Sine Wave Fan Grille in Fusion – Step-by-Step Tutorial
Complex shapes in Fusion often become easier to manage when you combine solid modeling and surface modeling. This workflow shows how to create a curved fan grille using sine-wave geometry while keeping the model clean and flexible.
The result is a design that is well suited for 3D printing and demonstrates several powerful Fusion tools working together.
What You’ll Learn
- How to structure a fan grille using sketch-driven geometry
- When to use surface tools instead of solid tools
- How rectangular patterns can simplify repeated geometry
- How to shape curved surfaces using fit point splines
- A workflow for combining bodies and fixing design errors
- Practical considerations when preparing models for 3D printing
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 the Frame Sketch
Press S to open Sketch Shortcuts, which allows you to quickly access commonly used commands without navigating the ribbon menus.
Create a center rectangle and set the dimensions to 120 × 120 mm.
This rectangle defines the outer frame of the fan grille. Structuring the sketch this way helps keep the rest of the geometry organized because most features will be built relative to this boundary.
Using a central frame also makes the design easier to scale later if you need a different grille size.
Center rectangle sketch defining the overall frame size of the fan grille. This base geometry establishes the main reference for positioning the circular airflow opening and mounting holes in the design.
Step 2: Define the Main Circular Opening
Press C and create a center diameter circle at the origin.
Set the diameter to 100 mm.
Placing the circle at the origin ensures that the model remains centered and symmetrical. This is important when the design later relies on patterned geometry and revolve operations.
A centered design is generally easier to manage when exporting for 3D printing or manufacturing.
Circle sketch created inside the square frame to define the airflow opening. This circle later controls the boundary where the patterned grille geometry will be trimmed.
Step 3: Add the Mounting Holes
Move to one corner of the frame and press C again to create a mounting hole.
Set the diameter to 5 mm.
Press D and dimension the hole 10 mm from the outer frame edges.
The exact placement of the hole does not need to be precise during creation because the dimension controls the final position. This approach keeps sketches fast to build while maintaining accuracy.
First mounting hole positioned along a diagonal construction line. Using construction geometry ensures the hole is correctly located relative to the frame corners and center.
Step 4: Pattern the Mounting Holes
Instead of manually creating four holes, use a Rectangular Pattern in the sketch.
The frame is 120 mm wide and the holes are 10 mm from each edge, so the pattern extent becomes: 120 − 10 − 10 = 100 mm
Set the pattern extent to 100 mm in both directions and the quantity to 2.
This instantly creates four mounting holes.
Although this could also be done later in the solid modeling environment, using a sketch pattern is quick for simple geometry. However, it is worth noting that models built with user parameters and feature patterns are often easier to edit later.
Rectangular pattern used to duplicate the mounting hole to all four corners of the frame. This keeps spacing consistent and avoids manually creating multiple identical holes.
Step 5: Round the Frame Corners
Open Sketch Shortcuts again and choose Sketch Fillet.
Set the radius to 5 mm and apply it to all four corners.
Be careful here:
F activates the solid Fillet tool, not the sketch fillet.
Adding these fillets directly in the sketch simplifies later operations because the extrusion will automatically inherit the rounded corners.
Sketch fillets applied to the frame corners to soften the geometry. Rounded corners improve the appearance and reduce stress concentrations when the part is manufactured.
Step 6: Build the Sine Wave Structure
Create a sketch line through the center of the circle.
Then add a short 3 mm line at the endpoint. These two lines form the structural foundation for the sine wave geometry.
This simple setup defines both the direction and the shape influence for the surface sweep that will follow.
Completed base sketch showing the square frame, circular opening, mounting holes, and a construction line running through the circle. A short 3 mm line at the endpoint defines the profile used for the upcoming sine wave sweep.
Step 7: Create the Sine Wave Surface with Sweep
Switch to the Surface workspace and choose Sweep.
Surface modeling is useful when working with open profiles and flowing geometry that would otherwise be difficult to create with solid tools alone.
A quick tip:
- Blue icons represent solid modeling tools
- Orange icons represent surface modeling tools
If selecting profiles becomes difficult due to overlapping geometry, press and hold the left mouse button to access the selection priority list.
Use the straight line through the circle as the path.
Set the Twist Angle to: 360° × 5
After entering 360 degrees, click the input field again and multiply by 5 to complete the twist value.
This twist creates the characteristic sine wave motion around the circular path.
Selecting both profiles at the end of the line and then selecting the line as the sweep path in Autodesk Fusion to define the geometry for the sweep operation.
Sweep preview showing the sine wave profile following the path across the grille opening.
Step 8: Extrude the Surface
Create a new sketch on the flat construction plane.
Press S and use Project to project the edges of the sine wave surface into the sketch.
Now use Surface Extrude (orange icon) and extrude the geometry 10 mm.
Surface extrusions are ideal here because the sine wave structure begins as a thin surface before gaining thickness.
Projected sine wave geometry onto a sketch to reuse the curve for later modeling steps.
Surface extrude applied to the sine wave sketch to generate a thin airflow rib.
Step 9: Add Thickness to the Surface
Apply the Thicken command and set the operation to Symmetric.
Use 1 mm thickness for the digital prototype.
For real 3D printing, a thicker value may be necessary depending on:
- the filament used
- nozzle size
- mechanical strength requirements
PETG or ASA prints often benefit from slightly thicker walls for durability.
Thicken feature converting the sine wave surface into a solid rib for the grille.
Step 10: Create the Base Body
Press E for Extrude and extrude the remaining profile as a New Body.
Because the mounting holes and corner fillets were defined earlier in the sketch, this extrusion becomes straightforward. Most design decisions have already been encoded into the sketch structure.
This is a common modeling strategy in Fusion:
push complexity earlier into sketches to simplify later features.
Square frame extruded to create the main body of the fan grille.
Step 11: Pattern the Sine Waves
Instead of patterning the sketch geometry, use a solid modeling Rectangular Pattern.
One benefit of this approach is that the pattern appears as a single feature in the timeline, making it easier to manage and edit later.
Set the pattern direction to Symmetric and change the distribution to Spacing.
Enter a spacing interval that fits the design.
Some waves will intersect the body at this stage. That is expected and will be resolved later.
Rectangular pattern replicating the sine wave rib across the circular airflow opening.
Step 12: Shape the Curved Top Surface
Create a Fit Point Spline.
This spline defines the curvature of the top surface.
Fit point splines are ideal for shaping surfaces because they provide flexible control points and handles. Small adjustments can significantly change the visual smoothness of the final geometry.
Extend the spline well beyond the base body. Oversketching ensures the curve reaches the corners when cutting the shape later.
Fit point spline used to refine the sine wave shape for smoother airflow geometry.
Step 13: Create the Revolve Cut Tool
Extrude the spline symmetrically to create a surface. Then apply Thicken to convert it into a solid body.
This solid body is used as the tool body in the next step. Activate Revolve, set the operation to Cut, and revolve it 360 degrees around the center axis.
That removes material and forms the rounded top surface of the fan grille.
Surface modeling Extrude applied to the sine wave sketch to create a surface body. This surface will later be thickened to form a solid body that can be used to cut away geometry from the main part.
Thicken applied to the surface body to create a solid body that extends higher than the final design requires. Making the body taller than needed simplifies the modeling process and ensures the upcoming cut operation removes the correct geometry without needing precise height adjustments.
Revolve cut used to trim the patterned ribs to the circular grille boundary.
Step 14: Combine Bodies and Check the Design
Turn off sketch visibility and run the Combine command.
Select all sine wave bodies as tool bodies and finish the operation as a New Component.
Switch to Top View and perform a quick visual inspection.
You may notice a small issue:
one sine wave intersects a mounting hole.
Catching issues like this early is part of good modeling practice.
Combine command merging patterned ribs and frame into a unified grille body.
Step 15: Fix the Geometry Error
Return to the timeline and add a Split Body operation to separate the problematic section.
Instead of updating the original Combine feature, delete it and create a new Combine operation that excludes the unwanted geometry.
Also remove the component created by the previous Combine step.
This iterative approach keeps the timeline clean and prevents feature conflicts later.
Split Body tool used to divide the top sine wave where it intersects with the mounting hole area. This split separates the portion that would collide with the hole so it can be excluded in the final combine operation, helping refine the grille structure before completing the model.
Timeline edit removing an incorrect feature to correct the parametric workflow.
Final Combine operation producing the completed fan grille body. The section of the top sine wave that intersects with the mounting hole is intentionally not selected in the combine operation so the mounting hole remains clear and functional.
Finished sine wave fan grille design optimized for 3D printing.
Key Takeaways
- Combining solid and surface modeling opens up more flexible design workflows in Fusion.
- Structuring sketches carefully early in the process simplifies later operations.
- Surface Sweep + Thicken is a powerful method for creating complex curved structures.
- Using feature patterns instead of sketch patterns often makes designs easier to edit later.
- Always perform visual checks after combine operations to catch geometry conflicts early.
- Iteration is normal in parametric modeling — refining the design through the timeline is part of the process.
If you want to explore another approach to modeling fan grilles, check the linked tutorial below. It uses a different strategy and has received strong engagement from the Fusion community.
🧰 Tools & Deals
I’ve gathered some of the tools, software, and gear I personally use and recommend for CAD work, 3D printing, and making things in one place. Some links may include discounts or special offers that can help you level up your workflows.
Please note: some of the links are affiliate links, which means I may earn a small commission at no extra cost to you. This helps support the site and the creation of free Fusion tutorials.
Explore everything here:
The Maker Letters – Tools & Deals
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⏱ Chapters
- 01:05 Rectangular Pattern Setup for Mounting Holes
- 02:15 Sketch Setup for a Parametric Sine Wave
- 02:51 Creating the Sine Wave Geometry
- 04:11 Surface Sweep + Extrude: Building the Sine Wave Structure
- 05:16 Rectangular Pattern of the Sine Wave Bodies
- 05:49 Sketching the Curved Top Surface with a Fit Point Spline
- 07:12 Shaping the Fan Grille Using Revolve Cut
- 08:04 Combine Bodies and Detect a Hidden Modeling Error
- 09:00 Fixing the Error by Editing the Timeline
- 10:28 Recommended Tutorial: Another Fan Grille Workflow
You Might Also Like
If you enjoyed this Fusion project, here are three related tutorials that explore honeycomb structures, surface modeling workflows, and practical design techniques for 3D-printable parts.
Learn how to combine parametric sketches, patterned geometry, and surface tools to design a strong and lightweight fan grille ready for 3D printing.
🧩 Master Surface and Solid Modeling in FusionUnderstand how surface and solid modeling work together in Fusion and why combining both approaches can simplify complex designs.
🐝 Create a Honeycomb Pattern in Fusion (Step-by-Step Guide)Follow a clear workflow for building a parametric honeycomb pattern that can be reused in many designs such as vents, grilles, and lightweight structures.
Together these tutorials show how parametric sketches, patterns, and surface tools can be combined to create strong, efficient geometry for real-world designs and 3D printing projects in Fusion.