Design a Fidget Cone in Fusion for 3D Printing
Updated April 22, 2026
Designing a fidget-friendly mechanism in Fusion is a great way to combine creative modeling with real-world 3D printing constraints. In this workflow, you’ll build a parametric cone, cut a twisted pattern through it, and finish with a simple animation to present your design.
What You’ll Learn
- How to create a tapered cone using Extrude with a taper angle
- Why working with duplicate bodies can speed up complex workflows
- How to use projected and offset sketches to control geometry
- How to create organic shapes with Fit Point Splines
- Why Sweep with Twist is ideal for helical cut patterns
- How to apply Combine and Press Pull for functional clearances
- How to convert bodies into components for animation
- How to create a simple animation in the Animation workspace
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 Base Cone
Start with a center diameter circle on the horizontal construction plane, centered at the origin. The exact size isn’t critical, but a base around 80 mm works well for a handheld print.
Center-diameter circle defines the base profile on the origin. Constraining it to the origin ensures predictable scaling and keeps all downstream features aligned.
Instead of finishing the sketch, go directly into Extrude. This is a small but efficient workflow improvement—fewer clicks, faster iteration.
Extrude the profile to 80 mm and apply a taper angle of -15 degrees. The negative taper narrows the cone as it rises, which gives the model a more ergonomic shape and also improves printability by reducing overhang severity.
Extrude with a negative taper angle creates the cone shape in a single feature. Using taper here is more efficient than lofting and keeps the timeline simpler for edits.
Step 2: Duplicate the Body for Boolean Work
Create a second copy of the cone directly in place using copy-paste in the browser. Confirm the paste without moving the body.
This setup—two identical bodies in the same position—is intentional. One will act as a tool body for cutting later, which gives you more control compared to editing a single body destructively.
Move/Copy duplicates the body for later boolean operations. Keeping copies as separate bodies allows non-destructive edits and easier iteration.
Apply different appearances to each body. This is not just cosmetic—it’s a practical way to avoid confusion when bodies overlap in the same space.
Applying appearance early helps visually distinguish bodies during modeling. This reduces selection errors when working with multiple overlapping features.
Different appearances are assigned to separate bodies to clarify which geometry will be cut or combined. This is especially useful before boolean operations.
Step 3: Prepare a Controlled Sketch Foundation
Hide the second body and continue working on the first.
Project the bottom edge of the cone into a new sketch using a linked projection. This is critical: a linked projection updates automatically if the original geometry changes, which keeps your downstream features stable.
Project with link creates associative geometry from the solid edge. This keeps the sketch updated if the base diameter changes.
Offset the projected circle inward by 5 mm and convert it to a construction line. This offset acts as a boundary, ensuring your future cut doesn’t weaken the outer wall too much.
Offset creates an inner boundary to control wall thickness. Using offset instead of a new circle preserves concentric constraints automatically.
Step 4: Define the Pattern Structure
Sketch lines from the origin outward to divide the circle into sections. Use dimensions or formulas to control spacing—dividing into 12 segments gives 30 degrees per section.
Convert these lines into construction lines. They’re only guides, and keeping them as construction geometry prevents unintended profile selections later.
A fit point spline defines the cut profile, then mirrored for symmetry. Mirroring reduces manual constraints and ensures both sides remain identical.
Step 5: Create the Cutting Profile with a Spline
Use a Fit Point Spline to sketch a flowing shape between two guide lines. Keep the number of spline points low—this gives smoother curvature and makes adjustments easier.
Break one of the construction lines so part of it becomes a real edge for your closed profile. Then mirror the spline and line across the vertical axis to complete the shape.
This approach—half sketch plus mirror—is efficient and keeps your geometry symmetrical and easy to edit.
Dimensions and constraints stabilize the spline profile. Without constraints, small changes later can distort the cut path unpredictably.
Step 6: Add a Sweep Path
Create a vertical line from the base upward to match the cone height (80 mm). This will act as the path for the Sweep.
While this line isn’t linked parametrically to the cone height, it works for now. In more advanced workflows, user parameters would tie these values together for full design control.
The line is converted to a construction line (X) and used as the sweep path. Using construction geometry keeps the path separate from profile constraints and avoids unintended interactions during feature creation.
Step 7: Perform a Twisted Sweep Cut
Use the Sweep command with the profile and vertical line as the path. Set the operation to Cut and apply a twist angle of 360 degrees.
This is where the design comes alive. Sweep with twist is ideal for creating helical or spiral cuts—something that would be far more complex with standard extrude cuts.
The earlier 5 mm offset now pays off. The cut gradually intersects the cone instead of removing too much material at the base.
Sweep cut removes material along the spline path. Orientation set to perpendicular maintains consistent cut thickness along the curved surface.
Step 8: Circular Pattern the Cut
Use a circular pattern around the vertical axis and set the quantity to six.
Patterning features instead of sketch geometry keeps your timeline cleaner and allows you to adjust the pattern later without reworking sketches.
Expect some computation time here—twisted sweep cuts are resource-intensive.
Circular pattern replicates the sweep cut around the central axis. Patterning features keeps the design parametric and editable.
The repeated cuts form a helical pattern across the cone. Even spacing ensures uniform visual rhythm and consistent structural thickness.
Step 9: Combine the Two Bodies
Turn the second body back on. You’ll see overlapping geometry where the patterned cuts intersect.
Use Combine → Cut:
- Target Body: Body Two
- Tool Body: Body One
- Operation: Cut
- Enable Keep Tools
This removes the overlapping regions while preserving both bodies, which is essential for the next step.
Combine merges or subtracts bodies to finalize the geometry. Keeping tools checked allows reuse if adjustments are needed later.
Step 10: Add Clearance for 3D Printing
Hide the second body again and use Press Pull on selected faces of the first body.
Apply a small negative offset, around -0.2 mm. This creates clearance between the two parts.
This step is critical for real-world functionality. Without clearance, printed parts will fuse together. The exact value depends on your printer, material, and tolerances.
Offset Face fine-tunes wall thickness after cuts are applied. This is faster than editing earlier features when only thickness needs adjustment.
Step 11: Convert to Components
Turn the second body back on and verify the gap.
Convert both bodies into components. This is required for animation and also aligns with best practices in Fusion—components provide better control over movement and assembly behavior.
Converting bodies to components organizes the design for animation or assembly. Components allow independent control of visibility and motion.
Bodies are converted into components to structure the design for assembly and animation. This separation enables independent transforms, clearer timelines, and better control when creating exploded views or motion studies.
Step 12: Create a Simple Animation
Switch to the Animation workspace.
Start by setting the initial camera angle. Then define a duration, for example ten seconds. Fusion records camera movement automatically between keyframes.
Move the second component upward to the top of the cone. Then apply a rotation of 360 degrees.
This mirrors the twist used in the Sweep, creating a cohesive visual story between modeling and motion.
Preview the animation and adjust if needed.
Animation workspace is used to separate components visually. This helps communicate how parts relate without modifying the design history.
Step 13: Publish the Animation
Click Publish, choose your settings, and export the animation.
This gives you a clean way to present your design—useful for YouTube, product pages, or portfolio work.
ideo export settings define resolution and aspect ratio. Matching output to 16:9 ensures compatibility with YouTube and avoids scaling artifacts.
Key Takeaways
- Extrude with taper is a fast way to create printable cone geometry
- Duplicate bodies enable flexible, non-destructive workflows
- Linked projections maintain design intent across the timeline
- Fit Point Splines are powerful when kept simple and controlled
- Sweep with twist is the most efficient way to create helical cuts
- Combine and Keep Tools allow precise boolean control
- Clearance is essential for functional 3D printed assemblies
- Components are required for animation and better structure
- Animation adds a professional layer to your CAD presentations
🧰 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
00:08 How to Create a Center Diameter Sketch in Fusion
00:32 Extrude a Circle with Taper Angle in Fusion
00:57 How to Copy a Body in Fusion for 3D Modeling
01:12 Add Glossy Plastic Appearances in Fusion
01:45 How to Project Geometry onto a Body in Fusion
02:16 Offsetting a Sketch in Fusion – Step-by-Step
02:30 Creating a Construction Line in Fusion
02:40 How to Create Guide Lines and Set Angles in Fusion
03:19 Add a Fit Point Spline in Fusion for Smooth Curves
03:43 How to Break a Line in Fusion – Essential Tips
04:07 How to Mirror a Sketch in Fusion Efficiently
04:31 Adjust Fit Point Splines in Fusion – Quick Guide
05:06 How to Add a Line in Fusion for Precise Design
06:00 How to Use Sweep with an Angle in Fusion
06:38 Create a Circular Pattern in Fusion 3D Modeling
07:35 How to Combine Bodies in Fusion for Complex Designs
08:28 Save Your Fusion Project for Better Workflow
08:40 How to Pull a Body to Create Clearance in Fusion
10:06 Create Components from the Project Browser in Fusion
10:31 How to Create an Animation in Fusion for 3D Models
10:51 Animate the Camera Angle in Fusion Tutorial
11:49 Animate the Movement Upwards in Fusion – Easy Guide
12:31 Animate the Rotation in Fusion for 3D Models
13:01 How to Publish the Animation in Fusion
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Each guide builds on core Fusion concepts—surface control, pattern efficiency, and real-world printability—so you can design parts that are both visually clean and functionally reliable.