How to Design a Honeycomb Lampshade in Fusion
Updated August 19, 2026
How to Design a Honeycomb Lampshade in Autodesk Fusion (formerly Fusion 360) for 3D Printing
A honeycomb pattern can turn a simple lampshade into a much more interesting 3D printing project—but the real value of this workflow is learning how to control repeated geometry, build parts in context, and keep the design editable. In this Autodesk Fusion tutorial, you’ll create a honeycomb lampshade prototype, model a simple lightbulb and electrical cable, and finish with a 1920 × 1080 rendering of the complete design.
What You’ll Learn
- How to create a honeycomb pattern from an inscribed polygon with a 5 mm dimension
- How to control a rectangular sketch pattern using 10 mm spacing and a quantity of 8 in both directions
- How to turn a patterned sketch into a cylindrical lampshade with a 100 mm diameter, 35 mm height, and 3 mm wall thickness
- How to use Intersect to extract only the honeycomb geometry that overlaps the lampshade
- How and why to add fillets before creating a circular pattern
- How to multiply the honeycomb section around the lampshade using a circular pattern
- How to organize the lampshade, lightbulb, and electrical cable as separate components
- How to model a simple lightbulb using an 8 mm diameter extrusion, a sphere, and Fusion appearances
- How to create a 3 mm diameter cable along a 70 mm sweep path
- How to prepare the geometry with 3D printing considerations such as wall thickness, orientation, and overhangs in mind
- How to set up a simple rendering at 1920 × 1080 resolution
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 First Honeycomb Polygon
Create the first of the three components used in this project, then start a sketch on the vertical construction plane facing you.
The honeycomb lampshade is created as a dedicated New Component in Fusion before any modeling begins. The component is activated immediately so the sketches, bodies, and features created afterward remain organized within the lampshade structure.
Starting with a component is useful for an assembly that will later include separate reference geometry for the light bulb and electrical cable. It keeps those objects independent while allowing them to remain positioned relative to the lampshade.
Select the Inscribed Polygon tool and place the polygon at the center of the origin. Using the origin as a consistent reference point makes it easier to keep the different parts of the lampshade aligned as the model becomes more complex.
Set the polygon dimension to:
- Polygon dimension: 5 mm
The exact size is less important than the workflow in this prototype, so you can modify it later if you want a larger or smaller honeycomb structure.
While working, keep an eye on the keyboard shortcuts displayed in the bottom-left corner of the Fusion canvas. Learning these shortcuts can significantly speed up repetitive CAD workflows.
A six-sided polygon is created from the sketch origin to define the first honeycomb cell. The polygon is centered on the origin, giving the later pattern operations a stable geometric reference.
The visible radial dimension is 5 mm, establishing the initial hexagon size. Because the entire honeycomb pattern develops from this seed geometry, controlling the first cell precisely is more efficient than trying to correct spacing after the pattern has been generated.
Step 2: Create Construction Lines for the Honeycomb Pattern
Create two guide lines that will define the directions of the upcoming rectangular pattern.
Convert both lines to Construction geometry. They are reference elements rather than geometry that should form part of the final sketch profiles.
The hexagon sketch is refined by converting its internal reference line to construction geometry. The Linetype control in the Sketch Palette is used so this reference can constrain the polygon without becoming part of a closed printable profile.
Construction geometry (keyboard shortcut X) is valuable in parametric sketches because it carries dimensions and relationships while remaining excluded from extrusion profiles. The 5 mm radial dimension remains the controlling size for the honeycomb cell.
Although fully constraining the sketch is not strictly required for this prototype, it is a good parametric modeling habit. A fully constrained sketch is less likely to move unexpectedly when dimensions or surrounding geometry change.
Fusion's AutoConstraints feature can help by suggesting appropriate geometric constraints as you sketch.
For models intended for 3D printing, predictable sketches become increasingly valuable as the design evolves. A seemingly small unintended movement in a sketch can eventually alter wall thickness, clearances, or repeating geometry elsewhere in the model.
Fusion's AutoConstrain tool analyzes the hexagon and proposes geometric constraints for the sketch. The results panel displays alternative constraint sets before they are committed.
Applying consistent constraints reduces the risk of individual lines drifting when dimensions are changed later. For repeated geometry such as a honeycomb lattice, a stable seed sketch is especially important because any error in the original cell propagates through every patterned instance.
Step 3: Build the Rectangular Honeycomb Pattern
Stay inside the active sketch and start a Rectangular Pattern.
Select:
- Object: the polygon
- Direction 1: the first construction line
- Direction 2: the second construction line
Change Distribution Type to:
- Spacing
The first honeycomb cell is expanded with Rectangular Pattern in the sketch environment. The distribution setting is changed to Spacing, which defines the distance between successive pattern instances rather than the overall extent of the pattern.
Spacing is particularly useful for lattice geometry because the cell-to-cell pitch stays consistent when the number of instances changes. That makes it easier to enlarge or reduce the honeycomb field without manually recalculating the total pattern dimensions.
Then change the pattern direction to:
- Symmetric
The first Rectangular Pattern direction is changed from One Direction to Symmetric. This distributes the repeated hexagons on both sides of the original seed geometry.
A symmetric pattern keeps the honeycomb field centered around the origin. That becomes useful later when the pattern is intersected with circular geometry, because the lattice extends evenly across the lampshade profile instead of requiring manual repositioning.
The second pattern direction is also switched to Symmetric, expanding the honeycomb grid in both axes around the original hexagon.
Using two symmetric pattern directions creates a centered rectangular field of honeycomb geometry. The pattern can deliberately extend beyond the eventual lampshade boundary because the excess geometry will be removed by later solid-modeling operations.
Set both pattern directions to:
- Distance: 10 mm
- Quantity: 8
This intentionally creates more polygons than the lampshade actually needs. Instead of trying to calculate the exact number of cells in advance, you create an oversized field of honeycomb geometry and extract the portion required later.
That is a useful CAD strategy when prototyping: create enough source geometry to give yourself flexibility, then use downstream features to define the final form.
There is, however, a parametric tradeoff to creating a large pattern directly inside a sketch. We’ll return to that in the Key Takeaways section.
The Rectangular Pattern is expanded until the sketch contains enough hexagons to cover the intended lampshade area. The visible settings use 8 instances and 10 mm spacing in the pattern directions.
It is not necessary to trim the honeycomb field precisely at this stage. Extending the repeated geometry beyond the final boundary provides complete coverage and lets the cylindrical body define the finished shape later in the workflow.
Step 4: Define the Honeycomb Section
Next, define which part of the large honeycomb sketch will eventually become a 3D solid.
Use the 2-Point Rectangle tool.
Start the rectangle at the center of one polygon and finish it at the center of another polygon.
This positioning is intentional. Later, you’ll use a circular pattern to repeat the resulting section around the lampshade. Starting and ending the rectangular region at polygon centers helps the repeated sections align correctly.
If you try to dimension the rectangle at this point, Fusion may create driven dimensions rather than driving dimensions. That happens because snapping the rectangle to the polygon centers has already constrained its geometry.
Those dimensions therefore report the size created by your earlier design decisions rather than controlling it.
Finish the sketch when the honeycomb section is ready.
With the honeycomb field established, additional sketch geometry is introduced around the origin to prepare the lattice for the lampshade body. The repeated hexagons remain centered on the primary horizontal and vertical axes.
Keeping the larger pattern referenced to the origin simplifies the transition from a flat 2D lattice to cylindrical solid geometry. It also provides predictable axes for later operations such as extrusion and circular patterning.
Step 5: Create the Basic Lampshade Body
Switch to the front view and then start another sketch on the flat horizontal construction plane.
Create a Center Diameter Circle directly above the origin.
Set:
- Diameter: 100 mm
A large circle is sketched concentrically around the honeycomb field to define the overall cylindrical envelope of the lampshade. The circle is centered directly on the sketch origin.
The circular boundary establishes the solid body that will be used to capture the honeycomb geometry. Rather than manually trimming dozens of individual hexagons at the perimeter, the workflow uses the cylindrical solid to control which portions of the lattice become part of the final lampshade.
Finish the sketch and extrude the circular profile:
- Extrude distance: 35 mm
- Operation: New Body
You now have a simple cylindrical volume that acts as the rough draft of the lampshade.
This temporary solid gives you a controlled envelope that can be used to trim the oversized honeycomb geometry created earlier.
The circular profile is converted into a solid using Extrude with a distance of 35 mm and New Body as the operation. This creates the cylindrical volume that establishes the height and curvature of the lampshade.
The honeycomb sketch remains available as reference geometry while the solid body provides the surface onto which the lattice structure will be developed.
Step 6: Shell the Lampshade to a 3 mm Wall Thickness
Switch to a bottom view and activate Shell.
Hollow the cylindrical body using:
- Shell thickness: 3 mm
- Direction: Inside
The 3 mm thickness creates a substantial wall for a prototype and gives the following intersect operation enough material to turn the honeycomb sketch into usable 3D geometry.
The cylinder is hollowed with Shell, using an Inside Thickness of 3 mm. The selected end face is removed, leaving a cylindrical wall rather than a solid volume.
The 3 mm wall establishes the depth available for the honeycomb structure. Shelling inward also preserves the original external diameter of the lampshade, which is useful when the outside dimensions are already established.
Wall thickness matters when designing for 3D printing. Extremely thin features may look fine in CAD but can become fragile, disappear during slicing, or resolve poorly depending on nozzle diameter and extrusion width. A deliberate wall thickness makes the relationship between your CAD geometry and the eventual toolpath much easier to control.
Shelling toward the inside also preserves the original outside dimensions of the lampshade.
The model is being viewed from below at this stage because it creates a convenient modeling angle. If you eventually manufacture the part with FDM 3D printing, you are not locked into this orientation: the lampshade can simply be flipped in your slicer before printing.
That distinction is important. CAD orientation and print orientation do not have to be the same.
Step 7: Intersect the Honeycomb Sketch With the Lampshade
Activate Extrude.
Because the sketch profile is located behind the solid body, press and hold the left mouse button to bring up Fusion's selection menu and choose the required sketch profile.
Individual regions of the honeycomb sketch are selected as Extrude profiles while the shelled cylinder provides the surrounding body geometry. Fusion allows overlapping sketch and model geometry to be selected from the same view.
The profile selection determines which portions of the lattice are carried forward into the solid-modeling operation. Careful selection here avoids introducing unwanted closed regions from the dense honeycomb sketch.
Over-extrude the profile beyond the lampshade body rather than stopping exactly at its edge.
The extra distance gives the feature some tolerance for future design changes. If you later modify the lampshade diameter, the extrusion is less likely to stop short and break the downstream geometry.
Set:
- Operation: Intersect
The Intersect operation keeps only the volume shared by the extruded honeycomb geometry and the lampshade body.
This turns the flat honeycomb layout into geometry that follows the volume defined by the cylindrical lampshade.
The selected honeycomb profile is extruded −100 mm, far enough to pass completely through the cylindrical body. Instead of creating or joining material, the Intersect operation is selected.
Intersect retains only the volume shared by the extruded honeycomb geometry and the existing body. This is an efficient way to convert a planar honeycomb pattern into geometry bounded by the curved cylindrical form without manually projecting and trimming every cell.
Step 8: Add Fillets Before Creating the Pattern
Refine the honeycomb section before multiplying it around the lampshade.
Start by applying a:
- Full Round Fillet to the top edge
After the intersection operation, the resulting honeycomb section is isolated and prepared for edge treatment with Fillet. At this stage the geometry consists of the honeycomb face with two long members extending from it.
The edge treatment is applied before circular patterning. Editing a single source body is substantially simpler than repeating the body first and then attempting to select equivalent edges across every patterned copy.
The Fillet command is changed to Full Round Fillet. A center face is selected, with Fusion using the adjacent side faces to replace the original flat face with a continuous rounded transition.
Full Round Fillet differs from a conventional fixed-radius fillet because the radius is determined by the surrounding geometry. On narrow structural members, this can create a consistently rounded section without manually calculating a radius.
A Full Round Fillet is parametric, so the curvature can adapt if you later modify the dimensions of the part.
Fillets can serve several purposes in a physical product:
- Remove sharp edges
- Improve handling
- Create a more finished appearance
- Reduce abrupt geometric transitions
- Potentially improve strength around stress concentrations
Fillets can also matter for 3D printing. Sharp transitions can create weak points, while gradual transitions may distribute loads more smoothly. Depending on orientation, rounded geometry can also create a more progressive change between layers than an abrupt horizontal ledge.
However, always inspect the resulting overhang angle in relation to your intended print orientation. A fillet is not automatically more printable simply because it is rounded.
Add additional fillets along the inside and back edges where appropriate.
A conventional Fillet is applied to four edges using a 1 mm radius. The selected edges sit where the long radial members transition into the honeycomb section.
The small radius removes sharp transitions while retaining most of the original cross-section. Performing this operation on the source body means the same edge treatment will automatically appear in every later circular-pattern instance.
A second Fillet operation targets two additional edges at the ends of the radial members. These edges require separate treatment because their geometry differs from the four-edge transition handled in the previous feature.
Separating fillet operations according to geometric function keeps the Fusion timeline easier to modify. If one radius or edge selection later fails, the unrelated edge treatments remain independent.
The full round fillets along the bottom are useful aesthetically, but they also make the finished lampshade more forgiving if someone bumps their head against it.
Making these changes now is much faster than editing every repeated body later.
If you forget, Fusion's parametric timeline gives you another option: return to the appropriate position in the timeline and insert or edit the fillet feature before the pattern operation.
All fillet operations appear in the timeline, and you can right-click them later to edit their individual settings.
Full Round Fillet is used again on the end faces of the structural members, producing fully rounded tips rather than leaving rectangular ends.
The completed source section now contains the honeycomb lattice, radial supports, and final edge treatments needed before repetition. Finishing these details on one body keeps the subsequent pattern operation compact and avoids duplicating unnecessary modeling work.
Step 9: Apply an Appearance Before Multiplying the Geometry
If you want every repeated honeycomb body to share the same appearance, apply the material appearance before creating the circular pattern.
For this example, use:
- Appearance: Glossy Yellow
Applying the appearance now allows the repeated bodies to inherit a consistent visual style.
If you want different colors across the lampshade, leave the appearances until later and assign them individually.
This step is primarily for visualization rather than 3D printing. Appearance settings in Fusion do not determine the physical filament or resin used when the model is manufactured.
The Appearance panel is opened and a glossy yellow appearance is applied to the completed source body. Appearance changes the visual representation without changing the underlying dimensions or solid geometry.
Using a distinctive appearance at this stage also makes the modeled lampshade easier to distinguish from the reference bodies that are introduced later for the lamp holder, bulb, and electrical cable.
Step 10: Pattern the Honeycomb Around the Lampshade
Create a Circular Pattern.
For the pattern axis, select:
- Axis: blue Z-axis centered above the origin
Because the earlier Intersect operation defined the width of the honeycomb section visually rather than by calculating a precise circumference division, you may not know the correct pattern quantity immediately.
That is fine.
Increase the circular pattern quantity until the bodies fill the circumference of the lampshade.
Switch to the front view and inspect how the repeated bodies meet. Make sure the pattern is correctly aligned before confirming the operation.
This is where the decision to start and finish the original rectangle at polygon centers becomes important. Those reference points help the repeating sections form a consistent honeycomb structure when wrapped around the full design.
The Circular Pattern tool in Fusion is used to repeat the completed honeycomb section around the lampshade. The patterned body is selected as the object, with the central Z-axis defining the axis of rotation.
Here, the quantity has been increased to 16 with the distribution set to Full. Rather than calculating the required number of repeats in advance, the pattern quantity can be adjusted visually until the honeycomb sections fill the circumference and align correctly.
Step 11: Create a Separate Lightbulb Component
Before modeling the bulb, activate the top-level component.
Create a new component for the lightbulb.
This places the lightbulb at the same hierarchical level as the lampshade rather than nesting it inside the lampshade component.
Separate components provide cleaner organization and independent timelines. That becomes particularly useful when a project contains multiple physical parts that may need to be edited, exported, hidden, rendered, or manufactured separately.
This project uses a top-down design methodology, meaning that additional parts are modeled in context around the existing design.
With the honeycomb lampshade complete, a separate Lightbulb component is created. The top-level project is selected as the parent so the new component sits alongside the Honeycomb Lampshade component rather than being nested inside it.
The Activate option is enabled when creating the component. This gives the lightbulb its own active modeling context and timeline, keeping its sketches and features separate from the lampshade geometry.
Step 12: Create a Tangent Sketch Plane
The full round fillets make sketching directly onto the top of the lampshade inconvenient because there is no longer a simple flat surface where you need one.
Create a Tangent Plane against the rounded body.
This gives you a clean, flat sketch surface positioned relative to the existing lampshade.
Tangent construction planes are useful in product design whenever you need to add geometry around cylindrical, curved, or filleted surfaces without modifying those surfaces first.
A Tangent Plane is created to provide a flat reference for modeling the lightbulb assembly in place. This is useful because the full-round fillets on the lampshade make its upper geometry unsuitable as a straightforward planar sketch surface.
The plane is positioned tangent to the selected rounded face with the displayed angle at 0.000°. Using construction geometry like this is a practical top-down modeling technique when new components need to be positioned relative to curved existing geometry.
Step 13: Model the Lightbulb Stem
Start a sketch on the new plane and create a Center Diameter Circle at the center of the design.
Set:
- Circle diameter: 8 mm
A Center Diameter Circle is placed at the center of the lampshade design to establish the profile for the lightbulb holder. The circle is dimensioned to exactly 8 mm in diameter.
The existing lampshade geometry provides a clear visual reference for positioning the circle. However, this quick workflow does not parametrically link the circle to the lampshade itself, so its position may require adjustment if the surrounding design is changed later.
Finish the sketch and activate Extrude.
Change the direction to:
- Two Sides
Set the two extrusion distances to:
- Downward distance: 20 mm
- Upward distance: 15 mm
- Operation: New Body
The 8 mm circle is extruded using the Two Sides direction to create the cylindrical part of the lightbulb assembly. One side is set to 15 mm, while the other extends 20 mm in the opposite direction.
Both extent types are set to Distance, the taper angles remain at 0.000°, and the operation is New Body. Using New Body keeps this geometry separate so another body can be added to the Lightbulb component in the next step.
This creates the basic solid used to position the lightbulb.
One limitation of this quick workflow is that the circle is positioned in place but is not parametrically linked to the lampshade geometry. If you substantially modify the lampshade later, the bulb placement may therefore need manual adjustment.
That is an important distinction in parametric CAD: geometry can look correctly positioned without necessarily having a design relationship that forces it to remain correctly positioned after an edit.
Step 14: Create the Bulb With a Sphere
Use Fusion's Sphere tool to create a simplified representation of the lightbulb.
Select the flat bottom face of the body created in the previous step as the working plane. Then select the center point of that face as the sphere's starting point.
Fusion may initially suggest:
- Operation: Cut
Change it to:
- Operation: New Body
The lightbulb component should now contain two separate bodies.
For this project, the sphere is primarily visualization geometry rather than a manufacturing-ready lightbulb model, so there is no need to overcomplicate it with unnecessary detail.
The Sphere tool creates a simple representation of the bulb below the cylindrical holder. The center of the holder's flat face provides the placement point for the sphere.
The visible Sphere settings use a 20 mm diameter and New Body operation. New Body is important here because the bulb and holder remain two distinct bodies inside the same Lightbulb component, allowing their appearances to be controlled independently later.
Step 15: Create the Electrical Cable Component
Return to the top level and create another component for the electrical cable.
The Browser should now contain three main components at the same hierarchical level:
- Honeycomb Lampshade
- Lightbulb
- Electrical Cable
Activate the Electrical Cable component before creating its geometry. This ensures its sketches and features are recorded in the correct component timeline.
A third component named Electrical cable is created for the cord. Like the lampshade and lightbulb, it is placed at the project's top hierarchical level rather than inside another component.
The Activate checkbox is enabled. This ensures the cable's upcoming sketches and Sweep feature are recorded in the Electrical cable component rather than accidentally added to the lampshade or lightbulb timeline.
Step 16: Sketch the 70 mm Cable Path
Start a sketch on the vertical construction plane facing you.
The vertical construction plane facing the front of the model is selected as the sketch plane for the electrical cable path. The front view makes it easier to position the cable relative to the center of the lampshade and lightbulb assembly.
Because geometry from the Lightbulb component has not been projected into the new Electrical cable component, there is no existing reference geometry to snap to. After selecting this construction plane, the view can be orbited as needed to locate the correct starting point for the 70 mm cable path.
Because no geometry has been projected from the lightbulb component, locating the correct starting point can initially be difficult.
Orbit the model and approach the sketch from another viewing angle if necessary.
You may notice that 3D Sketch is enabled in the Sketch Palette. It is not required for this operation because the path is being created as a 2D sketch.
Create the cable path with:
- Cable height/path length: 70 mm
Check the position before finishing the sketch.
Keeping the path simple is useful both parametrically and geometrically. More complicated sweep paths introduce additional curvature and can make later edits harder to diagnose.
A new sketch is started for the electrical cable path. Because geometry from the Lightbulb component has not been projected into this sketch, finding the intended starting position can be easier after orbiting the model and viewing the assembly from another angle.
The 3D Sketch option is visibly enabled in the Sketch Palette, but it is not required for this cable path because the geometry can be created as a conventional 2D sketch. The cable path is set to a height of 70 mm before it is used for the Sweep operation.
Step 17: Sweep a 3 mm Cable Along the Path
Create another sketch on top of the lightbulb component.
The top face of the lightbulb holder is selected as the sketch plane for the next step. This provides a flat surface centered on the holder where the electrical cable profile can be created.
In the upcoming sketch, a Center Diameter Circle will be placed on this face and set to 3 mm in diameter. That circle will then be used as the Profile for a Sweep, with the previously created 70 mm sketch line serving as the Path.
Draw a Center Diameter Circle and set:
- Diameter: 3 mm
A Center Diameter Circle is created on the previously selected top face of the lightbulb holder. This circle defines the cross-section of the electrical cable that will be created with the Sweep tool.
Set the circle diameter to 3 mm and position it at the center of the holder. The profile is kept separate from the 70 mm cable path, allowing the cable diameter and length to be controlled independently.
Finish the sketch and activate Sweep.
Set:
- Profile: 3 mm circle
- Path: 70 mm electrical cable sketch line
- Operation: New Body
Confirm the Sweep.
The Sweep command turns the circular cable profile into a solid body. Select the 3 mm circle as the Profile and the previously created 70 mm sketch line as the Path.
The Sweep uses Single Path, Perpendicular orientation, and New Body as the operation. The result is a straight cylindrical cable extending vertically from the lightbulb holder while remaining a separate body inside the Electrical cable component.
You now have a simple cylindrical electrical cable extending from the lamp assembly.
If this cable were intended for 3D printing rather than rendering, its 3 mm diameter would be an important manufacturing consideration. Long, thin vertical geometry can be vulnerable to flexing or breaking, while printing a cable-like feature horizontally could introduce substantial overhang or support requirements. For a functional printed model, you would therefore evaluate whether the cable should be printed separately or replaced with a real cable.
For this rendering model, however, the sweep provides the required visual geometry efficiently.
Step 18: Apply Cable and Lightbulb Appearances
Apply the following appearance to the cable:
- Black Glossy Plastic
With the cable geometry complete, open the Appearance panel and search the Fusion Appearance Library for glossy plastic. The electrical cable remains active in the Browser so the appearance can be applied to the correct body.
The search results include Plastic – Glossy (Black). Appearances affect how the model looks in Fusion and in the final rendering without changing the underlying cable geometry.
Then activate the Lightbulb component before modifying its bodies.
Apply:
- First lightbulb body: Metal Black Oxide
- Bulb body: 1500 lumen Frosted Bulb appearance
Switch to the Lightbulb component before applying appearances to its two bodies. This keeps the appearance-related actions associated with the correct component and helps maintain an organized Fusion timeline.
Here, the Coating – Black Oxide appearance is applied to the cylindrical lightbulb holder body. The bulb itself remains a separate body, allowing a different frosted bulb appearance to be applied in the next step.
The Lightbulb component contains two bodies, allowing different appearances to be assigned to the holder and bulb. Apply Coating – Black Oxide to the first part and use Fusion's appearance search to find the bulb material.
For the spherical bulb body, select A Type Bulb – Frosted – 1500lm. Fusion's searchable Appearance Library is useful for finding specialized materials like this without having to manually browse the full collection.
Switching to the relevant component before making changes keeps the project organized and ensures actions are recorded in the appropriate timeline.
Fusion includes a large appearance library, so using the search field is often faster than manually browsing categories. Exploring that library can also reveal materials and specialized appearances you may not have known were available.
Step 19: Review the Model for 3D Printing
Before moving to rendering, it is worth reviewing the lampshade specifically as a 3D printing project.
The design uses a 3 mm shell thickness, which gives the honeycomb structure meaningful physical thickness rather than leaving it as an infinitely thin surface.
Also consider print orientation carefully.
The modeling workflow naturally leaves the lampshade in one orientation, but the part can be flipped in your slicer before printing. Choose the orientation that provides the most stable contact with the build plate while minimizing difficult overhangs and unnecessary support material.
Pay particular attention to:
- The angle of the honeycomb geometry relative to the build plate
- The full round fillets
- Unsupported sections around the pattern
- Build-plate contact
- Whether the 3 mm walls resolve cleanly with your chosen nozzle and extrusion settings
- Whether the complete lampshade fits within your printer's build volume
Avoid assuming that a visually smooth CAD model will automatically print cleanly. Layer-by-layer manufacturing introduces constraints that do not exist inside Fusion.
For a prototype like this, slicing the design and inspecting the layer preview is an important final validation step before committing to a long print.
Step 20: Save a New Version and Create the Rendering
Once the model looks correct, save a new version before moving into Fusion's rendering workspace.
With the modeling and appearance work complete, save a new version of the Fusion project before moving into the Render workspace. The Version Description shown here is “Before Rendering.”
Creating a version at this point provides a useful checkpoint between the CAD modeling stage and visualization work. You can return to the completed design state later without relying solely on individual features in the timeline.
Set up a Photobooth environment and adjust the lighting until the honeycomb structure, curved surfaces, and bulb are clearly visible.
The completed lampshade is opened in Fusion's Render workspace, where the Scene Settings panel controls the environment, background, ground plane, reflections, and lighting conditions.
This stage does not change the modeled geometry. Instead, it controls how the yellow honeycomb structure, black cable, lightbulb, and other appearances are presented in the final image.
Open the Environment Library inside Scene Settings to choose the lighting environment for the render. The library includes options such as Grid Light, Photobooth, and Rim Highlights.
For this project, select the Photobooth environment. It provides a controlled studio-style setting that helps reveal the honeycomb geometry and the different surface appearances without requiring individual lights to be built manually.
After choosing the rendering environment, use Scene Settings to adjust its position and rotation relative to the lampshade. The image shows the environment rotation being changed while the lighting response updates directly on the model.
Rather than treating a specific rotation value as mandatory, adjust the environment visually until the honeycomb structure, bulb, and curved surfaces are clearly defined. This is an efficient way to control highlights and shadows before starting the final render.
For the final rendering, use:
- Resolution: 1920 × 1080 pixels
This 16:9 resolution works well for displaying the project on websites, video platforms, thumbnails, and other digital presentations.
The combination of the Glossy Yellow lampshade, Black Glossy Plastic cable, Metal Black Oxide fixture, and 1500 lumen Frosted Bulb appearance gives you a complete visual prototype without having to physically manufacture every part.
Open Render Settings to define the output size and quality of the finished lampshade image. The custom image dimensions are set to 1920 px wide × 1080 px high, creating a standard 16:9 image.
The dialog also provides controls for render method and quality, with Final selected here. Once the environment, composition, and resolution are ready, the model can be rendered as the final visualization of the honeycomb lampshade project.
Key Takeaways
This project combines sketch patterns, solid modeling, parametric features, components, sweeps, and rendering into one practical Fusion workflow.
The most important modeling decision to understand is the use of the rectangular pattern inside the original sketch. It is fast and intuitive, especially when you are exploring a concept and want to create a large honeycomb field quickly.
The tradeoff is editability.
Patterns created directly inside a sketch do not appear as independent pattern features in Fusion's parametric timeline. That can make the model more tedious to modify later.
For more robust parametric projects, a useful general principle is:
Keep sketches relatively simple and create repeated geometry as solid or surface pattern features whenever practical.
Those features appear independently in the timeline, making quantities, spacing, and other parameters easier to find and edit.
The same principle applies to 3D printing. A clean parametric model makes it much easier to iterate after your first test print. If a wall needs to become thicker, a pattern needs more clearance, or a feature creates an unwanted overhang, well-structured features let you make those changes without rebuilding the entire design.
The key dimensions and settings used in this project are:
- Honeycomb polygon dimension: 5 mm
- Rectangular pattern spacing: 10 mm in both directions
- Rectangular pattern quantity: 8 × 8
- Lampshade diameter: 100 mm
- Initial lampshade extrusion: 35 mm
- Shell thickness: 3 mm inside
- Honeycomb extrusion operation: Intersect
- Lightbulb stem diameter: 8 mm
- Lightbulb stem extrusion: 20 mm down / 15 mm up
- Cable path: 70 mm
- Cable diameter: 3 mm
- Cable operation: Sweep / New Body
- Rendering environment: Photobooth
- Final rendering resolution: 1920 × 1080
The workflow is deliberately approachable, but it introduces several techniques that scale well into more advanced product design: designing around an origin, using construction geometry, building parts in context, managing component hierarchies, and thinking about printability while you model.
🧰 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
.
You Might Also Like
Want to explore more Fusion workflows for honeycomb patterns and practical 3D printable designs? These three tutorials cover different ways to build repeatable honeycomb geometry and turn Fusion models into functional products for 3D printing.
Each project focuses on practical Fusion workflows for pattern creation, parametric modeling, and efficient 3D printable design techniques that translate well into functional real-world products.
Chapters:
00:11 Honeycomb Pattern Component in Fusion (formerly known as Fusion 360)
00:26 How to Sketch a Honeycomb Pattern in Fusion
01:10 Turn Reference Lines into Construction Lines in Fusion
01:20 Add AutoConstraints to Your Fusion Sketch
01:37 Create a Honeycomb Pattern from a Polygon in Fusion
02:58 Use a Rectangle Sketch to Refine the Honeycomb Layout
03:17 Driven Dimensions vs Regular Dimensions in Fusion
03:46 Design a Lampshade Sketch in Fusion
04:04 Extrude a Center Diameter Circle for the Lampshade
04:22 Hollow the Lampshade Using the Shell Command in Fusion
04:46 Cut a Honeycomb Pattern into the Lampshade Body
05:11 Use the Extrude Intersect Option in Fusion
05:29 Apply a Full Round Fillet in Fusion
05:44 Strengthen Your Design with Fillets in Fusion
06:41 Add a Glossy Yellow Appearance to Your Honeycomb Body
07:03 Use a Circular Pattern to Complete the Lampshade Design
07:13 Find the Right Quantity for a Circular Pattern in Fusion
07:38 Create a Lightbulb Component in Fusion
07:56 How to Create a Sketch Plane on a Rounded Body
08:20 Sketch on a Tangent Plane in Fusion
08:41 Extrude in Two Directions in Fusion
09:12 How to Create a Realistic Lightbulb Replica in Fusion
09:47 Create a New Component at the Correct Hierarchical Level
10:03 Sketch an Electrical Cable Path in Fusion
10:38 Draw a Center Diameter Circle for the Sweep Command
11:00 How to Use the Sweep Tool in Fusion
11:28 Apply a Black Plastic Appearance to the Electrical Cable
11:48 Add a Metal Black Oxide Coating in Fusion
11:59 Use a 1500 Lumen Lightbulb Appearance in Fusion
12:33 Set Up a Photobooth Rendering in Fusion (1920×1080)
12:46 Pros and Cons of This Honeycomb Workflow in Fusion
13:25 More Honeycomb Pattern Tutorials in Fusion