How to Create a Honeycomb Pattern in Fusion: A Step-by-Step Guide
You can find the full video tutorial linked at the bottom of this post.
Honeycomb patterns aren’t just visually stunning—they’re incredibly practical in 3D design. In this tutorial, you’ll learn how to create a reusable honeycomb pattern in Fusion that works with all kinds of shapes and forms.
By the end of this guide, you’ll know how to design, modify, and customize honeycomb patterns for your own projects. Whether you’re building lightweight panels, decorative designs, or functional parts for 3D printing, this workflow will save you hours of work.
Why Use a Honeycomb Pattern?
The honeycomb structure is lightweight, strong, and efficient—perfect for reducing material use while maintaining strength. It’s widely used in aerospace, architecture, and 3D printing. And in Fusion, you can create a parametric version that updates automatically when you change dimensions.
Step 1: Set Up Your Design Environment
Start by creating a new component in Fusion and making it active. Then, create a sketch on the horizontal construction plane.
Draw a polygon centered at the origin. This keeps your design clean and symmetrical.
Set the radius to 5 mm for this tutorial.
Draw two lines from the origin to guide the honeycomb pattern. Snap one to the midpoint of a polygon side.
Convert these lines into construction lines for reference.
Once done, extrude your sketch 4 mm to form a solid body.
Step 2: Build the Honeycomb Pattern
Turn the sketch visibility back on in the browser—it’s essential for the next steps.
To create the pattern:
Change Object Type to Bodies if the solid polygon isn’t selectable.
Select both construction lines.
Set Distribution to Spacing and Direction to Symmetric for Axis 1 and Axis 2.
Remember: The distance between polygon centers isn’t the polygon radius. For a 5 mm radius, the center-to-center distance is about 8.66 mm. In this example, we’ll round it slightly to 9 mm for simplicity.
Increase the quantity of polygons until the pattern fully covers your planned shape. Creating extra elements now lets you trim excess later.
Step 3: Define the Outer Shape
Next, sketch the outer shape of your design:
Start a new sketch on the horizontal plane.
Draw a center diameter circle at 100 mm.
Offset a second circle for a border thickness of 1 mm (final diameter: 102 mm).
Align these circles to the honeycomb pattern for a clean edge.
Step 4: Trim the Pattern to Shape
With your sketch ready:
Extrude it up to the top of the honeycomb pattern.
Turn off sketch visibility for easier selection.
Set your new body as the Target Body, and all honeycomb polygons as Tool Bodies.
Change the operation type to Cut.
This trims the honeycomb to your circular boundary.
Step 5: Add an Outer Border
To strengthen your design and add a clean edge:
Use Surface Extrude on the outer circle.
Apply the Thicken command for both inner and outer circles (1 mm thickness).
Make sure the inner border thickness is applied inward to avoid overlapping the honeycomb pattern.
Step 6: Refine with Fillets and Join Bodies
Adding fillets improves appearance and user experience—especially for 3D-printed objects. Select all exposed edges and apply a small radius.
When ready, join all bodies together:
Select your border as the Target Body.
Select all other parts as Tool Bodies.
Change the operation type to Join.
This simplifies your project and reduces clutter in the browser.
Step 7: Apply Finishing Touches
Before exporting for 3D printing, assign appearances to your model. Fusion’s library lets you preview materials and colors digitally.
Pro tip: Search for styles like glossy or matte, or combine with colors (e.g., “glossy yellow”) for faster results.
Bonus: Make Your Design Parametric
Since we built the honeycomb and outer shape using constraints and references, adjusting dimensions later automatically updates the whole design. This makes your pattern reusable for multiple projects.
Final Thoughts
This project demonstrates how to combine solid and surface modeling to achieve a clean, professional result. From concept to final fillets, you now have a versatile honeycomb pattern you can adapt to almost any shape.
Thank you for reading!
Chapters in the Fusion tutorial below:
00:10 Create a New Component to Keep Your Design Organized
00:26 How to Make a Honeycomb Pattern in Fusion (formerly Fusion 360)
00:36 Sketching the Base Polygon for Your Pattern
00:54 Add Help Lines for Pattern Alignment
01:05 Convert Sketch Lines to Construction Lines
01:15 Extrude to Create the First Solid Polygon
01:30 How to Unhide Your Sketch in Fusion
01:45 Set Up a Rectangular Pattern Using Custom Axes
02:07 Symmetric Pattern Distribution and Direction Explained
02:21 Understand Distance Settings for Accurate Pattern Layout
03:01 Adjust Quantity Settings for Honeycomb Coverage
03:17 Sketch the Outer Shape for Your Final 3D Body
03:30 Select Geometry at Depth in Crowded Sketches
03:44 Draw and Offset Circles for the Honeycomb Edge
04:25 Extrude the Circular Shape to Match the Pattern Height
04:40 Hide Sketches to Clean Up Your Workspace
04:55 Use Combine and Cut to Shape the Pattern
05:22 Add Edges Around the Honeycomb Pattern
05:33 Use the Surface Modeling Extrude Tool
05:49 Thicken Surfaces to Create a Solid Frame
06:26 Add Fillets to Improve Looks and Durability
06:55 Combine Bodies to Simplify Your Design
07:28 Add a Glossy Appearance for a Realistic Look
07:49 More Fusion Video Recommendations from The Maker Letters