Fusion Tutorial: Soap Holder Design with Pattern on Path for 3D Printing
Design a clean, repeatable soap holder that’s optimized for both 3D printing and STL sales.
What You’ll Learn
- How to build a hybrid soap holder design in Fusion
- Why simple features like Slot, Shell, and Project speed up your workflow
- How to wrap patterns using Pattern on Path
- How to create a clean fit between bodies
- How to design functional patterns
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 Base Shape with a Slot
Start by opening Design Shortcuts (S) and create a sketch on the horizontal construction plane.
Search for the Slot tool and use the overall slot. This is one of the fastest ways to define a rounded rectangular base with consistent curvature. It reduces sketch complexity compared to combining lines and arcs manually.
Slot sketch defining rounded soap holder base in Fusion. Overall slot tool enables fast setup with clean curvature and minimal constraints, ideal for parametric 3D printing workflows.
Set the dimensions to 100 mm length and 40 mm width, or adjust based on your soap size.
Instead of finishing the sketch, press E to extrude directly. This shortcut keeps your workflow fast and reduces unnecessary clicks.
Extrude the body to 10 mm height. This gives you a low-profile design that prints quickly and uses less filament—important for both prototyping and product margins.
Extrude command creating low profile soap holder base in Fusion. Direct extrusion from the sketch speeds up the workflow and reduces unnecessary steps in solid modeling.
Step 2: Hollow the Body with Shell
Use the Shell tool and set a wall thickness of 3 mm.
Shell is ideal here because it maintains uniform wall thickness automatically. Compared to manually offsetting geometry, it’s faster and more robust—especially if you plan to adjust dimensions later.
Shell tool hollowing the soap holder with uniform 3 mm wall thickness. This ensures consistent geometry and efficient material use for 3D printing.
Step 3: Analyze and Prepare the Side Profile
Switch to Shaded View with Hidden Edges (Ctrl + 5). This view mode makes it easier to read geometry and spot design issues early.
Use Inspect → Measure to check the straight section of the model. You’ll see the center section is 60 mm.
Inspect tool measuring the straight section of the soap holder side. Accurate measurements are critical for centering features and building symmetric designs.
Create a new sketch on this side.
Because the original sketch wasn’t centered on the origin, the view recenters when starting a new sketch. This isn’t critical, but it highlights why origin-centered designs are easier to manage in parametric workflows.
Place a center rectangle and dimension it to 10 × 2 mm.
Center rectangle sketch placed on the soap holder side for a pattern feature. Simple geometry keeps sketches stable and easy to control.
To center it:
- Total width: 60 mm
- Subtract rectangle width: 2 mm → 58 mm
- Divide by 2 → 29 mm offset
This ensures the feature is perfectly centered and symmetric.
Dimensions used to center the rectangle precisely on the side face. This ensures even spacing and symmetry across the final patterned design.
Step 4: Improve Printability with a Chamfer
Inspect the model from different angles—especially the bottom.
Add a 0.5 mm chamfer to the bottom edges.
Chamfers are useful for 3D printing because they reduce sharp edges and improve bed adhesion. They also give the design a more refined, manufactured look.
Chamfer applied to the bottom edge of the soap holder. This improves printability, reduces sharp edges, and gives the model a cleaner finish.
Step 5: Wrap a Pattern Around the Body
Measure the total perimeter of the soap holder using Inspect. The total length is approximately 245 mm.
Perimeter measurement of a soap holder model using the Inspect tool in Fusion. The outer edge loop is selected, showing a total length of 245.664 mm. This value is used to calculate spacing and quantity before applying a pattern around the body.
Extrude cut the rectangle 1 mm deep. This becomes your base feature for the pattern.
Extrude cut operation on the side of a soap holder in Fusion. A narrow vertical rectangle is cut 1 mm into the body to create the base feature for a patterned slot design. The cut is defined as a feature, enabling it to be reused in a pattern along the outer edge.
Use Pattern on Path:
- Select the feature and the edge path
- Change distribution from Extent to Spacing
Spacing gives you direct control over the distance between features, which is more predictable for design iteration.
Set the spacing to around 4 mm, accounting for the 2 mm feature width.
Set Compute Type → Path Direction. This ensures the pattern follows the curvature correctly, instead of repeating identical orientations that can distort along curves.
This creates a clean, evenly distributed pattern around the body.
Pattern spacing adjusted using path direction compute type. This ensures features align correctly along curved geometry without distortion.
Step 6: Create a Parametric Shelf for the Tray
Start a new sketch on the top surface.
Use Project (P) to bring in existing geometry. Projected geometry stays linked (purple lines), which means your sketch updates automatically if the base changes. This is critical for parametric design.
Project tool creating linked sketch geometry on the top surface. This keeps the design parametric and automatically updates with model changes.
Offset the sketch by 1.5 mm to create clearance.
Offset sketch creating clearance between the body and top tray. This prevents tight fits and improves real-world usability after printing.
Extrude cut 2 mm down to form a shelf. This defines where the tray will sit.
Extrude cut forming a recessed shelf for the tray. This defines a clear seating surface and improves assembly precision.
Step 7: Build the Soap Tray as a Separate Body
Create a new sketch on the shelf and use Project again.
Project tool used in a sketch on the soap tray shelf in Fusion. The outer edge of the body is projected as linked geometry, shown in purple, ensuring the sketch updates automatically if earlier dimensions change. This creates a reliable reference for building the tray feature.
Offset by 1 mm, then extrude 1.25 mm upward.
Set the operation to New Body.
Offset sketch defining the inner boundary of the tray pattern. This creates consistent margins and supports a clean visual layout.
Separating bodies is important if you plan to:
- Export parts individually
- Assign different materials
- Convert them into components later
Extrude operation set to new body to create the soap tray. Separating bodies allows for better control, reuse, and component-based design.
Step 8: Design the Top Pattern (Function + Aesthetics)
Create a center rectangle on the tray:
- 34 mm height
- 1 mm width
Center rectangle sketch created on the soap tray surface in Fusion. The rectangle is positioned along the midline and dimensioned to control its width and height, forming the base feature for the patterned cut across the tray. The sketch is aligned symmetrically to ensure an even distribution when patterned.
Extrude cut through the top surface.
This pattern serves two purposes:
- Drainage (prevents water buildup)
- Visual identity (important for product differentiation)
For reusable designs, avoid hardcoding dimensions. Instead, tie them to user parameters or reference geometry.
Center rectangle extrude cut defining the main drainage feature. This combines functionality and aesthetics in a simple, repeatable shape.
Step 9: Use Rectangular Pattern for Symmetry
Use Rectangular Pattern:
- Change object type from Bodies to Features
- Select the extrude cut
Using features instead of bodies keeps the model lightweight and easier to edit.
Set direction to Symmetric.
Always use an odd number of instances when working symmetrically. This keeps the original feature centered, with equal distribution on both sides.
Example:
- Distance: 30 mm
- Quantity: 19
This results in 9 cuts on each side + the center feature, giving a balanced layout.
Pattern spacing adjusted interactively to balance design and function. Iteration helps achieve both visual appeal and effective drainage.
Step 10: Final Optimization for Reuse
Before finishing:
- Convert bodies into components
- Add user parameters for key dimensions
This transforms your model from a one-off design into a reusable system. You can quickly generate variations for different soap sizes or product lines—ideal for STL sales.
Final soap holder design with separate tray and patterned base. The model is clean, parametric, and ready for 3D printing or STL distribution.
Key Takeaways
- Use Slot and Shell to build clean base geometry fast
- Pattern on Path is the most efficient way to wrap features around curved bodies
- Project is essential for maintaining parametric relationships
- Always design with symmetry and odd rectangular pattern counts for clean distribution
- Separate bodies into components for better control and scalability
- Add user parameters to turn a single design into a reusable product system
This workflow is simple, repeatable, and built for scale—exactly what you want when designing for 3D printing and digital product sales.
🧰 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
- 00:10 Hybrid Soap Holder Design in Fusion (Solid Workflow)
- 00:26 Create the Base Slot (Clean Design)
- 00:47 Faster Extrusions in Fusion (Simple Speed Trick)
- 01:09 Fusion Shortcut: Shaded View with Hidden Edges
- 01:26 Sketch on Curved Surfaces (Side Profile Setup)
- 02:21 Add a Bottom Chamfer (Stronger + Cleaner Edges)
- 02:37 Pattern on Path in Fusion (Wrap Around the Body)
- 04:21 Perfect Fit Clearance Using Project
- 05:20 Build the Soap Tray (Separate Body)
- 06:08 Design the Top Pattern (Drainage + Aesthetics)
- 07:16 Select the Right Feature Every Time (Fusion Tip)
- 07:44 Calculate Symmetric Patterns (Clean, Even Spacing)
- 08:20 Final Tips to Improve Your Fusion Workflow
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Learn how to use surface tools like sweep, patch, and stitch to create smooth, organic geometry and turn it into a solid ready for 3D printing.
🐝 Create a Honeycomb Pattern in Fusion (Step-by-Step Guide)Follow a clear workflow for building a parametric honeycomb pattern that can be reused in designs like trays, vents, and lightweight structures.
🧩 Create an Industrial Design Pen Holder in FusionCombine clean design intent with practical modeling techniques to create a polished, functional pen holder optimized for 3D printing.
Together these tutorials show how parametric sketches, patterns, and surface tools can be combined to create strong, efficient geometry for real-world designs and 3D printing projects in Fusion.