Faster Modeling in Fusion: Create a Parametric Honeycomb Pattern Step-by-Step
Create a Clean, Parametric Honeycomb Design in Fusion
If you want to model faster and keep your designs perfectly aligned, this technique will help you save time and get it right on the first try. It’s a clean, repeatable approach that works great for honeycomb-style projects and other patterned designs — ideal for 3D printing or manufacturing applications.
What You’ll Learn
This project builds on simple sketching and pattern tools in Fusion to create a clean, parametric result ready for 3D printing.
You’ll learn how to:
- Sketch with precision using the Polygon tool
- Control wall thickness with the Thin Extrude feature
- Create symmetric honeycomb patterns for even spacing
Every step stays fully parametric — meaning your entire design updates automatically when you change a single dimension.
Watch the Workflow — or Read It Step by Step
You can follow this guide in two ways:
- Read the steps below if you want quick written instructions, reference images, and modeling notes.
- Watch the full video at the end of this post to see the workflow in real time — including extra tips, camera angles, and shortcuts that don’t fit neatly into text.
Both formats build on each other.
Reading helps you understand why each step matters, while watching shows how to move faster in Fusion.
Step 1 — Create a New Sketch
Start by using the design shortcuts (S key) to create a new sketch.
A centered sketch makes it easy to keep the model symmetrical as it grows.
Keeping your origin visible helps ensure every step stays aligned later.
Fusion interface showing the creation of a new sketch on the top plane using the design shortcuts menu.
Step 2 — Add a Circumscribed Polygon
Add a circumscribed polygon right at the center of the canvas.
Use a 10-millimeter radius for this example.
A circumscribed polygon defines its radius from the center to the outer points — this makes it ideal for pattern-based designs because you can control the outer size precisely and repeat it with predictable spacing.
Sketch environment in Fusion with the polygon tool selected and circumscribed polygon highlighted.
A hexagon sketch centered on the origin, dimensioned with a 10 mm radius.
Step 3 — Draw a Midpoint Construction Line
Next, draw a construction line that snaps to the midpoint of one polygon side.
We’ll use this line later as a guide for our rectangular pattern.
The reason for this step is accuracy — snapping to the midpoint guarantees that the pattern spreads evenly on both sides of the center, keeping the geometry symmetric and predictable.
A construction line added from the center of the hexagon to the midpoint of one side.
Step 4 — Extrude with a Thin Feature
Now, extrude the polygon to any height.
In this example, we’ll use five millimeters.
Turn the extrude into a Thin Feature and set your wall thickness to one millimeter.
Using a thin extrude instead of a solid makes it easier to control wall thickness — especially for designs intended for 3D printing or lightweight structures.
It also keeps the honeycomb edges consistent across repeated features.
Extrude preview showing the hexagon turned into a solid body with a 5 mm height.
Step 5 — Create a Rectangular Pattern
Then, create a Rectangular Pattern.
Use the construction line you drew earlier as the direction, and align it with the green axis.
This ensures the pattern moves in a perfectly straight, controlled direction.
Because the guide line was drawn from the midpoint, the pattern remains centered on the origin — no manual alignment needed.
The solid hexagon body is ready in the Fusion workspace, with origin planes active before applying the rectangular pattern.
Rectangular pattern command opened, with one direction axis selected and spacing options visible.
Step 6 — Adjust the Pattern Settings
Change the Pattern Type to Spacing.
Set the distance to 19 millimeters for a slight overlap that matches the wall thickness.
Finally, set the Direction to Symmetric for even spacing on both sides.
Why 19 millimeters?
It comes from the formula:
19 = (10 mm × 2) – 1 mm
🟡 Polygon Radius × 2 – Thin Extrude Thickness
This formula keeps each shape close enough to form a continuous pattern without gaps — essential for a clean, printable honeycomb.
Pattern tool with both axes selected and spacing set to 19 mm for symmetrical distribution.
Distribution direction switched from one-direction to symmetric in the rectangular pattern settings
Step 7 — Result and Benefits
The result is a clean, precise pattern that stays parametric.
That means every dimension stays linked — if you change the polygon radius or thickness, Fusion automatically updates the spacing and alignment.
It’s a quick, reliable workflow that saves time and avoids the small errors that come from manual spacing or re-sketching.
Final view of the hexagon array forming a clean, repeating honeycomb structure.
Key Takeaways
- Use construction lines wisely: A simple construction line can guide your pattern without becoming part of the geometry. It keeps everything centered, aligned, and easy to adjust later.
- Thin extrude is efficient: Turning your extrude into a thin feature saves sketching time and gives you precise wall control — perfect for clean, printable results.
- Symmetry saves effort: Setting the pattern direction to Symmetric ensures even spacing on both sides, reducing manual adjustments and keeping the design balanced.
These small habits make your modeling faster, cleaner, and easier to refine — especially when working with repeating patterns or 3D printable designs.
⏱ Chapters
00:11 — Quick Sketch Setup with Shortcuts
00:22 — Add a Circumscribed Polygon
00:37 — Add a Midpoint Construction Line
00:51 — Use Thin Extrude for the Polygon
01:01 — Set the Wall Thickness
01:11 — Create a Rectangular Pattern
01:40 — Adjust Distance, Direction & Quantity
02:13 — More Fusion Videos from The Maker Letters
You Might Also Like
If you enjoyed this Fusion tutorial, here are three more projects tailored for honeycomb patterns in other situations — each offering unique modeling approaches and printable design ideas.
Each tutorial explores a different use case for honeycomb geometry — from surface-based patterns to solid modeling applications — helping you choose the best technique for your next design.