How to Design a 3D-Printable Soap Holder with a Honeycomb Lid in Fusion
Want to create a soap holder that’s both functional and stylish? In this step-by-step guide, we’ll show you how to model a printable soap holder with a honeycomb-patterned lid—using Fusion (previously Fusion 360). The final result is fully 3D-printable in materials like PLA, PETG, or any filament you prefer.
Whether you're a beginner or intermediate Fusion user, this project will sharpen your skills in parametric modeling, surface workflows, and design for 3D printing.
Step 1: Create a New Component for the Honeycomb Lid
Start by creating a new component. This keeps your timeline and design organized, which is especially helpful for future 3D printing and assemblies.
Create a sketch on the horizontal plane.
Use the circumscribed polygon tool and start at the origin.
Set the radius to 10 mm (for demo purposes).
Add two construction lines to define the honeycomb directions.
Step 2: Build the Honeycomb Pattern
Use Sketch → Rectangular Pattern.
Select the polygon edges as objects and the construction lines as directions.
Choose “Spacing” for distribution and “Symmetric” for direction.
Set spacing to 22.5 mm and quantity to 10 in each direction.
This creates an oversketched honeycomb layout so you can trim it down later.
Step 3: Create the Frame
Start a Center Rectangle sketch from the origin.
Use 125 mm height and calculate the width using dimensions between polygons.
Use Inspect → Measure or reference-driven dimensions to define the exact width.
Extrude the area between polygons by 2.5 mm.
Step 4: Use Surface Tools for the Lid
Use Surface → Extrude to pull the frame up to the top of your polygon array.
Apply Thicken (3 mm).
If needed, Combine the frame and honeycomb into one body.
Step 5: Create the Soap Box Component
Activate the main component, then create a new component for the box.
Sketch on top of the lid for parametric alignment.
Project the lid’s geometry and offset it ±3 mm to create the profile.
Extrude downward by 25 mm to form the box body.
Step 6: Cut Space for the Lid
Use Combine → Cut (set lid as Tool, box as Target).
Keep Tools checked to retain the lid.
Use Offset Face (e.g., -1 mm) to create clearance for a smooth fit.
Step 7: Add Fillets for Aesthetics and Strength
Use Fillet (2 mm) on all 12 edge corners of the box.
Activate the lid component and do the same.
This improves the look, grip, and durability of your model.
Step 8: Close the Bottom with Patch
Hide the lid and use Patch to fill the box bottom.
Extrude the patch upward by 3 mm, set to Join.
Step 9: Final Touches and Export
Apply material Appearances to visualize the final model.
Drag & drop colors or textures from Fusion’s appearance library.
Save and export your STL or 3MF files for 3D printing.
Tips for Printing
Use PETG for better water resistance.
Adjust clearances based on your printer’s tolerance.
Consider printing a test piece to check fit before committing to a full print.