Design a Soap Holder STL That Can Sell Online | Fusion + 3D Printing
Designing practical 3D printable products is one of the fastest ways to improve your Fusion workflow while building models that can actually sell. In this project, you’ll create a modern soap holder and tray using a hybrid workflow that combines solid modeling, sketch patterns, and Form tools in Autodesk Fusion.
The result is a clean-looking STL file optimized for FDM printing in materials like PLA and PETG, while also giving you a strong foundation for future parametric edits and product variations.
What You’ll Learn
- How to structure a Fusion project with components
- Why internal components are often better for product design workflows
- How to combine shell, chamfer, and pattern tools for cleaner geometry
- How to create printable rectangular and honeycomb patterns
- Why linked projections improve parametric editing
- How to build a removable soap tray with proper print clearance
- How to use the Form environment to create ergonomic curvature
- How to optimize geometry for reliable FDM printing
- Why timeline-friendly workflows make future iterations easier
Step 1: Set Up Components in the Hybrid Workspace
Start inside the Hybrid workspace and create both components before modeling. Components are especially useful in product design because they improve organization, simplify assemblies, and make print preparation easier later.
Activate the last component you create, this is useful because you can jump directly into modeling the correct component.
If you create external components, Fusion opens the Edit In Place dialog when editing geometry. External components are powerful for reusable design libraries because they can be inserted and linked across projects. For this workflow, though, internal components are usually the cleaner option since they reduce prompts and simplify navigation.
After creating the components, clean up the browser structure before moving into sketching.
Component setup for the soap holder and tray inside the Fusion Hybrid workspace before starting the modeling workflow.
Step 2: Create the Soap Holder Base Sketch
Create a sketch with a footprint of 100 by 60 mm. This size works well for smaller soap bars while still printing quickly and efficiently.
You can always scale the STL proportionally in your slicer later if you need a larger version.
There are two common approaches for corner fillets:
- Add fillets later in the solid environment
- Add fillets directly inside the sketch
Keeping sketches simple is generally good practice, but sketch fillets can save time in this situation because both the inner and outer corners resolve automatically during the extrude.
Base sketch for the soap holder with rectangular dimensions and rounded corners prepared for extrusion.
Extrude the profile to 20 mm using the Extrude command shortcut E. A 20 mm height gives a good balance between durability, print time, and material usage.
Extruded solid body for the soap holder showing the main outer shape before shelling and pattern features.
Step 3: Prepare the Pattern Features
Create two simple sketches for the side cut pattern. Splitting the setup into separate features makes the timeline easier to manage later, especially because the long and short sides use different layouts.
If you want more control over future versions, this is a good point to introduce user parameters. Parameters make it easier to scale spacing, wall thickness, and dimensions without rebuilding the model manually.
Sketch geometry used to create the side cut pattern for the soap holder using extrusion features.
Before applying the side patterns, use the Shell command and set the wall thickness to 3 mm.
This sequence matters.
If you apply the patterns before shelling, the Shell command has to process all the openings, which can create uneven internal walls and unpredictable geometry. Shelling first gives cleaner and more controllable results.
Soap holder model after using the Shell command to create consistent wall thickness for 3D printing.
Add a bottom chamfer afterward. A small chamfer improves bed adhesion, reduces sharp edges, and helps the print look more refined straight off the build plate.
Bottom edge chamfers added to the soap holder to improve print quality and edge transitions.
Step 4: Create the Long Side Pattern
Extrude the long-side cut feature separately from the short side feature. Keeping them isolated in the timeline gives you better flexibility when editing patterns later.
Set the extrusion extent type to All so the cut automatically adapts if the model height changes later.
Extrude Cut operation creating the first slot feature for the soap holder side pattern.
Use a Rectangular Pattern set to Features, select a horizontal axis, and switch the direction to Symmetric.
Using Symmetric distribution keeps the pattern centered automatically, which is especially useful in parametric designs because it prevents drifting geometry when dimensions change later.
For the distribution method, use Extent. This method controls the total span instead of manually controlling each spacing value.
The side length is 100 mm. After subtracting the 5 mm fillets on each end, you are left with 90 mm of usable straight distance for the pattern.
Use an odd quantity to keep the pattern perfectly centered around the original feature.
Rectangular pattern applied symmetrically across the long side of the soap holder.
Mirror the completed pattern across the original construction plane. Selecting features directly from the timeline is usually the cleanest way to avoid accidentally selecting the wrong geometry.
One major advantage of using Mirror this way is that future edits to the original pattern automatically update the mirrored result.
Mirrored rectangular pattern copied to the opposite side of the soap holder using the center construction plane.
Step 5: Create the Short Side Pattern
Repeat the workflow on the short side.
Again, use an extrusion with the extent type set to All so future height changes update automatically.
Extrude Cut operation creating the second slot feature for the soap holder side pattern.
This time, use the Spacing distribution mode inside the Rectangular Pattern command.
Each cut is 1 mm wide. By using a spacing value of 2.25 mm with 23 instances, you create approximately 1.25 mm of material between each opening.
Rectangular pattern configuration for the short side of the soap holder using spacing distribution.
That spacing prints reliably with standard 0.4 mm nozzles while still keeping the pattern visually open and lightweight.
The original 60 mm footprint combined with the corner fillets leaves roughly 50 mm of usable straight distance, which gives the short side a balanced appearance similar to the long side.
Mirror the feature using the center construction plane.
Step 6: Create the Soap Tray Shelf
Create a sketch on top of the soap holder and project the upper geometry into the sketch.
Keep Projection Link enabled.
Linked projections are extremely useful in parametric workflows because the projected geometry updates automatically if earlier dimensions change. That reduces rebuild work significantly during later iterations.
Linked projected sketch geometry used to create the support shelf for the removable soap tray.
Offset the projected profile by 1 mm and use Extrude Cut to cut the shelf downward by 5 mm.
Offset sketch geometry defining the outer frame and clearance for the soap tray component.
This creates the support ledge where the soap tray will rest.
Extrude Cut operation creating the recessed shelf where the soap tray will rest.
Step 7: Build the Soap Tray
Activate the soap tray component and start a new sketch directly on the shelf surface.
Project the profile and offset it by 0.5 mm to create print clearance between the tray and the holder.
Projected geometry on the tray surface used as the base for the removable soap tray design.
Offset profile creating print clearance between the soap tray and the outer holder.
Adding intentional clearance is critical in functional 3D printing. Without it, even small material expansion differences can cause parts to bind together after printing.
Instead of creating a traditional solid extrusion immediately, create a thin profile and use Press Pull to control thickness afterward.
Soap tray frame extruded 5 mm to create the removable insert for the soap holder assembly.
This workflow keeps the timeline cleaner and makes future thickness adjustments easier.
Set the tray thickness to 2.5 mm. Together with the earlier 0.5 mm offset, this creates a solid overall structure that prints reliably in PLA or PETG.
Offset Face adjustment used to refine tray thickness and improve print tolerances.
Finish by adding a 2.5 mm fillet to the inner corners. Rounded internal corners improve durability because stress concentrations are reduced compared to sharp corners.
Rounded inner tray corners created with fillets for smoother geometry and improved durability.
Step 8: Create the Honeycomb Pattern
Start a sketch on top of the tray and place a circumscribed polygon at the center origin with a radius of 3 mm.
Honeycomb polygon sketch created at the center of the tray surface for the drainage pattern.
Use the L shortcut to create a helper line and press X to convert it into a construction line.
Construction lines are useful because they provide directional references without becoming part of the final geometry.
Circumscribed polygon and construction line setup used for the honeycomb sketch pattern.
Create a Rectangular Pattern inside the sketch using the polygon as the patterned object.
Set the spacing to 7.6 mm. Since the polygon diameter is 6 mm, this leaves roughly 1.6 mm between cells.
That spacing gives enough structural strength while still printing cleanly with standard nozzle sizes.
Use Symmetric direction settings so the pattern expands evenly from the center.
Increase the quantity until the pattern extends beyond the tray frame.
Oversketching is completely fine here because only the geometry inside the projected tray boundary will become part of the final model.
Symmetrical rectangular pattern distributing honeycomb cells across the tray surface.
Step 9: Extrude the Honeycomb Geometry
Project the tray boundary into the honeycomb sketch and keep it linked.
Projected tray boundary controlling the final honeycomb geometry inside the sketch.
Extrude the honeycomb profiles to the same height as the tray frame.
Set the operation to Join if you want a single solid body.
If you plan to work with multi-color printing or advanced 3MF workflows, setting the honeycomb to New Body can be smarter because it gives you better control later in the slicer.
This is one of those workflow decisions that depends entirely on how you plan to manufacture the part.
Honeycomb geometry extruded and joined into the soap tray body for the drainage surface.
Honeycomb tray detail showing the patterned surface and adjusted tray depth.
Step 10: Add Curvature Using Form Tools
Switch into the Form environment to create curvature inside the tray.
Press and hold the left mouse button to bring up the face selection menu and choose the correct face.
Face selection inside the Form environment before creating curvature in the soap tray.
Place a box at the origin with dimensions of 40 by 80 mm.
This acts as a reference shape that approximates the soap geometry while giving you smooth curvature control.
Form box positioned at the origin with dimensions used to shape the soap support curvature.
Use the ViewCube to inspect the model from different angles, then move the form body downward by approximately 2.5 mm using the Move command.
Form body repositioned to refine the soap support cutout inside the tray model.
Finish the Form edit and return to the solid environment.
Step 11: Cut the Soap Support Geometry
Use Combine with the operation type set to Cut.
Select the soap tray as the target body and the form body as the tool body.
Fusion workflow showing the Combine command with the operation type set to Cut. The soap tray body is selected as the target body, while a form body shaped like a soap bar is selected as the tool body. This setup cuts a curved recess into the tray to match the shape of the soap for improved fit and drainage.
Previewing the operation from multiple angles before confirming is good practice because it helps catch incorrect selections before Fusion generates the final result.
The finished tray now has two usable sides:
- One flat side for larger soap bars
- One curved support side for smaller soap pieces
That gives the printed part longer practical usability over time.
Step 12: Final Clearance Adjustment
As a final tweak, offset the inside tray face by 0.5 mm to slightly increase the shelf margin.
Small tolerance adjustments like this are common in functional product design because real-world print variation often differs slightly from CAD-perfect geometry.
This type of final iteration is where Fusion’s timeline-based workflow becomes especially valuable.
Final Offset Face adjustment increasing tray clearance and improving fit between the tray and holder.
Key Takeaways
- Components improve organization and print preparation
- Shelling before patterning creates cleaner internal geometry
- Linked projections simplify future parametric edits
- Symmetric patterning helps maintain centered geometry
- Intentional print clearances improve real-world functionality
- Press Pull workflows keep the timeline cleaner and easier to edit
- Honeycomb spacing must balance strength and printability
- Form tools are excellent for ergonomic surfaces and organic shapes
- Timeline-friendly workflows make future product iterations much easier
- Small tolerance tweaks can significantly improve print usability
🧰 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
- 00:12 Set Up the Components and Clean Your Browser
- 00:50 Create the First Sketch for the Soap Holder
- 01:29 Extrude the Soap Holder and Apply Fillets
- 02:31 Shell and Chamfer the Main Body
- 03:00 Create the First Pattern Feature
- 03:20 Apply a Rectangular Pattern on the Long Sides
- 04:59 Apply a Rectangular Pattern on the Short Sides
- 05:39 Mirror the Pattern Features Across the Model
- 06:01 Create the Shelf for the Soap Tray
- 06:52 Start Building the Soap Tray Component
- 07:04 Create the Soap Tray Sketch
- 08:27 Build the Honeycomb Pattern Sketch
- 10:05 Extrude the Honeycomb Pattern and Frame
- 11:09 Create a Soap Replica in the Form Workspace
- 12:03 Shape the Honeycomb Pattern with Surface Curvature
You Might Also Like
If you enjoyed this Fusion project, here are three related tutorials that explore soap holder workflows, silicone mold design, and parametric honeycomb modeling for 3D printing.
Learn how to design a functional soap holder in Fusion using parametric sketches, shell features, patterns, and workflows optimized for clean PETG and PLA prints.
🧪 Create a Silicone Mold in Fusion for 3D PrintingFollow a practical Fusion workflow for building a silicone mold design with clean geometry, accurate clearances, and features suited for 3D printing and casting applications.
🐝 Create a Honeycomb Pattern in Fusion (Step-by-Step Guide)Build a reusable parametric honeycomb pattern in Fusion and learn techniques useful for lightweight trays, ventilation designs, and structural 3D printing projects.
Together these tutorials demonstrate how Fusion workflows like parametric modeling, Combine operations, patterns, and clean solid modeling techniques can be used to create practical products optimized for 3D printing.