Mastering Surface and Solid Modeling in Fusion
Updated February 23, 2026
Autodesk Fusion, formerly known as Fusion 360, offers powerful tools for blending surface and solid modeling. In this tutorial, we’ll explore a workflow that simplifies complex designs. If you watch the full video below, keep an eye on the keyboard shortcuts in the bottom left corner of the screen.
What You’ll Learn
- How to set up reference sketches on construction planes for controlled surface workflows
- How to build a parametric honeycomb pattern using sketch patterns and spacing logic
- How to extract the negative space between profiles to define the pattern geometry
- How to use Surface Extrude with symmetric direction to create a controlled base surface
- How to apply Intersect to trim patterns cleanly against surface geometry
- How to convert thin surface geometry into solids using Thicken
- How to replicate geometry efficiently with Circular Pattern
- How to refine edges and symmetry using fillets and mirror workflows
- How to assign materials and combine bodies for final presentation
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: Laying the Foundation
Begin by creating a new component, followed by a sketch on a vertical construction plane. Using a circumscribed polygon ensures precise alignment. Starting at the origin keeps it centered on the horizontal construction plane, which will be useful later. A 5 mm distance results in a polygon with a total height of 10 mm.
Using a mouse with a scroll wheel makes zooming easier. Activate Construction Line mode and create two guide lines for the honeycomb pattern. Fusion helps snap the second line to the middle of the polygon’s side with a small symbol indicating the correct alignment.
New component created in Fusion to structure the model hierarchy before starting the honeycomb sketch workflow.
Circumscribed polygon created in Fusion to define the base hex cell for the honeycomb pattern.
Construction guide lines aligned to polygon edges to control direction and spacing of the honeycomb pattern in Fusion.
Construction guideline snapped to the midpoint of a polygon side in Fusion to control honeycomb alignment and pattern direction.
Step 2: Patterning the Design
Select Rectangular Pattern in the sketch environment—the option with unfilled symbols. Include the entire polygon and use both construction lines for direction. Set distribution to Spacing and direction to Symmetric for a balanced layout.
A small gap between polygons is necessary. Since half the polygon is 5 mm, the total height is 10 mm. Increasing the spacing slightly above 10 mm ensures the proper separation.
Rather than calculating the exact number of polygons now, generate more than needed and refine the design later. While it may seem excessive initially, this workflow ensures flexibility as the design evolves.
Rectangular sketch pattern applied to propagate the hex cell across the work area with symmetric spacing.
Rectangular sketch pattern used to generate more honeycomb cells than needed, allowing flexible trimming and refinement later in the workflow.
Step 3: Creating the Base Shape
The key focus is not the polygons themselves but the space between them. A 2-point rectangle captures this space efficiently. Aligning with the grid allows for quick positioning, but dimensions can refine placement for precision.
If construction lines were left on, they appear as dashed lines. Select the rectangle and convert these to regular lines. This creates a closed profile forming the base of the pattern.
Rectangle sketched to capture the negative space between honeycomb polygons, defining the cutout geometry used for the pattern.
Step 4: Setting Up Measurements
The height from the middle to the top is 22 mm, giving a total height of 44 mm. Create a sketch on the horizontal construction plane and draw a center diameter circle at the origin. This circle forms a thin cylinder that defines the pattern’s structure. A 75 mm diameter maintains balance with the polygon pattern.
Use the Surface Extrude command on the circle. Set direction to Symmetric with a total height of 44 mm. The measurement setting can define either the full or half length—verify it matches your intent. A quick check with the ViewCube confirms the cylinder is correctly positioned.
Measuring the rectangle that captures the negative space between honeycomb cells to set consistent pattern height before creating the base surface.
Center diameter circle sketched at the origin in Fusion to define the base profile for the cylindrical surface used in the honeycomb intersect workflow.
Surface extrude set to symmetric in Fusion to create the thin cylindrical surface used as the base for intersecting the honeycomb pattern.
Step 5: Extruding the Pattern
Save your project regularly. Then extrude the honeycomb pattern. Adjusting the rectangle’s size allows future scaling, and the timeline keeps this workflow flexible.
Extrude the pattern through the surface model and set the operation to Intersect. This retains only the intersected areas, removing the rest and leaving an infinitely thin pattern.
Honeycomb pattern extruded and intersected with the cylindrical surface in Fusion to trim the pattern to the bracelet form.
Step 6: Transforming the Design into a Solid Model
Convert the pattern into a solid using the Thicken command. A 2 mm thickness provides structural definition while keeping the model lightweight.
Apply a Circular Pattern to replicate the design around an axis. Since the layout is centralized, the axis serves as a natural reference. Instead of calculating the exact count, increase the number until the pieces align, matching the blue original object with the grey patterned copies.
Use the ViewCube to verify alignment. Minor adjustments may still be required.
Thicken command used in Fusion to convert the thin honeycomb surface into a solid model with defined wall thickness for 3D printing.
Circular pattern applied in Fusion to replicate the honeycomb segment around the bracelet axis for full circumference coverage.
Step 7: Refining the Design with Additional Features
Sketch directly onto the existing body to create the top ring. This ring defines the edge profile of the bracelet and sets up the geometry that will later be mirrored to form a matching bottom ring.
At this stage, the design remains flexible, although it does not yet use user parameters or constraints. These are useful for controlled adjustments but fall outside the scope of this tutorial.
Circle sketched on the bracelet rim in Fusion, matching the bracelet diameter to define the top ring profile.
Offset curve applied to the top ring sketch in Fusion to control ring width and wall thickness.
Top ring profile extruded in Fusion to add a reinforced rim and clean edge to the honeycomb bracelet.
Step 8: Using Fillets and the Mirror Command
Apply a full round fillet before mirroring the top to save time. A parametric fillet updates automatically if top dimensions change. This workflow highlights the benefit of symmetry around the horizontal construction plane and the advantage of keeping the top as a separate body.
Select the object, choose the Mirror plane, and set the operation to New Body. This approach makes achieving precision in Fusion more predictable and efficient.
Full round fillet applied to the top ring in Fusion to create a smooth, continuous edge on the honeycomb bracelet.
Mirror operation used in Fusion to duplicate the top ring body and create a matching bottom ring on the honeycomb bracelet.
Step 9: Applying Materials and Finalizing the Design
Refine the appearance by assigning materials. Since the bodies are not yet merged after the circular pattern, different colors can be applied to different parts.
If a single body is preferred, select all bodies, activate Combine, and merge them into one solid directly in the Browser.
Different appearances applied to individual honeycomb bracelet bodies in Fusion to visually inspect alignment and segmentation before combining.
Combine command used in Fusion to merge all honeycomb bracelet bodies into a single solid model ready for export.
Key Takeaways
- Prepare surface geometry before applying lofts or intersects
- Model negative space, not just solid profiles
- Use construction geometry to control alignment and symmetry
- Apply Intersect to trim patterns cleanly against surfaces
- Convert surfaces to solids late in the workflow
- Delay circular patterns until the core form is correct
- Apply fillets before symmetry to reduce rework
🧰 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:
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📌 Chapters
⏱️ 00:14 Sketching a Polygon for a Honeycomb Pattern
⏱️ 00:38 Creating a Honeycomb Pattern Sketch in Fusion
⏱️ 02:52 Measuring for Precision in Fusion
⏱️ 03:10 Extruding a Circle with Surface Modeling
⏱️ 04:08 Applying a Pattern to a Surface Model
⏱️ 04:41 Converting a Surface Model into a Solid Body
⏱️ 04:57 Creating a Circular Pattern in Fusion
⏱️ 05:36 Adding a New Body on Top of Another
⏱️ 06:30 Using Parametric Fillets for Adjustable Edges
⏱️ 06:49 Mirroring a Body in Fusion
⏱️ 07:18 Assigning Different Appearances to Bodies
⏱️ 08:02 More Fusion Tutorials from The Maker Letters
You Might Also Like
If you enjoyed this Fusion tutorial, here are three more projects that dive deeper into honeycomb patterns, pattern-based design, and building clean, 3D-printable geometry in Fusion.
Together, these tutorials build on the same core ideas used here — constructing repeatable honeycomb geometry, controlling pattern spacing, and turning CAD workflows into practical, 3D-printable designs you can adapt across different projects.