How to Combine Surface and Solid Modeling in Fusion (Previously Fusion 360) to Make a Vase
If you’re looking to expand your Fusion skills, this tutorial walks you through a hybrid approach using both surface and solid modeling tools to design a beautiful, 3D-printable vase. Whether you're designing for fun or production, this method gives you added flexibility and control over your geometry.
Note: Fusion was previously known as Fusion 360. Some older tutorials and documentation still use that name.
The full video tutorial is embedded at the bottom of this post if you prefer to follow along visually.
Step 1: Start with a New Component and a Circle Sketch
Following Fusion’s golden rule, we begin by creating a new component.
Next, sketch a center diameter circle on the horizontal construction plane, positioned at the origin. Set its diameter to 100 mm to match the tutorial's dimensions. A circle gives you better control for the later steps.
You’ll only be working with a small segment—specifically 1/8 of the circle, or 45 degrees. To do this, draw construction lines that define a 22.5-degree angle on either side, which gives you a total of 45 degrees.
Once the lines are in place, fully constrain the sketch. Black lines mean your geometry is locked in, which makes your model more predictable.
Step 2: Use a Loft Between Offset Planes
Set an offset plane 200 mm above the base sketch. Create a new sketch on that plane and use the Project tool to link the geometry from the lower sketch.
Offset the projected sketch outward by 30 mm. This new shape still represents 1/8 of the circle and will align correctly when patterned later.
With both sketches in place, use Surface > Loft to connect the open profiles. Since they aren’t closed loops, use the Surface Loft, not the Solid Loft.
Step 3: Design a Custom Profile with Splines
Create another offset plane, this time in front of the model—about 150 mm away. This gives you enough working room.
Sketch a Fit Point Spline that defines the curve of the embossed design. Begin the spline above the model, then bring it down past the surface for better control. Keep it rough—this is just a first draft.
Adjust the spline’s curvature and length using the green handles. Then, offset the spline to make a second one. These will stay linked, so changes to one update the other.
Use the Line tool to connect the spline endpoints and form a closed profile. Once the profile fills with a light blue color, it’s ready to be mirrored.
Step 4: Mirror, Thicken, and Emboss
Mirror the closed profile using the vertical construction plane as your mirror plane. Select both splines and lines.
Now thicken your surface body 2 mm inward. If the arrow points the wrong way, just use -2 mm. Make sure to set the operation to New Body.
Then activate the Emboss tool, select both closed profiles, and set the effect to “Emboss” with a depth of 2 mm. No alignment adjustments are necessary.
Step 5: Add Fillets and Prepare for Patterning
Before patterning, add fillets to the embossed edges. You can use the Rolling Ball setting or select individual edges to fine-tune the look.
Fillet both embossed shapes. Alternatively, you could emboss one and mirror it, but you’d lose the helpful visual reference when editing.
Also, don’t forget to fillet the bottom edge—it’s easy to overlook.
Step 6: Customize the Appearance
Add some polish by editing the Appearance of individual faces. Right-click your color in the Appearance menu to tweak RGB, HEX, or HTML color values. For color inspiration, try using online palette generators.
This step is optional but makes your design more appealing—especially if you plan to showcase it or 3D print in multicolor.
Step 7: Create a Circular Pattern
Save your file before patterning—it’s always a good habit before running complex operations.
Create a circular pattern using the blue Z axis as your reference. Fusion will suggest a quantity of 8, which is perfect since your design is 1/8 of a full circle. Set the pattern type to Full to complete the vase.
Step 8: Seal the Bottom and Final Touches
You’ll still see a hole at the bottom of the vase. You can quickly fill this with a circle, but note: if it’s not linked to the rest of the design, it won’t adjust automatically with changes.
If you extrude the base without a taper, a small gap may appear—fine for dry flowers, but not ideal for watertight use.
Lastly, revisit Appearance to apply finishing touches to the new geometry.
Pros and Cons of This Workflow
Pros:
Focus on one manageable segment (1/8 of the vase)
Easy visual control with linked sketches and mirrored profiles
Flexibility from using surface modeling
Cons:
Some steps like project/trim can be time-consuming
Base extrusions may not always update with other geometry
Requires manual adjustments for watertight designs
This method is great for experimenting with custom geometry while staying organized and efficient in Fusion.
Chapters:
00:10 How to Create a New Component in Fusion
00:20 Draw a Center Diameter Circle in a Sketch
00:36 Convert Circle to Arc with Precise Dimension
01:07 Create Parametric Dimensions in Fusion
01:27 Trim Unnecessary Sketch Geometry
01:46 Create an Offset Plane 200mm from Base
02:07 Project Sketch to a New Offset Plane
02:28 Offset a Projected Sketch in Fusion
02:52 Use Loft with Surface Modeling to Connect Profiles
03:09 Create a New Offset Plane for Side View Sketch
03:28 Save and Version Your Fusion Project
03:48 Sketch and Refine a Fit Point Spline
04:39 Offset a Fit Point Spline Curve
05:14 Close Open Sketch Profiles for Lofting
05:35 Mirror Sketches in Fusion with Fit Point Spline
06:11 Edit Mirrored Sketches by Adjusting Originals
06:34 Thicken Surface to Create a Solid Body
06:57 Emboss Sketch Profiles onto a Solid in Fusion
07:36 Apply Fillets: Rolling Ball vs. Standard Method
08:35 Add Custom Colors Using HTML Color Codes
09:35 Create a Circular Pattern Around the Z Axis
10:16 Surface Modeling Workflow: Pros and Cons
11:57 Do you want to Support The Maker Letters?