Day 5 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2026 EDITION – Ice Cube Tray

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 #5 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.

3 Compute Types Explained

The Rectangular Pattern tool in Autodesk Fusion has three different Compute types.

1. Optimized

This is the fastest compute method. It creates the pattern by duplicating the faces of the original feature rather than recalculating the entire feature’s logic.

• Best for: Large patterns (e.g., a grill with 500 holes) on a flat surface.
• Constraint: It cannot be used if the pattern instances need to change shape or interact with different geometry (like wrapping around a curved face).

2. Identical

This method creates exact replicas of the original feature by calculating the first instance and then copying the resulting geometry to all other locations.

• Best for: Complex features that are identical in every way.
• Difference from Optimized: It is slightly more robust than “Optimized” but faster than “Adjust,” as it doesn’t re-solve the feature’s parameters for every instance.

3. Adjust

This is the most computationally expensive but “smartest” method. It recalculates each instance individually based on the surrounding geometry.

• Best for: Patterns where each instance must “adjust” to its location. For example, if you pattern a hole across a surface that varies in thickness, “Adjust” ensures every hole terminates correctly at the next face.
• Constraint: It can significantly slow down your computer if the pattern count is high because Fusion is essentially “re-modeling” the feature at every step.

Transcript

Your fifth challenge in Fusion starts right now: modeling this ice cube tray. I’m Kevin Kennedy, and this is Day 5 of Learn Fusion in 30 Days. Today,  you’ll learn a secret trick with the Shell command, how to remove material from 3D objects, and how to taper an Extrude. Let’s get started!

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

For some projects, such as this ice cube tray, you may find it easier to start with a 3D block, then remove material to create the final shape.

Activate rectangle with the shortcut letter “R” for Rectangle. Select the Bottom origin plane, as we’ll sketch this ice cube tray from a top view.

Switch to the Center Rectangle type in the Sketch Palette. This allows you to start from the center origin. Later in this lesson, you’ll see that using the center rectangle allows you to leverage the origin planes to sketch the outer lip of the tray.

After clicking the origin to start the rectangle, type 104 millimeters for the width, press Tab to switch inputs, and type 300 millimeters for the length.

Click to place the rectangle.

View the model from the home position so you can see the Extrude.

Activate Extrude from the solid toolbar or with the shortcut “E” for Extrude. Define the distance as 50mm. This will represent the overall height.

We’re now going to create the first ice cube cutout, allowing you to pattern the remaining ones.

Right-click the top surface and select Create Sketch.

Activate the Rectangle tool again, but this time leave it as the 2 Point rectangle.

Start the rectangle without worrying about the location.

Define the height as 40mm and the width as 30mm. Click to place the rectangle.

Our active sketch is not yet fully defined. Press Escape to clear the rectangle command; notice you can still click and drag the rectangle.

Use Sketch dimensions to precisely place the rectangle from each edge of the tray.

Activate the Sketch Dimension tool from the Toolbar. A Sketch Dimension requires you to select two sketch curves and then define the distance or angle between them.

Select the top of the rectangle, followed by the top edge of the 3D body. Remember from the toy block on day one: you must place the dimension.

Drag your mouse to the left and click to place the dimension. Type 7mm for the distance.

The Sketch Dimension tool remains active. Select the left edge of the rectangle and the left edge of the 3D body.

This time, place the dimension above. Here’s a pro tip: In cases where you want the same dimensions, you can select the other dimension field.

Notice this action fills out the dimension input with ‘d’ for dimension, followed by a number. This number reflects the sequence in which the dimension was created and can be used to reference that value elsewhere.

Press Enter and notice the dimension says FX: 7mm. The FX represents a function, where the software pulls the 7mm value from that original dimension.

For example, if you change the left dimension, notice the top changes as well. This works great for achieving a uniform distance between two adjacent edges. Leave this set to 7mm.

We’ll now use Extrude to cut this out. Activate Extrude with the shortcut ‘E’ for Extrude and view the model from the Home position. This makes the Extrude easier to see.

Remember, since you have more than one profile, you must select the profile to Extrude.

If you drag the blue arrow into any existing 3D body, a red preview indicates which area the software will cut away.

The “Operation” automatically changes to “Cut” in the Extrude dialog. You can manually change this at any time if it does not change automatically.

Define the distance as -30mm. It’s very important to keep the minus symbol to make this cut into the existing 3D body. Removing it creates a new 3D body above the tray.

In the Extrude dialog, you will find a Taper Angle. Ice cube trays include a taper angle to allow the ice to fall from the tray.

Define the taper angle as -10 degrees.

Notice the cube is now tapered on all four sides.

Click OK to confirm the Extrude.

Before you pattern the remaining cutouts, add some Fillets to include them in the pattern.

Activate Fillet and select all five inner faces of the cutout.

Use the ViewCube to reorient the model as needed.

Once you select all the faces, define the Fillet radius as 4mm.

Ensure the corner type defaults to ‘Rolling Ball’ before clicking OK.

Similar to the toy block on day 1, we’ll now use the solid modeling Rectangular pattern tool.

We’ll once again use the ‘Features’ Object Type, which allows you to select the Extrude and the Fillet in the parametric timeline.

One important word of caution: use care when patterning objects with Fillets. In this case, the project remains simple enough that you shouldn’t run into performance issues. However, patterning many fillets in a large file often causes performance problems.

For the Axis selector, select the two edges of the 3D body. Select the long edge first so it becomes Axis 1 in the dialog.

Click and drag the directional arrows to start the patterns. This is never required, but it makes it easier to verify which direction is Axis 1 or 2.

You may also find it helpful to view this from the top view and zoom out to see the full model.

For Axis 1, define a quantity of 7.

Fusion calculates the Distribution in one of two ways: the Full Extent or “length” of the pattern, or the “spacing” between each object.

Oftentimes, you won’t know the distance until you drag the directional arrows. This can take some trial and error.

With the “Extent” option selected, define a total extent distance of 255mm.

For Axis 2, set the Quantity to 2. The Extent distance is 50mm.

Before you select “OK,” take note of the “Compute Type.” This determines how the pattern computes and may affect Fusion’s performance.

Change this to “Optimized,” which computes the fastest. I’ve placed explanations of each Compute Type below this video.

Click OK and view the model from the Home Position.

It’s now time to show you one of the ‘secret’ or lesser-known ways to use the Shell command.

On days 1, 2, and 4, we saw how Shell hollows out bodies when you select a single face. Many users do not know that you can select multiple faces to perform an exterior shell.

Activate Shell from the Toolbar.

Orbit the model to select the four side faces as well as the bottom face.

With these five outer faces selected, define the Shell thickness as 2mm.

The Shell command traces the outer contour of our ice cube cutouts, leaving only the defined thickness… this makes it super easy to create complex shapes.

Let me know in the comments if you’re surprised by the Shell results.

To complete the ice cube tray, add a flange to the outer perimeter.

We will sketch a profile and sweep it around the outer edge.

We need to first round over the four corners to create a continuous sweep path.

Activate the modeling Fillet command and select each of the four corner edges.

Define the Fillet radius as 10mm before clicking OK.

To sketch our sweep profile, we’ll start the sketch where we can snap to the existing edge.

To start this lesson, we used a center rectangle instead of the 2-point rectangle. This allows us to leverage the origin plane that runs down the middle of our tray.

Toggle open the Origin folder in the Browser. Right-click on the XZ origin plane and select Create Sketch.

Zoom in on the left side, so it’s easier to see the sketch.

Activate the Line tool. Start by clicking at the upper edge and sketch a backwards “L” shape without worrying about the dimensions.

However, ensure the automatic sketch constraints keep your lines vertical and horizontal. Fusion should automatically apply a perpendicular constraint to each corner.

Once the shape is defined, our goal is to get the red lock icon in the Browser, so our sketch cannot move.

Activate the Sketch Dimension tool with ‘D’ for Dimension.

Click the top line, place the dimension, and define it as 2mm.

Set the left vertical line to 3mm. You may notice our starting point has moved; we will fix that in a second.

Define the bottom line as 5mm.

We also want the bottom left line to be 2mm. However, instead of defining another sketch dimension, press ESC to clear the Sketch Dimension tool.

Activate the Equal constraint in the toolbar. With Equal active, select two sketch lines to make them equal in size. Select the 2mm line, followed by the desired line. Notice it changes in size to 2mm.

When possible, it’s a best practice in Fusion to use constraints over dimensions. This keeps your sketches simpler and easier to maintain. 

Constraints are a critical concept that we will continue to discuss throughout this course.

Switch to the Coincident constraint in the toolbar. Coincident forces the points to stay together. Select our starting point of the line and the upper edge of the ice cube tray.

Notice the entire sketch moves to snap to that edge. Our sketch is now fully defined, and we have a red lock icon in the Browser.

Activate the Sweep tool from the Solid toolbar.

Select the backwards “L” sketch profile and view the tray from the Home Position.

Switch to the Path selector.

For a Sweep path, you can often select the existing edge of a 3D body instead of creating a sketch. Ensure you check ‘Chain selection,’ which allows you to select the entire edge with a single click.

Double-check that the profile sweeps all the way around the model and that the operation “Joins” the existing 3D body.

Click OK, and let’s activate the Fillet tool.

Apply a 1mm fillet to the four edge lines around the outer contour, rounding over the sharp edges.

Great job creating the Ice Cube Tray! I’ll see you on Day #6, where I’ll show you how to create geometry even faster using Midplanes.