror tool. This allows you to add the threaded hole before the mirror command.

Fusion offers a Hole command; however, it does not allow you to chamfer the thread like a real hex nut. Instead, we’ll create a manual hole and then use the Thread tool.

Press “C” to activate the Circle tool and choose the top plane as the sketch plane. Start at the center origin and define the diameter as 12mm. Activate Extrude with the letter “E” for Extrude and select our circle profile.

We want this hole to always span the full height of the 3D body by setting the “Extent Type” to “All”. This setting ensures the hole always cuts through the entire thickness, even if you

update the height of the hex nut later. Verify that the operation cuts away the existing 3D body before clicking OK. Let’s now add a Chamfer to the hole.

While the Fillet tool creates rounded edges, Chamfer creates beveled edges. Activate Chamfer from the Modify menu. Select the edge of the cutout.

Change the type to Distance and Angle, then define the distance as 0.5mm and the angle as 45°.

Finally, activate the Thread tool from the Create menu. Select the inner cylinder face to apply the thread. Very important - you must check “Modeled” option if you want the

thread to affect the actual 3D body. Otherwise, Fusion defaults to representing threads with a static image that does not affect the model upon exporting.

This helps reduce latency in large files containing hundreds of threads. For a 20mm hex nut, use the standard pairing M12 x 1.75. Keep the thread type as ISO Metric Profile and change the size to 12mm.

Fusion often detects the hole size and sets this for you automatically. Ensure the Designation reads M12 x 1.75. If you click OK now, you will notice the thread does not start inside the chamfer.

A functional hex nut requires the thread to begin there. Double-click the thread in the timeline to edit it. Uncheck the Full Length option.

Notice the arrows point downward; you need them to point in the other direction so you can drag the thread into the chamfer. Here’s a pro tip on how to fix this: Let’s select the Thread command in the timeline

and press the Delete key to start over. Fusion determines the starting direction based on where you select the cylinder face.

Reactivate the Thread tool. Instead of selecting near the top, select near the bottom of the cylinder. This behavior is not very intuitive—let me know in the comments if you

think Fusion should add a flip button for these directional arrows. Check Modeled again and uncheck Full Length. The arrows should now point toward the top.

Set the length to 9.5mm. Take a minute to verify that the rest of the settings defaulted to the correct sizes.

Click OK to save the thread. We can now drag the timeline marker back to the end of the timeline. Since the Mirror tool did not originally include the chamfer, you must add it now.

Let’s edit the mirror feature. Double-click it in the timeline. With the Objects selector active, hold the Command key for macOS or

the CTRL key for Windows and select the Chamfer from the timeline. This allows you to select additional objects. Click OK and notice that the mirror now includes the chamfer.

Great job completing the hex nut! I will see you on Day 7, where you will learn to Project geometry, one of the most critical commands for building intelligence into your models.