Design a 3D Printed Lampshade in Autodesk Fusion CAD Software
Updated December 21, 2025
Designing visually striking 3D-printed products often comes down to mastering a few core modeling principles. This lampshade project combines surface modeling, controlled curvature, and parametric thinking to create a design that is both elegant and highly adaptable for 3D printing. The workflow is efficient, robust, and easy to modify—ideal for anyone looking to turn Fusion skills into real, printable products.
What You’ll Learn
In this tutorial, you’ll learn how to design a multi-color 3D-printable lampshade in Fusion using a clean, production-ready workflow. The focus is on building stable geometry that is easy to edit, visually balanced, and well suited for FDM 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: Set Up Reference Geometry with Construction Lines
Start by sketching a single vertical line and convert it into a construction line. This line defines the total height of the lampshade and acts as a stable reference throughout the design. Setting it to 140 mm ensures that proportions stay consistent even if the design changes later.
Offset two additional construction lines horizontally. One represents the top diameter reference and the other the bottom diameter. Using construction geometry for layout keeps the sketch flexible and prevents accidental profile creation that could interfere with later operations.
Reference lines and base dimensions establish ordered spacing and overall height for the lamp shade. This layout defines the vertical envelope before any curvature is introduced, making later spline edits predictable and easy to control.
Step 2: Define Key Horizontal Reference Points
Deactivate construction lines (keyboard shortcut X) and sketch a horizontal line near the top of the vertical reference. The exact position matters more than the line itself—this distance controls how the curvature transitions near the top opening.
Add another horizontal line in the middle of the vertical reference and mirror it to the bottom using the sketch mirror tool. The sketch environment includes multiple mirror options, but only one applies to sketch geometry—the hollow icon indicates the correct choice. This guarantees symmetry and balanced proportions.
A vertical construction line defines the revolve axis and symmetry reference. Anchoring all critical geometry to this axis ensures the final revolve remains centered and avoids off-axis solids caused by drifting sketch points.
Step 3: Create Smooth Curvature with a Fit Point Spline
Use a Fit Point Spline to connect the top and bottom width references. Limit the spline to four points to maintain clean curvature and avoid unnecessary complexity. Fewer control points result in smoother surfaces and more predictable downstream features.
Adjust the spline handles to refine the shape. If Fusion automatically applies constraints that lock the spline, remove them selectively. This step is critical for achieving a controlled, organic profile without fighting the software.
A fit-point spline is introduced to control the lamp shade’s outer curvature. Early spline placement focuses on overall flow rather than precision, allowing the profile to be refined after constraints are added.
Step 4: Add the Pattern Guide Line
Sketch a straight line at a 70-degree angle. This line will later define the repeating pattern around the lampshade. Although a closed profile appears, it is intentionally ignored—the line itself is all that’s needed.
Extend the line slightly beyond the bottom reference to simplify later extrude operations. Over-sketching at this stage helps prevent failed features without affecting the final geometry.
An angled reference line constrains the inner profile and controls taper toward the opening. This ensures consistent wall direction and prevents accidental inward curvature that could cause thin or self-intersecting geometry later.
Step 5: Revolve the Surface Profile
Switch to the Surface workspace and use the Revolve tool. Select the spline as the profile and choose the central axis above the origin as the axis of revolution. Keeping the origin centered from the start simplifies symmetry, mirroring, and patterning later in the workflow.
This operation creates a surface body rather than a solid, which is ideal for controlling thickness and transitions with precision.
The surface modeling Revolve tool is configured by selecting the spline and the central construction axis. Creating a new body preserves design flexibility and keeps the base geometry isolated for later surface or solid operations.
Step 6: Thicken the Surface into a Solid
Apply a thickness of 3 mm to the revolved surface. This converts the surface into a solid body with uniform wall thickness—an important consideration for reliable FDM 3D printing and consistent material flow.
The Thicken tool converts the revolved surface into a solid body by adding a uniform 3 mm wall thickness in one direction. Applying thickness at this stage preserves the external shape defined by the surface model while establishing structural rigidity suitable for 3D printing.
Step 7: Create Top and Bottom Splitting Surfaces
Turn on the visibility of the horizontal sketch lines at the top and bottom. Use the Surface Extrude tool to extend them symmetrically. Symmetric extrudes reduce guesswork and maintain alignment around the center plane.
These surfaces are not part of the final geometry. They exist purely to split the lampshade into manageable sections.
Horizontal sketch lines are extruded as surfaces using a symmetric extent around the center plane. These surfaces are intentionally oversized to guarantee full intersection with the lamp shade body during later split operations. Using symmetric surface extrudes keeps the setup centered and avoids manual offset adjustments when the overall height changes.
Step 8: Split the Body for Controlled Editing
Use the extruded surfaces to split the lampshade into three bodies: top, middle, and bottom. This allows aggressive edits to the patterned middle section while preserving clean transitions at the top and bottom openings.
This technique is especially useful for decorative prints where surface detail is dense but edge quality must remain consistent.
The lampshade is shown intersected by two horizontal surface planes, one above and one below the patterned midsection. The Split Body dialog is active, using the extruded surfaces as splitting tools to divide the original form into three separate bodies. This setup isolates the middle section for detailed edits while keeping the top and bottom openings clean and consistent.
Step 9: Extrude the Pattern Line
Hide the top surface temporarily to simplify selection. Extrude the angled line far enough to pass through the lampshade without intersecting unwanted geometry. Set the thickness to 3 mm to match the rest of the model and maintain consistent wall behavior.
An angled sketch line on the lampshade is selected and extruded using the Extrude tool. The top surface is hidden to simplify selection, and the extrusion extends far enough to fully pass through the lampshade without creating unwanted intersections. The extrusion thickness is set to 3 mm in the next step.
The Thicken command is used to convert the previously extruded angled surface into a solid by applying a 3.0 mm thickness in one direction. This step turns the construction surface into usable solid geometry so it can participate in boolean operations, such as splitting, mirroring, or patterning, later in the workflow.
Step 10: Use Extrude Intersect for Pattern Creation
Turn off visibility for the top and bottom bodies. Over-extrude the patterned body through the lampshade and change the operation type from Join to Intersect.
Intersect keeps only the overlapping volume, which is ideal for generating complex cut-through patterns without manual trimming. A quick visibility check confirms that the top and bottom sections remain unaffected.
The angled patterned body is extruded beyond the full height of the lampshade to ensure it fully overlaps the target geometry. Over-extruding guarantees a clean intersection result and avoids partial cuts caused by insufficient extrusion length.
The Extrude dialog is shown with the operation changed from Join to Intersect. This keeps only the shared volume between the patterned extrusion and the lampshade, automatically generating a clean cut-through pattern without manual trimming or additional boolean steps.
Step 11: Mirror the Patterned Body
Mirror the intersected body using the vertical axis above the origin. Any apparent length mismatch is visual only and caused by the intersect tool’s temporary geometry. Once mirrored, re-enable visibility for the top and bottom bodies and keep them active for the remainder of the design.
The Mirror command is used to duplicate the intersected patterned body across a vertical construction plane aligned with the model’s center axis. This creates a symmetrical pattern layout without rebuilding geometry. Any apparent length mismatch is temporary and caused by the intersect operation’s visual preview, not actual geometry differences. After mirroring, the top and bottom bodies can be made visible again for continued refinement.
Step 12: Apply Appearances Before Patterning
Apply appearances before creating circular patterns to minimize contact points and reduce selection overhead. Fusion allows precise color control using RGB or Hex values, which is ideal for matching branding or preparing multi-color prints.
Duplicate appearances for other bodies if designing a multi-color product. Multi-material or color-separated designs often command higher perceived value and stand out in product listings.
Appearances are applied at the body level using the Appearance panel before any circular pattern is created. Assigning colors at this stage keeps each patterned instance independent and avoids excessive face-level selection later. Fusion’s appearance system supports precise RGB or hex color control, which is useful for previewing multi-color designs, separating bodies visually, and preparing models for color-specific printing or product visualization.
Step 13: Finish with a Circular Pattern
Hide unnecessary surface bodies and apply a Circular Pattern using the vertical axis above the origin. Dense pattern repetition works well for lampshades, creating visual depth and even light diffusion.
The earlier decision to apply appearances first makes this step significantly cleaner and more efficient.
A Circular Pattern is applied to the patterned bodies using the vertical construction axis through the origin as the rotation axis. Only the relevant pattern bodies are selected, while temporary surface bodies and non-participating solids are hidden to keep selection clean. Using a full 360-degree distribution with a high instance count creates a dense, evenly spaced pattern that adds visual depth and improves light diffusion for lampshade designs. Applying appearances earlier allows each patterned instance to inherit its color automatically, avoiding post-pattern cleanup and reducing timeline complexity.
Key Takeaways
This project demonstrates how surface modeling and solid modeling can work together to create complex yet editable designs in Fusion. Construction geometry keeps sketches adaptable, surface tools provide precise curvature control, and intersect-based workflows simplify pattern creation. By structuring the model into logical bodies and applying appearances early, the design stays flexible, printable, and easy to iterate—ideal for high-quality 3D-printed products.
🧰 Tools & Deals
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⏱ Chapters
- 00:00 Setting up the Sketch in Autodesk Fusion
- 01:25 Setting up the curvature with the fit point spline in Autodesk Fusion
- 02:14 How to revolve a Sketch Line in Fusion
- 02:33 How to make a surface thick in Fusion
- 02:48 How to extrude a symmetric Surface from a Sketch Line in Fusion
- 03:17 How to split a solid model using surfaces in Fusion
- 03:40 How to extrude a Line in Autodesk Fusion
- 03:53 How to thicken a surface in Fusion
- 04:13 How to use Extrude Intersect in Fusion
- 04:35 How to mirror a body in Autodesk Fusion
- 05:13 How to add a Hex Color in Fusion
- 06:08 Create a Circular Pattern in Fusion
- 06:33 Inspiration for this Video
- 06:45 Subscribe to The Maker Letters
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🧩 Master Surface and Solid Modeling in Fusion
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✏️ Create an Industrial-Style Pen Holder for 3D Printing in Fusion
Each tutorial walks through a complete, real-world modeling workflow — from sketch setup and surface control to solid features and print-ready geometry — helping you build cleaner, more reliable designs that are easy to modify and manufacture.