How to Create a Fan Grille with a Honeycomb Pattern in Fusion
Fusion, formerly known as Fusion 360, is a powerful tool for 3D modeling and design. Creating this computer fan grille is a great way to blend surface and solid modeling. And if you have workflow tips, drop them in the comments. A step-by-step video tutorial is included at the bottom of this post.
Step 1: Setting Up the Component and Sketch
Start by creating a new, activated component. Then, create a sketch to define the boundaries of your grille. Using a center rectangle keeps the design centralized above the origin. Set dimensions to 120 × 120 mm, but adjust them as needed.
Next, sketch a single hole instead of four, as solid modeling features will generate the others. This keeps the design flexible. Add dimensions for quality control and easier pattern creation later. Also, create a center-diameter circle in the middle—this will serve multiple purposes.
Step 2: Creating the Honeycomb Pattern Sketch
Start a second sketch to isolate the honeycomb pattern. Use the same construction plane as before. Sketch a circumscribed polygon at the center, then add two construction lines: one vertical and one at a 45-degree angle. Convert them into construction lines to avoid interference.
Select the Rectangular Pattern tool designed for sketches. Choose the polygon first, then use the two construction lines as direction guides. Set the spacing slightly over 10 mm to ensure a well-proportioned pattern and use the Symmetric option for direction.
This separate sketch approach allows for oversketching and refining the pattern later.
Step 3: Preparing the Extrusions
Instead of extruding the polygons, extrude the area between them. Use the Project tool to link the circle from Sketch 1 into Sketch 2 to align elements.
Now, extrude the area between the rectangle and the circle from Sketch 1 to 10 mm. Hide Body 1, turn on Sketch 2, and ensure the projected circle is a regular line (not a construction line). Then, extrude the honeycomb pattern up to Body 1’s top to maintain adaptability in the Fusion timeline. Set this as a New Body operation for flexibility.
Step 4: Creating the Rectangular Pattern for Holes
Before adding complexity, create the rectangular pattern for the holes while the model remains simple. Set the object type to Faces and select the hole’s face. Use both axes to distribute the pattern evenly. Since the total width is 120 mm with a 10 mm edge gap, setting the total extent to 100 mm ensures even spacing.
Step 5: Adding Fillets for Smooth Corners
Filleting early keeps the process simple before adding curvature. Select all sides, switch to the Top View, and apply the fillet. This step can be adjusted later in the timeline.
What are the pros and cons of filleting now versus later? Share your thoughts in the comments!
Step 6: Adding the Curved Shape
Create a new sketch on the central construction plane. Use the Fit Point Spline to design a smooth curve. The green handlebars help refine the curvature. Extend the spline beyond the model to cover the corners in the next step.
Extrude the spline minimally to create a surface for thickening. Then, use a Revolve Cut operation to trim away parts around the model, ensuring the corners are cut properly.
Step 7: Finalizing and Exporting
Creating the grille around the central axis makes selections fast and precise. Hide any unnecessary parts and explore appearance options. A glossy plastic look works well and is 3D printable.
Since the honeycomb pattern was created as a separate body, you can color each body differently if needed.
Watch the Full Tutorial
For a detailed walkthrough, watch the video tutorial below. This visual guide will help you follow along and apply the steps in Fusion.