Day 7 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2026 EDITION – Bike Handlebar Grip

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 #7 of the 2026 Revised version of the course.

Full Course on YouTube

Watch the full course in this official PDO YouTube playlist.

Get the 15-day Bundle of Companion Guide (Step-by-step PDFs)

Grab the official, step-by-step PDF guides and build your CAD mastery on a rock-solid foundation of practice projects and challenges. Serves as a standalone guide or the perfect companion to the video lessons.

Transcript

Welcome to Day 7 of Learn Fusion in 30 Days. Today, you’ll create a bike handlebar grip as you learn to create text, use the Emboss Tool, and how to reference existing geometry with the Project tool. Let’s get started!

Start with a new Part Design file and save your design.

We’ll start by sketching the side profile of the handlebar using a Center Diameter Circle. Press “C” for Circle, then select the side XZ origin plane.

Follow the best practice of starting the sketch from the origin point. Click the origin and define the circle as 30mm before clicking to place the circle.

Let’s define the thickness with the Extrude tool. Activate Extrude and set a total length of 125mm.

Click OK. The base cylinder provides a 3D body for embossing or debossing text. We’ll then finish the model with additional details later.

To run the text along the length of the cylinder, we’ll create a new sketch on the YZ origin plane.

Right-click the YZ plane in the Browser and select Create Sketch.

Find the Text command in the Create menu of the Sketch tab, or press the shortcut letter “S” and type “Text” to find the feature.

Once active, the Text command requires you to define a bounding box, similar to graphics programs.

Click in the upper left to place the first corner, then click a second time to place the lower right corner.

We’ll eventually dimension the bounding box to the edges of the cylinder.

In the Text dialog, type out your name.

Choose your desired font, but note that Fusion’s 3D tools, including the Emboss tool, require a TrueType Font (.ttf). OpenType Fonts (.otf) will not work unless you use an online converter. If your text fails to emboss later, the font type is likely the cause.

I will stick with a common font, such as Arial.

Center-align the text in both directions. This ensures the text remains in the middle once you finalize the bounding box.

After you choose a font, be sure to define the text height and character spacing according to your personal preference.

Make sure the text fits on the cylinder. I’ll set the text height to 16mm.

Click OK once you are satisfied with your text.

If you click and drag the bounding box corners, the box still moves freely. Constrain the bounding box to ensure it stays exactly where you want it.

Let’s use the Intersect command again to reference the points where the active sketch intersects the cylinder.

Activate Intersect from the shortcuts box or the Create menu.

Select each edge of the cylinder to include all four corner points.

Use the Coincident constraint to force each of the four corners of the bounding box to snap to the four intersected points.

With Coincident active, select a bounding box corner, then select the corresponding purple point. Repeat this for the remaining three corners. 

Carefully select only the points and not other geometry. When you reach the last corner, click twice because the points overlap. This provides us with a fully defined sketch.

To see why this matters, finish the sketch and double-click the Extrude in the timeline. If you change the distance, the text automatically stays centered because you constrained the bounding box to the four corners.

I will undo this to set the Extrude back to 125mm.

Activate Emboss from the Create menu of the Solid tab.

Emboss allows you to raise or recess a sketch profile relative to a solid body.

Start by selecting the blue text as the Sketch Profile.

Switch to the Faces selector and select the outer cylinder face. Notice the Emboss tool automatically wraps the text around the cylinder.

Again, if this fails, try changing the font. When you edit your sketch, you can double-click on the Text to reopen the Text settings.

Within the Emboss dialog, you can switch between an Emboss and a Deboss or change the position of the effect.

Change the depth to 2mm, select the Emboss option, and click OK.

We’ll now create a new sketch on the leftmost face of the cylinder.

Right-click the face and select Create Sketch.

Sketching on this side profile allows you to create the first “ring” of the grip pattern.

In the past few lessons, you have used the Intersect tool. But what happens when you want to reference geometry that does not intersect your sketch plane?

This is where the Project command comes into play. You can find the Project tool in the same flyout menu as Intersect.

With Project active, select the outer cylinder edge. While the Intersect command could also achieve this, you also want to include a reference point from the letters. Select the top and bottom edges of your first letter. Notice how this projects the geometry onto your active sketch plane.

Project and Intersect are very similar; however, Project allows you to select objects that do not intersect with the sketch.

Before you click OK, ensure you check the Projection link. This ensures the data always updates, so the grip texture automatically changes size if you change the original circle sketch. We will test this in a minute.

Activate the Offset tool from the Sketch toolbar. Select the circle edge and define an offset distance of 2mm. Using Offset adds further intelligence to your parametric model; this circle will always stay 2mm away from the projected circle, even if you change the size of the cylinder.

Before you extrude the shape, draw two lines to block the section around the letters.

Activate the Line tool and hide the 3D body to see the sketch more easily.

Draw two lines connecting the circles, ensuring they lie outside of the projected points. We’ll adjust the position later.

Turn the 3D body back on and activate Extrude.

Select the new Profile shape and use the ViewCube to look at the model from a perspective view.

Define a distance of 1.5mm, ensuring it heads toward the letters. You may need to add a minus symbol to flip the direction of the Extrude.

Lastly, set the Operation to “New Body.” This creates a separate body in the Browser, making it easier to pattern.

Toggle open the Bodies folder in the Browser. Notice you have two different bodies; you can turn this new body on and off as needed.

Activate the Rectangular Pattern tool. Instead of Features, set the Object Type to Bodies and select the ring body. This would not be possible if you had joined the body to the existing cylinder.

Click the Axes selector, followed by the Y-Axis. Drag the blue arrow to start the pattern. You can then experiment with the various quantity and spacing options.

I will set mine to the Spacing distribution, with a quantity of 50 and a distance of 2.5mm. Click OK to save the pattern.

Looking at the pattern, I would prefer the grip to wrap all the way around where there is no text. As you design in Fusion, you will often want to go back and change your approach, which is one of the many advantages of parametric modeling.

Double-click the last Extrude in the timeline to edit the profile. Select the second part of the profile to include the full circle.

After clicking OK, you will see the rings now collide with the text. To fix this, leverage that same sketch. At times, you can use a single sketch for multiple 3D features in your file.

In the Browser, turn Sketch 3 back on.

Activate Extrude again, this time selecting only the smaller sketch profile.

Extrude this across the grip texture by clicking and dragging the blue arrow. Notice the profile turns red, indicating it will cut away geometry.

Since you do not want to cut through the text, toggle open the “Objects to Cut” section of the Extrude dialog.

Unselect the ‘Body 1’ option, as this includes both the text and the cylinder.

To avoid the rings, you could uncheck bodies in the long list; however, changing the Start and Extent types is the easier method.

Select the “To Object” extent type. This allows you to select a specific object to extrude to instead of relying on a distance. Zoom in and select the inside face of a ring closest to your text.

Very important: you must select an inside face rather than the outer face, as you need to reference a face in the same planar direction.

Let’s do the same for the Start option. Change the Start type to “Object.”

The tool will not appear to let you select a face. You will need to hold the CMD key on macOS or the CTRL key on Windows. Then, select one of the faces near the letters.

With just a few additional settings, we’re able to create a complex Extrude from an existing sketch. Click OK to save it.

Let’s now hollow the cylinder. Activate Shell from the toolbar and select the left face. Define the thickness as 2mm.

If an error message appears, it is because the Shell command cannot effectively trace the inside of some of your letters.

One great benefit of Fusion being parametric is that you can change things you may not have originally planned for.

Cancel the Shell tool and drag the timeline marker back to just before the Emboss command.

Complete the Shell with a thickness of 2mm, then drag the timeline marker back to the end.

You may notice we have a large number of 3D bodies in the Browser. Keeping the grip rings as separate bodies was originally important to complete the pattern.

If you no longer have a reason to keep them separate, we can simplify the file by using the Combine command.

Activate Combine from the toolbar. Select the cylinder, which is Body 1, as the Target Body.

For the Tool Bodies, select the next body in the list, scroll to the bottom, hold the Shift key, and click the very last body. Shift-clicking allows you to select the entire list at once.

Ensure the operation is set to Join, as the command allows you to join, cut, or intersect objects.

Very important: uncheck “Keep tools” because you no longer need the rings as separate bodies. Sometimes you might keep tools if you need them for other features, but not in this case.

Click OK and notice that only a single body remains in the Browser.

Let’s now test that the Projected geometry from earlier works as expected. 

Double-click the very first sketch in the timeline to edit it.

Double-click the circle’s dimension and define a larger size, such as 50mm.

Finish the sketch and observe how all the rings and features update their size. If you had not projected or intersected that circle, the rings would remain at their original size.

Project allows you to reference existing geometry and stands as one of the most powerful tools to master in Fusion. Let me know in the comments if Project makes sense or if you need more clarity.

When you created the grip sketch, you intentionally left the profile under-defined, as the two lines can still move freely. With Sketch 3 turned on, you can now click and drag those lines to update where the grip rings start.

Because you projected the points of the first letter, you can easily see where to drag them. You could even edit the original sketch and dimension this line a specified distance from the projected point.

Here’s a pro tip: sometimes experimentation is critical, and you will take several actions to think things through. Next to the Undo button, you will find a dropdown menu.

Watch what happens when I select “Undo Edit Sketch.” This takes us all the way back to before we altered the circle sketch, and saves you from pressing undo multiple times.

Let’s finish the model by creating a larger cylinder on the left side.

First, turn off Sketch 3 in the Browser. Right-click the left side of the cylinder and select Create Sketch.

Activate Project by pressing the letter “P” for Project and select the outer edge.

Once you project the edge, use Offset again, this time defining the distance as 5mm. Ensure it offsets to the outside; if it does not, press the Flip button.

Activate Extrude and select the outermost profile. Define a depth of 1.5mm, ensuring it moves toward the text.

Ensure this operation is set to “Join” the single 3D body.

One last pro tip for today related to applying appearances. Activate the Appearance command with the shortcut “A” for appearance.

Search for “Rubber” and download the material if you have not already. 

Drag and drop it onto the model. This automatically applies the appearance to the entire model since only a single body exists.

In the Appearance dialog, switch to the Faces option. This allows you to drag a different appearance onto the faces of the individual letters.

I’ll remove the rubber appearance to demonstrate this tip: hold the Shift key and select all of your letters to drop the appearance on all of them at once. Ensure you release the cursor within the highlighted area of the selected faces.

Notice that this applies the appearance only to the faces of each letter without affecting the rest of the 3D body.

I will see you on Day 8, where you will model a 3D-printable doorstop.