Speed Up Your Fusion Workflow: Master 3D Sketching and Sweep Cut Design
If you’ve ever wrestled with Fusion’s 3D sketching tools or struggled to get the Sweep command just right—this tutorial is for you. In this guide, you’ll learn how to model an efficient, shellable design using 3D sketching, Sweep Cut, and body management workflows.
Whether you're designing for 3D printing or just want to expand your Fusion modeling skills, this project unlocks faster, smarter workflows that many users overlook.
Let’s jump in.
1. Sketch and Extrude the Outer Cylinder
Begin by creating a new component in Fusion. Start a 2D sketch on the horizontal construction plane, which sets the natural orientation of the object.
Draw a center diameter circle at the origin—I’m using a 50 mm diameter, but feel free to adjust for your project.
Use the E shortcut to launch the Extrude command right from the sketch. Set the height to 75 mm.
2. Hollow the Body with Shell
Use the Shell command to hollow out the body while keeping the bottom intact. A wall thickness of 2.5 mm strikes a good balance between print strength and speed.
3. Create a Second Inner Cylinder
We’ll now build a second, smaller cylinder inside the first.
Instead of redrawing geometry, project the inner circle from the existing sketch to reuse your references. This keeps your design parametric and clean.
Use the Project tool, then Extrude the new circle down to the base of the outer cylinder. Before confirming, change the operation from Join to New Body to keep these as separate bodies.
4. Use Section Analysis to Check Alignment
It’s smart to run a Section Analysis to see the interior. Use a vertical construction plane as the Cut Plane, and reverse its direction for a clear inside view.
You should now see two neatly aligned, separate bodies.
5. Sketch the Knob and Position for the Sweep
Start a new sketch on a central vertical plane. This sketch defines the path for the Sweep Cut operation.
Draw a circle with a 10 mm diameter and position it 25 mm from the top of the main cylinder. Then Extrude it 35 mm in the negative direction (away from the cylinder) to form a protruding knob.
Be sure to switch the operation to New Body before confirming.
6. Move Bodies for the Sweep Path
Use Free Move to shift the knob and the inner cylinder upwards. The goal is to position the knob completely above the main cylinder.
Don’t forget to confirm the new pivot when moving. This setup is key to a successful sweep cut.
7. Build a 3D Sweep Path with Offset Plane and Sketch
Create an Offset Construction Plane from the top of the main cylinder. Offset it to match the center of the knob (in this case, 25 mm).
Begin a 3D Sketch on this plane:
Draw a straight line from the origin to the knob
Add an angled line and define the angle between them
From the knob center, draw a vertical line straight down
Switch to Top View and draw a center diameter circle (70 mm in this case)
Use the Trim tool to clean up the sketch and keep only the geometry needed for the Sweep path.
8. Perform a Solid Sweep Cut
Turn off the inner cylinder visibility to avoid accidental removal.
Activate the Sweep command:
Type: Solid Sweep
Orientation: Perpendicular
Operation: Cut
Path: your 3D sketch
This creates a precise cut through the outer body using the knob as the cutting profile.
9. Combine and Shell the Knob Cylinder
Now that the cut is done, it’s time to merge the knob and inner cylinder. Use Combine > Join to create one solid body.
Then use Shell to hollow it out, again using 2.5 mm wall thickness.
10. Convert Bodies to Components (Optional)
If you're planning assemblies or animations, convert the bodies into components:
Right-click each body in the browser and choose Create Components from Bodies. This is a good practice even for simple projects.
11. Add Clearances and Fillets
Use Offset Face to add a small clearance—0.1 mm—between the knob and the outer cylinder. This is useful for manufacturing or 3D printing.
Apply Fillets to the edges to create a smooth, finished look. These small touches enhance the appearance and usability of your model.
12. Apply Appearances
Wrap up by adding visual finishes:
Apply a matte plastic appearance to match common 3D printing materials.
For a realistic preview, choose standardized Fusion materials.
Looking for more styling options? Check out my custom lampshade tutorial for tips on custom appearances.
Final Thoughts
This Fusion tutorial covered:
3D Sketching for Sweep Cuts
Smart Shelling Techniques
Managing Bodies and Components
Creating Cutouts with Offset Paths
Adding Clearances and Fillets for Manufacturing
These tricks are easy to miss, but once you know them, your Fusion workflows become faster and more flexible—especially for 3D printing projects.
📦 Ready for your next challenge? Try designing a multi-part assembly or an interlocking mechanism.
Watch the Full Video Tutorial
🎥 Prefer to follow along visually? Here’s the full tutorial with all the steps and shortcuts shown on-screen:
Chapters
00:09 Start Your First Sketch in Fusion (formerly Fusion 360)
00:19 Draw a Center Diameter Circle at the Origin
00:29 Extrude the Circle to Begin the Main Form
00:39 Use the Shell Command to Hollow the Cylinder
00:53 Create an Inner Cylinder for Multi-Body Modeling
01:03 Use Sketch Project with Projection Link for Precise Referencing
01:34 Extrude the Inner Profile as a New Solid Body
01:44 Perform a Section Analysis to Check Interior Geometry
02:18 Set Up the Sweep Cut Operation – Beginner-Friendly Workflow
02:28 Sketch on a Vertical Construction Plane
02:39 Add Dimensions to Control Circle Placement
02:53 Extrude Without Cutting – Keep Bodies Separate
03:15 Switch from Cut to New Body in the Extrude Operation
03:26 Use Free Move to Reposition the Knob and Inner Cylinder
04:08 Create an Offset Plane to Align the Sweep Path
04:31 Begin a 3D Sketch for the Sweep Cut Path
04:44 Oversketch a Line to Define the Sweep Direction
04:58 Add a Dimension Between Two Lines to Set the Cut Angle
05:15 Draw a Vertical Line from the Knob Center
05:33 Create a Center Diameter Circle for the Sweep Profile
05:47 Trim Extra Lines to Clean Up the Sketch
06:06 Use Solid Body Sweep Cut for a Clean Opening
06:17 Apply Solid Sweep with Proper Orientation Settings
06:27 Use Perpendicular Orientation for a Consistent Cut
06:56 Combine the Knob and Inner Cylinder
07:13 Select Target and Tool Bodies in the Combine Operation
07:23 Use Shell to Hollow Out the Knob for 3D Printing
07:39 Convert Bodies into Components via the Browser
07:58 Save Your Project – A Key Step in Every Fusion Workflow
08:08 Offset a Face to Create a Small Manufacturing Gap
08:37 Fillet Edges for a Softer, Print-Ready Finish
09:00 Apply Matte Plastic Appearances to Match 3D Print Material
09:19 Watch More Fusion Projects for Beginners – Recommended Videos