How to Design a 3D Printed Honeycomb Soap Holder in Autodesk Fusion
Updated August 25, 2026
A honeycomb pattern can turn a simple soap holder into a lightweight, functional 3D printed product—but the interesting part is building it so the lid and box remain connected parametrically. In this Autodesk Fusion (formerly Fusion 360) tutorial, we’ll create a two-component soap holder while using linked geometry, sketch patterns, surfaces, offsets, and clearance to build a model that is easy to modify and prototype.
What You’ll Learn
- How to organize a Fusion design using separate components for the lid and box
- How to create a honeycomb pattern with a 10 mm polygon radius and 22.5 mm spacing
- How to oversketch patterns instead of calculating every boundary in advance
- How to use construction geometry and referenced dimensions to control a sketch
- How to create a 125 × 85 mm starting footprint and refine it parametrically
- How to combine solid and surface modeling workflows
- How to create a 2.5 mm honeycomb structure and 3 mm frame
- How to project geometry between components so design changes propagate
- How to build a 25 mm deep box around the lid
- How to create 1 mm clearance between 3D printed parts
- How to add 2 mm fillets and a 3 mm bottom
- How modeling decisions such as wall thickness, clearance, and rounded edges affect 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: Create the Honeycomb Lid Component
Start by creating a new component for the honeycomb lid. Give it a descriptive name and make sure the component is active before you begin sketching.
We’ll use two components in this project: one for the lid and one for the box.
This is more than organizational housekeeping. Components give Fusion a clearer design structure and make it easier to manage assemblies, component-specific operations, the parametric timeline, and separate parts intended for 3D printing.
When working with multiple printable parts, this structure also makes it much easier to export and manufacture each component independently later.
Create a New Component before starting the honeycomb soap holder geometry. The component is named Honeycomb lid and activated immediately.
Keeping the lid in its own component separates its sketches and features from the rest of the design, making the Fusion timeline and Browser easier to manage as the model becomes more complex.
Step 2: Sketch the First Hexagon
With the lid component active, create a new sketch on the horizontal construction plane.
Select the Circumscribed Polygon tool and place the polygon from the origin at the center of the canvas. Starting from the origin makes the design easier to constrain, mirror, pattern, and modify later.
Start a sketch and use Circumscribed Polygon to create the first hexagonal cell. The command is accessed here through Fusion's Sketch Shortcuts search.
A six-sided polygon provides the repeating geometry for the honeycomb structure. Building one controlled cell first makes it possible to generate the larger pattern parametrically rather than drawing individual hexagons.
Set the polygon radius to:
10 mm
These dimensions are intended as a demonstration rather than dimensions for a specific commercial soap product.
Place the center of the Circumscribed Polygon directly on the sketch origin and create a six-sided polygon.
Anchoring the initial hexagon to the origin gives the subsequent pattern a stable reference point. This is particularly useful when the honeycomb array will later be positioned relative to the soap holder's overall dimensions.
Next, draw two sketch lines that we’ll use to control the honeycomb pattern. Convert both lines to construction geometry, since they are references rather than physical parts of the final model.
For the line pointing toward the side of the polygon, snap its endpoint to the midpoint of one polygon edge. Fusion should automatically display the midpoint constraint as you approach the correct location.
Set the circumscribed polygon to 10 mm, defining the size of the base hexagonal cell used throughout the honeycomb pattern.
Because every later cell is generated from this original geometry, changing this dimension provides a straightforward way to control the scale and density of the entire pattern.
Step 3: Create the Honeycomb Rectangular Pattern
Activate the Rectangular Pattern tool inside the sketch environment.
Use Sketch > Rectangular Pattern and select all six edges of the hexagon as the pattern objects. Two directions are selected so the cell can be repeated across the sketch in both axes.
Patterning the sketch geometry keeps the honeycomb regular and avoids manually copying and aligning individual cells.
Fusion contains separate rectangular pattern tools for sketches and solid geometry, so make sure you are using the sketch version.
In the Rectangular Pattern dialog:
- Select the polygon edges as the Objects
- Select the two construction lines as the Directions
- Set Distribution to
Spacing - Set Direction to
Symmetric - Set the spacing to 22.5 mm
- Set the quantity to 10 in both directions
Because the polygon radius is 10 mm, its diameter is 20 mm. Using 22.5 mm spacing introduces a small separation between neighboring polygons.
The goal here is deliberately to create more geometry than we need.
Rather than spending time calculating exactly how many hexagons will fit inside the finished soap holder, we can oversketch the honeycomb field and trim or select the geometry we need later. This is often faster and makes the design more flexible while you are still exploring dimensions.
Change the Rectangular Pattern Distribution from Extent to Spacing.
With Spacing, the entered distance controls the interval between neighboring pattern instances rather than the overall size of the complete array. This makes the honeycomb layout easier to control because the relationship between adjacent cells remains consistent as the pattern quantity changes.
Change the pattern Direction from One Direction to Symmetric. This distributes instances on both sides of the original hexagon along the selected axis.
Using a symmetric pattern keeps the original cell at the center of the honeycomb field and makes later positioning relative to the soap holder geometry more predictable.
Apply Symmetric direction to both axes of the Rectangular Pattern while keeping the distribution set to Spacing.
The resulting setup expands the honeycomb from its central reference cell in four directions. This is useful when creating a deliberately oversized pattern that can later be trimmed by the soap holder's final boundary.
Set the Rectangular Pattern to 10 instances with 22.5 mm spacing in both directions. The resulting array creates a honeycomb field substantially larger than the final part.
Creating excess pattern geometry ensures the soap holder boundary can define the final shape without needing to calculate exactly how many individual cells are required beforehand.
Step 4: Define the Soap Holder Footprint
Create a Center Rectangle starting at the origin.
Set its initial dimensions to:
- Height: 125 mm
- Width: 65 mm
The 65 mm width is intentionally temporary. At this stage, the exact required width is awkward to calculate because of the geometry of the polygons.
Starting with an approximate value lets us keep modeling and solve the geometric relationship parametrically instead of interrupting the workflow with manual calculations.
If you accidentally create the rectangle as construction geometry, switch its four lines back to regular sketch geometry. Unlike the construction lines used to define the pattern directions, this rectangle will become part of the actual model.
Create the rectangular boundary for the soap holder over the oversized honeycomb pattern. The visible width is dimensioned to 65 mm, with the boundary centered around the sketch origin.
This boundary establishes the usable area of the honeycomb lid independently of the repeating pattern behind it. The oversized array can therefore be trimmed or used selectively wherever it intersects the final soap holder footprint.
Step 5: Calculate the Correct Width with Construction Geometry
The center rectangle needs to sit correctly relative to the honeycomb geometry, but directly measuring the required distance with the Inspect tool can be unnecessarily cumbersome.
Instead, use construction geometry and sketch dimensions.
A new line is drawn over the existing honeycomb sketch to begin defining the rectangular boundary of the soap holder. The honeycomb geometry remains visible underneath, making it possible to position the boundary relative to the pattern.
This boundary will control which portion of the larger honeycomb pattern becomes part of the finished design.
The boundary geometry is positioned with a 20 mm sketch dimension. Applying dimensions rather than positioning the line visually keeps the soap holder geometry controlled parametrically.
The visible 90° constraint also establishes the orientation of the boundary geometry relative to the adjoining line.
Trim the unnecessary geometry until you can dimension the relevant distance from the polygon center to its side.
Place a dimension on that distance.
The existing sketch construction lines are used as references to position the boundary geometry accurately. A horizontal dimension of 38.971 mm is applied from the central construction geometry to the boundary.
Using the construction geometry as the dimensional reference keeps the boundary tied to the underlying layout rather than positioning it independently. This makes the soap holder dimensions easier to control as the sketch develops.
Then double-click the rectangle dimension you want to control and reference the dimension you just created. Modify the expression by adding:
* 2
The rectangle width is therefore controlled by twice the measured half-width.
Instead of entering another independent numerical value, the opposite boundary dimension is defined using the existing parameter d8 multiplied by 2.
Referencing an existing sketch dimension creates a relationship between the dimensions. If the controlling value changes later, the dependent dimension updates with it rather than requiring manual adjustment.
This is a useful parametric modeling technique because the dimension is no longer just a fixed number. It has a mathematical relationship with another part of the sketch.
If the underlying geometry changes, Fusion can recalculate the dependent dimension automatically.
The completed boundary now encloses the portion of the honeycomb pattern that will form the soap holder. The visible horizontal dimension is approximately 77.942 mm, corresponding to twice the earlier 38.971 mm value.
The rectangular boundary provides a clean limit for the honeycomb geometry before it is converted from sketch geometry into a 3D body.
Step 6: Extrude the Honeycomb Structure
The center rectangle now acts as a boundary for the honeycomb geometry.
Without leaving the sketch, activate the Extrude command and select the areas between the polygons that fall within the frame.
Extrude them by:
2.5 mm
This creates the primary honeycomb structure of the lid.
A relatively shallow extrusion works well for a part like this because the honeycomb geometry provides distributed structure without requiring a thick solid slab. For 3D printing, that can reduce material consumption and print time while retaining a useful amount of stiffness.
The open cells also make sense for a soap holder because they prevent the lid from becoming a large uninterrupted surface.
The enclosed honeycomb profile is selected with Fusion's Extrude command. The extrusion is set to 2.5 mm, with One Side direction, Distance extent type, and New Body as the operation.
This converts the 2D honeycomb layout into the first solid geometry of the soap holder while preserving the open hexagonal cells.
Step 7: Build the Outer Frame with Surface Modeling
Turn the sketch visibility back on if Fusion automatically hid it after the first extrusion.
Switch to the Surface tab and activate the orange Extrude tool.
With the honeycomb geometry visible as a shallow 3D structure, Fusion's command search is used to access Extrude.
The angled view makes the newly created thickness easier to inspect before additional solid geometry is added.
Select the rectangular frame and extrude the surface up to the top of the polygon pattern rather than entering another independent distance.
This creates a parametric relationship between the frame and honeycomb structure. If the height of the honeycomb changes later, the surface can follow that change instead of requiring another manual edit.
Set the operation to:
New Body
A second Extrude operation is previewed at 2.5 mm using One Side, Distance, and New Body. The selected profile follows the perimeter around the honeycomb structure.
Creating this geometry as a separate body keeps the perimeter and honeycomb structure independently editable before they are combined later in the workflow.
Next, activate Thicken and give the surface a thickness of:
3 mm
You can leave the frame as a separate body temporarily.
The combination of surface modeling and Thicken is particularly useful when you want to define the location and shape of a wall first and its physical thickness second.
For FDM 3D printing, 3 mm also creates a substantial frame around the thinner honeycomb structure. The exact printable wall behavior will depend on nozzle diameter, extrusion width, material, and slicer settings, but avoiding extremely thin structural walls generally makes a functional part more robust.
Fusion's Thicken command is applied to the selected perimeter geometry with a thickness of 3 mm. Chain Selection is enabled, the direction is One Side, and the result is created as a New Body.
The operation turns the selected perimeter geometry into a substantial outer frame around the honeycomb lattice. Keeping it separate at this stage makes the frame easier to modify before merging it with the rest of the soap holder.
Step 8: Combine the Honeycomb and Frame
Once you are happy with the frame, combine it with the honeycomb geometry.
Use the Combine command and select the appropriate:
- Target Body
- Tool Body
Confirm the operation so the frame and honeycomb become a unified lid body.
We’ll return to the Honeycomb Lid later. For now, activate the parent component so the next part is not accidentally created inside the lid component.
The honeycomb structure and perimeter frame are brought together using Fusion's Combine command. One solid is selected as the Target Body and the other as the Tool Body, with the Join operation active.
Combining the previously separate bodies creates a unified soap holder body that can be treated as a single solid during the following modeling operations and eventual preparation for 3D printing.
Step 9: Create the Box Component
Create another standard internal component for the box underneath the lid.
Activate the new component immediately.
Keeping the box separate from the lid gives us two independently manageable parts while still allowing them to reference each other parametrically.
This is particularly useful for 3D printing because the two parts can eventually be exported, oriented, sliced, and printed independently.
Create a second standard internal component for the box beneath the honeycomb lid. The New Component dialog has Activate enabled, so subsequent sketches and features are recorded inside the new Box component.
Separating the lid and box into components keeps their parametric timelines organized and makes the two parts easier to manage independently when preparing the soap holder for 3D printing.
Step 10: Project the Lid Geometry into the Box
Create a new sketch on the top of the Honeycomb Lid component.
Rather than manually recreating the lid dimensions, use Fusion’s Project tool to bring its geometry into the box component.
Project the outer edges of the frame.
Projected geometry appears purple, indicating that it remains linked to the original geometry.
This relationship is one of the major advantages of a parametric CAD workflow: the box is being designed from the lid rather than from a duplicate set of manually entered dimensions.
If the lid dimensions change, the projected references can update with them.
With a sketch created on top of the honeycomb lid, use Project to bring the lid’s outer frame geometry into the Box component. The Project dialog shows Projection Link enabled, maintaining a parametric connection to the source geometry.
Rather than recreating the box dimensions manually, the projected geometry allows the box to reference the lid directly. Changes to the original frame can therefore propagate into the dependent sketch.
Step 11: Offset the Box Profile
Use Offset on the projected geometry to create the profiles required for the box walls.
Create offsets of:
- -3 mm outward
- 3 mm inward
This creates the sketch profile we need for the box.
The workflow also demonstrates an alternative to the surface modeling technique used for the lid. Instead of creating a surface and applying Thicken, we are defining the wall thickness directly through offset sketch geometry.
Both techniques are useful in Fusion, and understanding when to switch between solid, sketch-based, and surface workflows can make complex models much faster to build.
Use the sketch Offset command on the projected frame geometry with Chain Selection enabled. Here, the selected rectangular chain is offset by -3 mm.
The offset creates one boundary of the wall profile while preserving the relationship with the projected lid geometry. Using a linked projection followed by an offset avoids manually dimensioning another rectangle.
Create the second offset from the projected frame, this time using a distance of 3 mm. Together with the previous -3 mm offset, this produces the closed sketch regions required for the box walls.
This is a sketch-based alternative to the surface workflow used earlier for the lid frame, where a surface was extruded first and then given thickness with Thicken.
Step 12: Extrude the Box 25 mm Downward
Select the box profile, making sure that both required profile sections are selected.
Extrude downward by:
-25 mm
The negative value simply indicates the extrusion direction relative to the sketch plane.
A 25 mm depth works for this demonstration, but the ideal depth depends on the soap, packaging, or product you intend to fit.
For a real product, this is a good point to prototype. 3D printing makes dimensional experimentation relatively inexpensive: print a quick version, test the proportions and fit, then adjust the parameter in Fusion.
That iterative CAD-to-print workflow is often more useful than trying to predict every ergonomic dimension before making the first physical prototype.
Select both wall profiles and use Extrude to extend them downward by -25 mm. The Extrude dialog confirms that 2 profiles are selected and the operation is creating a New Body.
The 25 mm depth is a demonstration dimension rather than a fixed product requirement. For a functional 3D printed version, this parameter can be adjusted after checking the intended contents or testing a quick prototype.
Step 13: Cut the Lid Shape into the Box
At this point, the lid intersects the box.
Use Combine to create the matching interface.
Set:
- Target Body: Box
- Tool Body: Honeycomb Lid
- Operation:
Cut - Keep Tools: Enabled
Keeping the tool is important because we still need the lid as a separate printable component.
This operation effectively uses the lid itself to define the corresponding geometry in the box, reducing the need to reproduce complicated dimensions manually.
Use Combine with the box as the Target Body and the honeycomb lid as the Tool Body. Set the operation to Cut and enable Keep Tools.
The cut transfers the lid geometry directly into the box while preserving the original lid body. Keeping the tool is essential here because the honeycomb lid remains a separate component needed for the finished assembly and 3D print.
Step 14: Add 1 mm Clearance for 3D Printing
A mathematically perfect fit in CAD is usually not a physically useful fit after 3D printing.
The resulting box now contains a recessed frame derived directly from the honeycomb lid geometry. The lid is hidden so the newly created interface can be inspected clearly.
At this stage the geometry matches too closely for a practical printed fit. Nominally matching CAD surfaces do not account for dimensional variation from extrusion, material behavior, or printer calibration, so clearance is added next.
The lid is currently too tight, so activate Offset Face and enter:
-1 mm
This pushes the relevant face outward and creates additional clearance around the lid.
The ideal clearance depends on your printer, material, layer height, extrusion calibration, print orientation, and the type of fit you want. A sliding lid needs different tolerances from a press fit or snap fit.
The 1 mm clearance used here is therefore a practical starting point rather than a universal rule.
For functional 3D printed parts, designing clearance directly into the CAD model is much more reliable than expecting two nominally identical surfaces to fit perfectly after printing.
Select the four inner faces around the lid interface and activate Offset Face. The dialog shows all four faces selected with a distance of -1 mm.
This moves the faces outward to create clearance between the box and honeycomb lid. The ideal fit depends on the printer, material, slicer settings, and desired amount of movement, so the 1 mm clearance used here should be treated as a starting point rather than a universal tolerance.
And before continuing, save your project if you haven’t already.
Save the Fusion design after completing the Offset Face operation. The version description records the model state after the clearance adjustment.
Saving at meaningful milestones is particularly useful in a parametric project with linked components. It provides a clear version point before moving into finishing operations such as fillets and the bottom of the box.
Step 15: Add 2 mm Fillets to the Box
Next, soften the corners using the Fillet command.
There are three edges per corner and four corners, giving:
12 selected edges
Fusion displays the selection count in the interface, which makes it easier to confirm that you have not missed an edge.
Set the fillet radius to:
2 mm
Fillets improve the appearance and handling of the soap holder, but they can also be useful for functional 3D printed designs.
Sharp transitions can create stress concentrations, while rounded transitions distribute loads more gradually. Rounded external corners are also more comfortable to handle and make a printed product feel more finished.
Use Fillet to round the vertical corner edges of the box. Three edges are selected at each of the four corners, giving 12 edges total; Fusion’s selection counter in the lower-right corner provides a quick way to confirm that none have been missed.
Set the fillet radius to 2 mm. The rounded transitions soften the appearance and handling of the box while removing sharp corner geometry from the finished 3D printed part.
Step 16: Add 2 mm Fillets to the Lid
Activate the Honeycomb Lid component before creating the next fillets.
This ensures the operations are recorded in the correct component context and timeline.
Apply another:
2 mm fillet
to the corresponding lid edges.
When finished, turn the box visibility back on and inspect the two components together.
Keeping component activation under control becomes increasingly important as Fusion designs grow more complex. A clean timeline makes later edits considerably easier to understand.
Activate the Honeycomb Lid component before adding the final corner treatment so the feature is recorded in the correct component timeline. Select the four outer corner edges of the lid frame and open the Fillet command.
Set the fillet radius to 2 mm, matching the rounded treatment previously applied to the box. Using the same radius on both components gives the assembled soap holder a consistent edge profile while removing sharp corners from the 3D printed lid.
Step 17: Close the Bottom with the Patch Tool
The box still needs a bottom.
Instead of creating another sketch, switch to the surface tools and activate Patch.
Orbit underneath the model, hide the lid if necessary, and select the open boundary. Patch creates an infinitely thin surface across the opening.
Orbit underneath the box and use the Patch tool to close the open bottom. Select the connected boundary edges around the opening; with Enable Chaining active, Fusion can follow the continuous perimeter rather than requiring every segment to be handled independently.
Patch creates an infinitely thin surface across the opening rather than immediately adding solid material. This avoids creating another sketch and provides a surface that can be converted into the physical bottom in the next operation.
Now extrude that patched surface:
3 mm upward
Set the Extrude operation to:
Join
This converts the previously open geometry into a closed solid with a 3 mm bottom.
A substantial bottom is useful for a functional 3D printed container because it provides stiffness and gives the part a stable base. It also avoids relying on an extremely thin floor that may flex or depend too heavily on only a few printed layers.
Select the patched surface and use Extrude to give the bottom physical thickness. Set the distance to 3 mm and the operation to Join, integrating the new geometry with the existing box body.
The result is a 3 mm thick solid bottom rather than the zero-thickness surface created by Patch. This thickness gives the 3D printed box a substantial base while completing the previously open solid geometry.
Step 18: Check the Model for 3D Printing
Before exporting the parts, inspect the completed model as something that will actually be manufactured rather than just as CAD geometry.
The main dimensions and settings used in this project are:
- Polygon radius: 10 mm
- Honeycomb pattern spacing: 22.5 mm
- Pattern quantity: 10 × 10
- Initial rectangle height: 125 mm
- Initial rectangle width: 85 mm
- Honeycomb extrusion: 2.5 mm
- Frame thickness: 3 mm
- Box offsets: -3 mm outward / 3 mm inward
- Box depth: -25 mm
- Lid clearance: -1 mm
- Box fillets: 2 mm
- Lid fillets: 2 mm
- Bottom thickness: 3 mm
For FDM printing, think about how each component will sit on the build plate. The large, relatively flat geometry of the box gives you a natural print orientation, while the honeycomb lid should be oriented so the lattice does not require unnecessary support material.
Support-free or low-support geometry generally prints faster, uses less material, and produces cleaner surfaces than designs that rely heavily on steep unsupported overhangs.
Also check the honeycomb connections and 3 mm structural sections in your slicer. Actual printable behavior depends on your nozzle and extrusion width, so always inspect the sliced toolpaths rather than assuming that every CAD feature will translate perfectly to an FDM print.
Step 19: Add Appearances and Finish the Design
With the functional modeling complete, you can add appearances to make the design easier to visualize.
Open the Appearance library and drag and drop a material or appearance onto each component.
This does not change the physical geometry, but it is useful when presenting a concept, creating renders, or comparing different product styles before printing.
You can also assign contrasting appearances to the lid and box to make the two-component construction easier to see.
The final result combines several useful Autodesk Fusion (formerly Fusion 360) workflows in one relatively compact project: sketch patterns, construction geometry, referenced dimensions, surface modeling, Thicken, linked projections, Offset, Combine, Offset Face, fillets, and Patch.
With the modeling complete, open Fusion’s Appearance panel to change the visual finish of the honeycomb soap holder. The library is filtered for a glossy yellow appearance, which can be dragged directly onto a body or component.
Appearances change how the model is displayed without altering its geometry or 3D printing dimensions. They are useful for exploring color combinations, distinguishing the lid from the box, and preparing cleaner product renders before exporting the finished parts for printing.
Key Takeaways
This soap holder is a useful example of designing around relationships rather than simply entering dimensions.
The 10 mm polygon radius, 22.5 mm honeycomb spacing, and oversized 10 × 10 pattern let us generate the lattice quickly without calculating every cell individually. The 125 mm frame dimension then defines the useful region of that larger sketch.
Separating the lid and box into components allows us to project geometry from one part into another. That means the box can respond to changes in the lid instead of being modeled as an unrelated object with duplicated dimensions.
The project also demonstrates two approaches to creating wall thickness: surface extrusion plus a 3 mm Thicken operation for the lid frame, and offset sketch profiles for the box.
Most importantly, CAD dimensions are not the same thing as manufactured dimensions. The -1 mm Offset Face clearance acknowledges that 3D printed components need tolerance, while the 2 mm fillets and 3 mm structural sections help turn a geometric model into a more practical physical object.
That combination of parametric modeling and rapid physical testing is where Fusion and desktop 3D printing work especially well together.
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