Design a 3D-Printable Hexagon Pot in Fusion
Updated March 15, 2026
Watch the full Fusion Tutorial at the bottom of this blog post:
Looking for a great 3D-printed gift or a product to sell online? This hexagon pot is both stylish and functional. In this tutorial, we’ll walk through the entire process in Fusion, from sketching the base to finalizing the design for 3D printing.
What You’ll Learn
- How to set up stacked sketches on different planes to control the overall shape of the model.
- How to create geometry efficiently using surface lofts and circular patterns instead of modeling every face manually.
- How to close open surfaces with the Patch tool and convert the surface model into a solid body using Stitch.
- How to refine the model with Shell and Fillet to create a clean, 3D-printable hexagon pot.
- How to apply materials and render the model in Fusion’s Render workspace.
- How parametric modeling lets you modify dimensions and automatically update the entire design.
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: Setting Up the Sketches
Every great Fusion project starts with a new component. This keeps your design organized and makes future edits easier.
We begin by creating two polygon sketches at different heights along the Z-axis. First, we’ll use a circumscribed polygon, centered at the origin, with a diameter of 100 mm. Feel free to tweak the dimensions—customization is a great way to learn.
Next, instead of closing the sketch environment, we activate the Offset Plane command, setting an offset of 50 mm to create the base for our second sketch. This time, we’ll use an inscribed polygon, also centered at the origin, positioned 50 mm above the first polygon. Now, we have two stacked polygon sketches—ready for lofting.
The project begins by creating a new component for the vase. Working inside a dedicated component keeps sketches, bodies, and construction geometry organized and prevents later features from accidentally referencing geometry outside the design. This also makes the model easier to reuse in larger assemblies or parametric projects.
A hexagon sketch defines the base profile of the vase. The polygon is centered on the origin so the model stays symmetric and easier to control parametrically. Using the origin as a reference helps ensure that later features such as lofts, mirrors, and patterns align correctly without extra constraints.
An offset construction plane is created above the base sketch. This second reference plane will hold another sketch used for the loft operation. Construction planes allow you to control vertical spacing between profiles, which directly influences the curvature and proportions of the final form.
A second hexagon is sketched on the offset plane using a circumscribed polygon. The orientation of this polygon relative to the lower one controls how the triangular faces twist around the vase. Small changes in rotation or size here can significantly change the final surface structure.
Step 2: Lofting the Surfaces
Instead of lofting every side manually, we take a more efficient approach. By lofting a single edge from the lower polygon to a midpoint on the upper polygon, we ensure precise alignment.
After lofting the first surface, we use the circular pattern tool to distribute it evenly around the model. With the blue axis at the center, selecting the correct rotation point is simple. Setting the pattern to six instances completes the shape.
While I could have patterned two lofted surfaces at once, demonstrating each step separately makes the process clearer. Once you’re comfortable, combining steps will speed things up.
The Loft tool connects profiles from the lower and upper sketches to create the first triangular face of the vase. Lofting between polygon edges produces faceted surfaces that form the distinctive geometric pattern. Starting with one face keeps the model simple before duplicating the geometry later.
The Circular Pattern tool duplicates the first lofted face around the central axis. Patterning bodies instead of sketch geometry keeps the sketches lightweight and easier to edit later. This approach also allows individual faces to remain independent bodies during early modeling stages.
Multiple triangular loft faces now surround the vase. At this stage the geometry is still made of separate surfaces or bodies. Working with individual elements first makes it easier to troubleshoot geometry before combining everything into a single watertight model.
The patterned loft faces now form the full outer structure of the vase. Each triangular panel contributes to the faceted appearance. Patterns are particularly useful for geometric designs because they guarantee consistent spacing and angles around the entire model.
Step 3: Sealing the Model with the Patch Command
Now that the side surfaces are in place, we need to close the top and bottom. Using the Patch command, we select the boundary edges to seal both openings. If your sketches are hidden, toggle their visibility back on to make selection easier.
Even though the model looks complete, it’s still a surface model—meaning it has zero thickness. A quick section analysis confirms this.
Patch feature used to close the bottom opening of the surface model. The boundary edges of the triangular surface structure are selected so Fusion can generate a planar patch surface. Closing open boundaries early helps maintain a watertight surface model before converting it into a solid body later in the workflow.
Patch feature used again to close the top opening of the vase surface model. By defining the boundary edges around the hexagonal rim, Fusion creates a new surface that completes the outer skin of the geometry. At this stage the model consists of multiple connected surfaces rather than a single solid body.
Section Analysis tool used to inspect the interior structure of the surface model. Cutting through the model with a temporary analysis plane reveals whether the surfaces align correctly and whether any gaps or overlaps exist before stitching the surfaces into a solid.
Step 4: Converting to a Solid Body
To make the model solid, we use the Stitch command to join all the surface pieces together. Once stitched, the section analysis now shows a fully enclosed solid model—ready for further refinements.
Stitch command combining the individual surface patches into a single closed surface body. Fusion highlights all selected surfaces and reports free edges and tolerance values. If all edges connect within tolerance, the stitched result becomes a solid body instead of a surface body.
Section Analysis used again after stitching to verify that the model has converted into a watertight solid body. The cross-section shows a continuous volume without surface gaps, confirming that the geometry can now support solid modeling operations such as shell, fillet, or combine.
Step 5: Completing and Refining the Shape
First, mirror the body using the Join operation to combine both halves into a single solid. This completes the full vase geometry while keeping the modeling process efficient.
Next, use the Shell command to hollow out the pot, setting the wall thickness to 3 mm. This creates a lightweight structure that balances print time, material usage, and durability.
Finally, add a fillet to the top edges to soften the sharp corners and give the vase a cleaner, more refined appearance.
Mirror operation duplicating the modeled half of the vase across a central construction plane. Mirroring geometry reduces modeling time and guarantees perfect symmetry across the design. The mirrored body is joined with the original to create the complete vase form.
Shell feature applied to hollow the solid vase body while maintaining a consistent wall thickness. The top face is removed and Fusion offsets the interior surfaces inward to produce printable wall geometry. Shell operations are commonly used when preparing containers or vases for additive manufacturing.
Fillet feature rounding the sharp edges around the top rim of the vase. Small edge fillets improve both aesthetics and usability by removing sharp corners that could otherwise chip during printing or feel uncomfortable when handling the object.
Step 6: Applying Materials and Rendering
For the final look, we apply a metal flake appearance—though you can experiment with different materials. Rendering the model in Fusion’s Render workspace brings out its details.
Switching to a photobooth environment optimizes the lighting, and adjusting the focal length fine-tunes the final image. Before rendering, double-check the resolution settings to ensure high-quality output.
Appearance panel used to assign a material finish to the solid body. Applying appearances helps visualize the final object and is useful when preparing renders or preview images for product listings, tutorials, or design documentation.
Scene Settings panel in the Render workspace controlling lighting environment, ground plane, and reflections. Adjusting these parameters helps create realistic renderings that better communicate the shape and surface quality of the modeled object.
Render Settings dialog defining output resolution, aspect ratio, and rendering method. Cloud rendering can produce higher-quality images without using local computing resources, which is useful when generating presentation images or thumbnails for tutorials.
Step 7: Making Design Changes with Parametric Modeling
One of Fusion’s greatest strengths is parametric modeling, which allows easy modifications. For example, if we increase the top polygon’s radius from 50 mm to 75 mm, Fusion automatically updates all dependent features. This ability to iterate quickly is key to refining designs without starting over.
Timeline used to edit the original sketch that drives the vase geometry. In a parametric workflow, modifying an early sketch allows the entire model to update automatically, making it easy to explore design variations without rebuilding the model from scratch.
Sketch defining the main dimensions and proportions of the vase. Because the model is built using parametric relationships, adjusting these sketch dimensions automatically updates downstream features such as surfaces, mirror operations, and shell thickness.
Final vase geometry after modifying the driving sketch parameters. The entire model rebuilds automatically through the timeline, demonstrating the advantage of parametric modeling when refining proportions or adapting a design for different sizes.
Key Takeaways
- Creating a new component at the start keeps Fusion projects organized and easier to modify later.
- Stacked sketches on offset planes are a simple way to control complex shapes.
- Surface modeling tools like Loft and Patch allow you to build geometry that would be difficult with solids alone.
- Circular Pattern can dramatically speed up modeling by repeating a single feature around an axis.
- Surface models must be converted into solids using Stitch before applying solid modeling tools.
- Shell and Fillet help prepare models for 3D printing by improving strength and printability.
- Fusion’s parametric design system lets you change key dimensions and automatically update the entire model.
🧰 Tools & Deals
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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
00:13 Sketching the Hexagon Base
01:25 Lofting the Polygon Edges
01:50 Using a Circular Pattern for Efficiency
02:16 Creating Additional Lofted Surfaces
03:00 Sealing the Top and Bottom with Patch
03:20 Analyzing the Surface Model
03:41 Converting to a Solid with Stitch
04:04 Duplicating the Body with Mirror
04:21 Hollowing the Model with Shell
04:53 Smoothing Edges with Fillets
05:06 Applying a Metal Flake Finish
05:27 Rendering with Photobooth Lighting
06:52 Editing the Design with Parametrics
07:57 Subscribe to The Maker Letters
You Might Also Like
If you enjoyed this Fusion tutorial, here are three more projects that explore surface modeling, smooth geometry, and practical modeling workflows you can reuse in many different designs.
Together, these tutorials build on the same core ideas used here — shaping smooth geometry, combining surface and solid tools, and turning CAD workflows into practical designs you can adapt for many different projects.