Day 8 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2026 EDITION – 3D Printable Doorstop

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 #8 of the 2026 Revised version of the course.

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Recommended 3D Print Settings

Planning to 3D print the doorstop? Use the following settings as general guidance. They serve as a great starting point, but keep in mind that every 3D printer and filament may require some additional fine-tuning.

Keep most of your settings to your default 0.2mm – 0.4mm layer height of something that doesn’t have much detail. Then, adjust the following:

• Infill Density: 15% – 25%
• Infill Pattern: Gyroid. This is the best pattern for flexible materials because it provides equal strength and flexibility in every direction.
• Wall Line Count: 3 to 4. This provides enough “skin” to resist the door’s edge without making the whole block feel like a rock.
• Combing Mode: Set to “All” or “Within Infill”. This keeps the nozzle over the print as much as possible, hiding the TPU oozing/stringing inside the doorstop.

Note: As seen in the video, please ignore my horrible stringing on the last layer, as I ran out of filament with 30 seconds left 🙂

TPU Filament is Recommended

This is my favorite TPU 3D printer filament (Amazon affiliate).

Regardless of your printer, start here for TPU-specific adjustments:

• Nozzle Temperature: 230°C (Polymaker prints best in the 220°C–235°C range).
• Bed Temperature: 30°C – 40°C (TPU sticks very well; higher temps can make it nearly impossible to remove without ruining that first layer).
• Flow Rate: 105% to 110%. Because TPU is stretchy, the extruder gears often “slip” slightly. Increasing the flow compensates for this.
• Cooling Fan: 50% to 80%. Keep it at 100% for the overhangs of the doorstop, but lower for the first few layers to ensure a solid bond.

Transcript

Welcome to Day 8 of Learn Fusion in 30 Days. Today, you’ll create a 3D-printable doorstop as you learn the Thin Extrude, Pattern on Path, and exporting for 3D printing. Let’s get started!

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

When designing for 3D printing, always consider the orientation of your design.

In our case, we’ll print the doorstop on its side to allow the inner cavity to print without any support material.

Start a new sketch on the XY Origin plane, as you’ll create the doorstop lying on its side.

Activate the line tool and start at the center origin.

Sketch the first line running to the right and click where it snaps horizontally, without defining a dimension.

Sketch back to the green Y-axis.

Notice if you start near the origin and move your mouse upward, Fusion helps you snap vertically from the origin.

Click to place this line.

Then, click the origin to sketch the third line of the triangle.

Take note of the two automatic sketch constraints applied: a horizontal constraint on the first line and a perpendicular constraint at the corner.

If you don’t see these, manually apply the constraints.

Let’s now fully define the sketch with dimensions.

Press the shortcut “D” for Dimension and select the bottom line.

Click to place the dimension and define the length of the doorstop as 135mm.

Add a second dimension to the left, defining the overall height as 50mm.

The sketch is now fully defined. Double-check by finding the red lock icon in the Browser.

Press the shortcut “E” to activate the Extrude tool.

In the previous days of this course, you extruded closed profiles and shelled them to hollow them out. Today, switch to the Thin Extrude option in the dialog.

Thin Extrude acts as a shortcut for creating walls or shelled structures. It transforms a simple 2D profile into a 3D feature with a defined wall thickness, in one single step.

Define the extrude distance as 40mm.

Notice the Thin Extrude includes a wall thickness in the dialog.

Update the wall thickness to 4mm.

This provides a nice 3D printed wall thickness that resists breaking if someone steps on the doorstop.

Click OK to save the Extrude.

Notice you created the overall doorstop shape with a single sketch and single Extrude, versus using the Shell command after the Extrude.

Use Thin Extrude for quick, simple walls built directly from a sketch, but stick with the Shell command for complex 3D shapes where you need a uniform wall thickness across multiple faces.

To make the doorstop more usable, we’ll sketch a grip on top, followed by the Pattern on Path to wrap it around the triangle.

Let’s first round over the sharp corner edges to create a continuous path to follow.

Activate Fillet from the toolbar, and start by selecting the two inside edges on the left side. Rotate the model if it makes it easier to select the edges.

Type 3mm for the fillet radius.

The fillet dialog allows you to add different fillets within the same tool.

Select the plus symbol to add a new selection set. This allows you to select the outer two edges separately, defining these as 6mm.

Hold the CMD key on Mac OS, or the CTRL key on Windows, if you happen to select the wrong edge or face. This allows you to deselect or select additional edges.

You can also toggle between selection sets in the dialog.

Add a final selection set, selecting the front edge of the doorstop. This time, define a fillet radius of 2mm.

Click OK to save the Fillet.

Notice you only have a single Fillet in the parametric timeline.

Selection sets help you define multiple fillet radii without the need to use Fillet multiple times.

Let’s now sketch the first grip shape.

Right-click on the top planar face and select Create Sketch.

Activate the Circle tool from the Toolbar. Click anywhere out in space to start the circle, and define the diameter as 4mm before pressing Enter.

The circle will still move freely.

Activate the Coincident constraint. Use this to force the circle to snap to the top edge of the doorstop.

Select the center point followed by the top edge of the 3D body.

Press ESC to clear the Coincident constraint.

Click and drag the circle. Notice the coincident constraint forces it to stay on this edge, though it still moves freely along the edge.

Use the Sketch Dimension tool to fully define the sketch.

Activate Sketch Dimension and click the center point of the circle, followed by the starting point of the top edge.

Click to place the dimension and define the distance as 7mm.

You now have a fully defined sketch and don’t have to worry about it moving.

Press the shortcut letter “E” for Extrude, and select the top half of the circle. The 3D body automatically splits the circle profile in half.

When designing parametric models, there are many small settings that will help you build intelligence into your model.

Here’s a best practice in Fusion: Instead of simply typing out the height of 40mm, set the Extent Type as To Object.

Rotate the model and select the opposite face as the Object to extrude to.

The second extrude feature then automatically adapts if you change the height in the first Extrude.

Take note of the operation being set to “Join” the existing 3D body before you click OK.

Double-click the first Extrude and change the height; notice the grip on top automatically adapts.

Press Undo to revert the change.

Activate the Rectangular Pattern tool from the toolbar. In the dialog, switch to the Pattern on Path type.

This allows you to define an object and pattern it along a path, such as the outer contour of the triangle.

Because you set the grip texture to Join the existing 3D body, use the Faces Object Type. This will allow you to select the outer face of the grip.

Switch to the Path selector and select the outer contour as the path.

Click and drag the directional arrow to pattern the faces along the path.

This type of pattern often takes some trial and error to find the right numbers. Define the quantity as 40.

With the distribution set to Extent, define the entire length of the path.

Here’s a pro tip: You can find the length by shift-clicking all the path edges before you enter the Pattern tool.

Fusion will then display the total length in the lower right corner.

The total path distance is 303.955mm.

Notice the faces currently all match the original. To make them follow the path, switch the Orientation from Identical to Path Direction.

This forces the object to follow the contour of the path.

Here’s another pro tip: check the Suppression option in the dialog, as you don’t need many of the patterns, including those on the height of the doorstop.

This allows you to uncheck any instances that you want to exclude.

Take a minute to uncheck all of them on the left side.

Uncheck the ones that are too close to the corner edges as well.

Click OK to save the pattern.

A quick note on this design. This design works best if you print it in TPU filament. Its unique combination of flexibility and high friction allows it to grip smooth floors while also absorbing impact without cracking.

Experiment with the grip shape, using rounded shapes for hard floors or sharp triangles for carpet.

Let’s now add some final structure to the inside cavity.

Right-click on the top face and select Create Sketch.

Activate the Circle tool. Sketch a large 30mm circle anywhere on the left. We’ll constrain this in a second.

With the circle still active, create a second circle with a diameter of 15mm, clicking to place it anywhere on the right.

Activate the Tangent Constraint tool. This allows you to force the circle to remain tangent with the inside edges.

Select the larger circle and the top inside edge.

Notice the tangent glyph, which shows the circle is now tangent to the inside edge.

Click the circle again, followed by the bottom inside edge.

This fully constrains the circle.

Take a minute to repeat these steps to add the tangent constraints to the 15mm circle.

This fully defines the sketch and ensures the circles don’t move. Using a Tangent constraint is better than adding a dimension to the edge. If the wall moves, the circles will stay touching the wall.

Activate Extrude and once again switch to the Thin Extrude option in the dialog.

Select both circle profiles. Very important: When using Thin Extrude, ensure you select the sketch geometry – the lines or curves – rather than the shaded area inside the profile.

Similar to the grip pattern, use the ‘To Object’ extent type.

Select the bottom face as the extrusion target.

Change the Wall Thickness to 4mm to match the outer wall thickness.

Notice, however, that the circles extrude to the inside so they just barely contact the inner walls of the triangle.

In the Extrude dialog, change the Wall Location to the Center option. This adds thickness on both sides of the selected profiles.

Very important: A software bug may reset the Extent Type when you change the wall location.

First, set the operation to Join to create a single body for 3D printing. Reset the Extent Type to To Object, then select the bottom face.

Notice Fusion now applies the wall thickness to both sides of the circle profiles.

Click OK to save the Extrude.

Before exporting for 3D printing, add some final Fillets to strengthen the connections where the circles meet the triangle.

Activate Fillet and select the four inside connections where the larger circle meets the triangle.

Define this fillet radius as 3mm.

Add a new selection set in the Fillet dialog. Repeat the steps for the smaller circle, but define this fillet radius as 2mm.

Click OK to save the Fillet.

Fusion supports many ways to export your models for 3D printing.

Most slicers, including Bambu Studio, Prusa, and Cura, now support STEP files.

While STL and 3MF files break your design into thousands of flat triangles, a STEP file preserves the original mathematical curves.

This gives you perfectly smooth surfaces without any “faceting” and helps your slicer identify holes and features for custom settings.

Right-click the top-level Part in the Browser and select the Export option.

Choose the STEP file type and save your design to your local hard drive.

You can then open it in your preferred slicer program.

I’ll share recommended print settings on the resource page.

You will also see the Save as Mesh option in the right-click menu.

This allows you to send mesh files directly to your 3D printing slicer.

Check out the video linked in the description to learn more about that workflow.

I’ll see you on Day 9, where you’ll learn how to use Fusion’s Primitive shapes to create a standard light bulb.