Speed Modeling a Straight Bevel Gear in Fusion Using the SpurGear Add-In
Updated June 24, 2026
Designing bevel gears from scratch can be intimidating, especially if you're still building confidence with lofts, patterns, and parametric workflows in Fusion. In this project, you'll create a straight bevel gear concept by combining the Spur Gear add-in with several core modeling tools to quickly generate a printable gear-like design.
This workflow prioritizes speed and experimentation over strict component management. Along the way, you'll practice sketching, revolves, lofts, circular patterns, construction geometry, and several techniques that translate well to 3D printing.
What You'll Learn
- How to create a shaft profile using a revolve workflow
- Why fully constrained sketches improve model stability
- How to project geometry between sketches for parametric updates
- How to use the Spur Gear add-in to generate gear teeth quickly
- How to build a straight bevel gear concept using lofts and circular patterns
- How to perform quick quality checks using Section Analysis
- Why certain modeling decisions produce more reliable 3D printable geometry
- How to use Fusion (formerly Fusion 360) tools efficiently for concept development
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 Shaft Sketch
Start a sketch on a vertical construction plane.
Create a two-point rectangle as a rough framework for the shaft profile. This rectangle is only used as a visual guide while sketching the shaft shape that will later be revolved.
Sketch the profile loosely at first. Focus on establishing the overall shape before worrying about exact dimensions.
Fusion automatically adds sketch constraints as you draw. These constraints help maintain relationships between sketch entities and can significantly reduce editing time later.
Keep an eye on sketch colors:
- Blue geometry is under-constrained
- Black geometry is fully constrained
For early concept work, under-constrained sketches are often acceptable. As the design matures, fully constrained sketches become increasingly important because they behave more predictably when dimensions change.
A fully dimensioned sketch defines the shaft profile used to create the base bevel gear body. The profile consists of a 165 mm long rectangle with a 45 mm overall height and serves as the foundation for the revolve operation later in the workflow. Creating a complete cross-sectional profile before modeling helps maintain a fully parametric design that can be adjusted through sketch dimensions.
Step 2: Add Curves and Fully Define the Sketch
To make the shaft more interesting, add an arc to part of the profile.
The Trim command removes excess sketch geometry from the shaft profile. A semicircular cutout and stepped profile are being refined by deleting overlapping segments while preserving the intended shape. Trimming simplifies the sketch and prevents multiple profile regions from interfering with downstream features such as Revolve.
Instead of trying to draw the perfect shape immediately, use an iterative workflow:
- Sketch extra geometry
- Trim away what you don't need
- Add dimensions afterward
This "oversketch and trim" approach is often faster than attempting to create a perfect sketch from the start.
The shaft profile has been fully defined with dimensions controlling lengths, offsets, radii, and shoulder locations. Features include a 10 mm offset, a 20 mm wide slot with a 10 mm radius arc, and several stepped diameters. Applying dimensions and constraints at this stage improves model stability and ensures design intent is preserved when parameters change later.
After trimming, you may notice previously black geometry turns blue. Fusion will display a warning indicating that constraints were removed during the operation.
In this example, the missing constraint is restored by adding a dimension between the sketch endpoint and the origin. This fully defines the profile again.
A warning indicates that constraints or dimensions were removed during a sketch operation. This commonly occurs when geometry is deleted, trimmed, or replaced. Reviewing the sketch after such warnings is important to verify that critical dimensions remain intact and that the profile is still fully constrained before creating solid features.
Step 3: Revolve the Shaft
Before creating the revolve, trim away any unnecessary sketch geometry.
This leaves a clean profile that is easier to edit later.
Launch the Revolve command and select:
- The remaining closed profile
- The center axis
Fusion automatically detects the profile in many cases, making the operation quick.
Because the revolve is parametric, you can return to the sketch through the timeline and update the shaft shape at any time.
For 3D printing, revolved geometry often creates smooth, continuous surfaces without unnecessary edges or transitions that could complicate slicing.
The Revolve command converts the shaft sketch profile into a solid body by rotating it 360 degrees around a central axis. Revolve is well suited for rotationally symmetric components such as shafts, hubs, pulleys, and gear blanks because a single sketch controls the entire solid model.
Step 4: Create Decorative Shaft Features
Apply an appearance to the face you'll sketch on.
The Appearance dialog is used to assign a blue anodized aluminum material finish. Fusion allows appearances to be applied to entire bodies, components, or individual faces. Applying materials during modeling helps distinguish features visually and improves presentation quality for renders and design reviews.
This is purely a visual aid but makes sketching significantly easier. Using the same appearance planned for the final model also helps visualize the finished design.
Create a new sketch and project the underlying geometry.
A new sketch is created directly on the circular shaft face that was highlighted with a blue appearance. Selecting the correct face before starting the sketch establishes the sketch plane for subsequent projected geometry and tooth profile creation. Using a visually distinct face helps avoid accidentally selecting adjacent cylindrical surfaces or construction planes.
Projected geometry remains linked to the source geometry, which means future modifications to the original sketch can automatically update dependent features.
The Project tool converts an existing model edge into sketch geometry. The outer circular edge of the shaft is projected into a new sketch, creating a linked reference that updates automatically when the source geometry changes. Projected geometry provides accurate references for secondary features and helps maintain parametric relationships throughout the design.
Sketch a feature profile using projected circles as trimming boundaries.
A rectangular sketch feature is created on top of the projected circular face. The geometry is centered along the vertical axis and dimensioned relative to the projected edge. Establishing feature geometry directly from projected references ensures accurate placement and reduces the likelihood of alignment errors.
Several approaches could work here, including:
- Sketch and Extrude
- Loft
- Rib
- Surface modeling workflows
The rectangular sketch has been refined by trimming unnecessary segments and narrowing the profile to a 2.5 mm width. The resulting shape forms the basis for a tooth or cutting feature used later in the bevel gear modeling process. Simplifying sketch geometry before creating solids reduces complexity and produces cleaner downstream operations.
In this example, a sketch-based workflow is used because it is fast and easy to modify. The sketch is then converted into a solid body using an Extrude operation, allowing the overall shape to be updated quickly by editing the original sketch dimensions.
A tooth profile is extruded 60 mm along the shaft using the Extrude command with the operation set to New Body. Creating the tooth as a separate body simplifies patterning and editing before combining it with the main gear body.
Step 5: Add a Full Round Fillet
Before creating a pattern, apply a Full Round Fillet.
This has several advantages:
- Easier to create before patterning
- Updates automatically if the sketch changes
- Remains intact if the pattern quantity changes later
Parametric features become much easier to manage when they're introduced early in the design process.
For 3D printing, fillets also help reduce stress concentrations and improve visual appearance.
The Full Round Fillet command is used to blend the tooth profile into the shaft. This creates a smooth transition between faces and removes sharp edges that would otherwise remain after the extrusion.
Step 6: Create a Circular Pattern
Create a circular pattern of the body feature.
Use:
- Distribution Type: Full
- Quantity: 30
The quantity of 30 is simply an example and not based on any specific engineering requirement.
Because the design was created around the origin, selecting the pattern axis becomes straightforward.
Keeping models centered on the origin often simplifies future patterning, mirroring, and assembly operations.
The patterned tooth body is duplicated around the shaft using a Circular Pattern. The gear axis is selected as the rotation axis and the quantity is set to 30, creating a complete tooth layout around the pitch diameter.
Step 7: Generate the Spur Gear
Measure the shaft diameter before creating the gear.
In this example, the diameter measures:
- 90 mm
The Measure tool is used to verify the finished gear diameter. The selected circular edge reports a diameter of 90 mm, confirming that the modeled geometry matches the intended design dimensions before generating the mating gear.
Open:
Utilities → Scripts and Add-ins → SpurGear
The Spur Gear sample script is selected from the Scripts and Add-Ins dialog. This built-in utility generates an involute spur gear based on user-defined parameters such as module, pressure angle, and tooth count.
Run the Spur Gear add-in and modify:
- Module: 4
This produces a gear with a:
- Pitch Diameter: 96 mm
The gear is created as a new component centered at the origin.
Using the built-in gear generator is significantly faster than manually creating involute tooth geometry and provides access to standardized gear parameters.
The Spur Gear script parameters are configured before generating the gear. In this example, the gear uses a module of 4 and 24 teeth. These values determine the pitch diameter and tooth geometry required for proper meshing.
Step 8: Position the Gear
Use the Move command with:
The generated spur gear body is rotated using the Move/Copy command. Reorienting the gear aligns it with the existing model and prepares it for positioning relative to the bevel gear geometry.
- Move Type: Point to Point
Avoid using joints here.
Although joints are extremely useful in assemblies, this workflow modifies the gear geometry directly and is not being treated as a traditional assembly.
Carefully select:
- Origin Point
- Target Point
Fusion's snapping tools make it easy to locate geometric centers and align components accurately.
After positioning, inspect the model from multiple angles using the ViewCube.
The Point to Point move option is used to accurately position the generated gear. Matching reference points provides precise placement without manually entering offsets or dimensions.
Step 9: Isolate a Single Gear Tooth
Expand the Spur Gear operations in the timeline.
The Spur Gear feature is expanded in the timeline to reveal the operations created by the script, including sketches, extrusions, fillets, and the circular pattern that generates the teeth. Examining the feature structure makes it easier to identify which operations can be edited, suppressed, or removed when adapting the generated spur gear into a bevel gear workflow.
Delete:
- The gear pattern
- The gear base
The Circular Pattern feature that created the gear teeth is removed from the timeline. Deleting the pattern leaves the underlying construction features available, allowing the workflow to reuse the original tooth geometry for the bevel gear design.
The original spur gear body is deleted from the timeline, leaving only the geometry needed for the bevel gear workflow. Removing unnecessary features helps simplify the model and prevents unwanted dependencies later in the design process.
This leaves a single tooth body.
Rotate the tooth using:
- Angle: -45°
A single tooth body is rotated around the gear axis using the Move/Copy command. The rotation angle is calculated from the tooth count to position the tooth correctly before creating the bevel gear tooth pattern.
The tooth body is rotated by -45 degrees to align it with the intended bevel gear geometry. This adjustment changes the tooth orientation relative to the gear axis and prepares it for the construction geometry used in later steps.
This isolated tooth becomes the foundation for creating the bevel gear geometry.
Using the Spur Gear add-in this way saves considerable modeling time while still allowing full customization afterward.
Step 10: Create the Loft Framework
Create a 3D sketch on the vertical construction plane.
A new sketch is started after positioning the tooth body. The sketch will be used to create guide geometry that defines the cone shape and tooth alignment required for the bevel gear.
The sketch is created on a plane that passes through the gear axis. Using a central plane makes it easier to construct the reference lines and angles needed to define the bevel gear profile.
Draw a construction line from the shaft center.
A horizontal sketch line with a length of 100 mm is created from the gear center. This reference line serves as a construction aid for locating the virtual apex of the bevel gear cone.
The previously created line is converted to construction geometry. Construction lines help define relationships and dimensions without contributing to profiles that could accidentally be used for solid features.
The exact length is not important.
Create a second construction line:
- Starting at the tooth center
- Angled downward at 135°
An angled guide line is added from the end of the reference line, creating a 135-degree relationship. This geometry helps establish the cone angle used to shape and position the bevel gear teeth.
The angle comes from:
- 180° − 45° = 135°
Trim the excess construction geometry and finish the sketch.
These construction lines act as a guide for both loft direction and length.
Unneeded sketch segments are removed using the Trim tool, leaving only the guide geometry required for the bevel gear construction. Cleaning up the sketch makes later operations easier to select and modify.
Step 11: Create the Bevel Tooth Loft
Launch the Solid Loft command.
A Loft feature connects the tooth profile near the large end of the gear to a smaller profile near the apex. This creates the tapered tooth shape required for a straight bevel gear. The operation is set to Join so the tooth becomes part of the existing body.
Select:
- The tooth end face as Profile 1
- The construction-line intersection as Profile 2
Before confirming the loft:
- Hide the shaft body
- Ensure the loft joins only the tooth geometry
- Apply a full round fillet
A Full Round Fillet smooths the tooth tip by replacing sharp transitions with a continuous rounded surface. This produces a cleaner tooth form and removes unnecessary sharp edges that can cause modeling or manufacturing issues later.
This prevents accidental joins to unwanted geometry.
Lofts are particularly useful for creating bevel gear concepts because they gradually transition geometry between different diameters and angles.
Step 12: Pattern the Lofted Tooth
Create a circular pattern using the newly created loft feature.
Settings:
- Distribution Type: Full
- Rotation: 360°
Because everything was centered around the origin from the start, the patterned teeth align cleanly around the shaft.
At this stage you'll notice a gap behind the patterned features, which will be filled next.
The completed tooth is duplicated around the gear axis using a Circular Pattern. The pattern distributes 24 instances evenly over 360 degrees, creating the full set of bevel gear teeth while maintaining consistent geometry.
Step 13: Fill the Rear Section
Place a Point at Vertex where the patterned geometry ends.
The Point at Vertex construction tool is used to reference the apex of the bevel gear cone. This point serves as a precise geometric reference for later operations and helps maintain alignment with the gear's theoretical pitch cone.
Use Solid Loft to connect:
- The circular profile
- The newly created point
A Loft operation is prepared using the circular face of the gear and the apex point as profiles. This creates a conical reference surface that represents the bevel gear geometry and can be used for analysis or subsequent modeling operations.
Operation:
- Join
This creates a smooth transition and completes the rear section of the bevel gear.
The lofted conical surface is created between the gear face and the apex point. Using the Join operation integrates the new geometry into the existing model and establishes a continuous cone extending from the bevel gear.
Step 14: Perform a Section Analysis
Create a Section Analysis to inspect the internal geometry.
If the section appears on the wrong side:
- Use the Flip option
Section Analysis is one of the fastest ways to identify:
- Internal gaps
- Intersections
- Unexpected geometry problems
Performing these checks early can prevent wasted print time later.
A Section Analysis cuts through the model to reveal internal geometry. This view makes it easier to verify tooth placement, shaft features, and overall symmetry without creating permanent modifications to the design.
Step 15: Flatten the Top Surface
Create a construction plane slightly in front of the model.
An Offset Plane is positioned relative to existing geometry and extended toward the gear apex. Construction planes like this provide stable sketch locations for downstream features without altering the solid model.
Sketch a Center Rectangle on the plane.
A centered square sketch is created on the offset construction plane. Diagonal construction lines establish the center point, allowing the sketch to remain aligned with the gear axis and adapt predictably if dimensions change.
Use Extrude Cut to remove the top portion of the model.
This creates a flat surface for the next operation.
A more advanced workflow could use parametric construction geometry that automatically updates when the model changes, but this simplified approach is faster for concept work.
The square sketch is extruded as a Cut operation through the front portion of the model. This removes excess material beyond the desired boundary and produces a clean, controlled termination of the bevel gear geometry.
Step 16: Cut the Center Hole
Create a circular sketch on the newly flattened surface.
A sketch is created on the flat end face of the bevel gear. Using the newly created planar surface as a sketch plane allows additional features, such as shaft holes and mounting geometry, to be positioned accurately relative to the gear axis. Creating sketches directly on existing faces reduces the need for extra construction geometry and keeps the timeline easier to manage.
A new sketch is created on the flat end face of the bevel gear. A centered circle defines the diameter of the shaft hole and remains aligned with the gear axis through the sketch origin.
Use Extrude Cut and cut:
- Through the entire model
The circular sketch profile is extruded as a Cut operation through the gear body. Creating the hole after the main geometry is complete simplifies the workflow and allows the shaft diameter to be adjusted independently.
Avoid using a fixed cut depth.
Cutting through all geometry is generally more robust because the operation automatically adapts if the model thickness changes later.
For 3D printing, this reduces the risk of incomplete cuts after future design revisions.
Step 17: Apply Final Appearance and Review
An appearance from the Fusion material library is applied to the bevel gear. Visual materials help distinguish components, improve rendered presentations, and make it easier to evaluate the final design before manufacturing.
The completed bevel gear includes the patterned teeth, center hole, and applied appearance. The model is ready for rendering, assembly work, design validation, or export for manufacturing and downstream engineering workflows.
At this point, the straight bevel gear concept is complete.
This workflow intentionally prioritizes speed over strict project organization.
For production-ready designs, you would typically:
- Separate components more carefully
- Manage bodies more systematically
- Apply appearances later in the workflow
- Create stronger parametric relationships
For concept development, however, this approach allows you to move quickly and test ideas without excessive setup.
Why This Workflow Works Well for 3D Printing
Several decisions in this project naturally support additive manufacturing:
- Lofted transitions reduce abrupt geometry changes.
- Full round fillets improve strength and appearance.
- Circular patterns create consistent tooth spacing.
- Through-all cuts remain stable during design changes.
- Revolved geometry produces clean surfaces that slice reliably.
When preparing a real bevel gear for printing, you'll also want to consider:
- Print orientation
- Layer direction relative to gear loads
- Material selection
- Tooth clearance
- Shaft tolerances
These factors often have a greater impact on performance than the CAD model itself.
Key Takeaways
- Start with simple sketches and refine them later.
- Fully constrained sketches provide greater design stability.
- Projected geometry helps maintain parametric relationships.
- The Spur Gear add-in is a fast way to generate gear geometry.
- Lofts are excellent for creating bevel gear concepts.
- Full Round Fillets are easier to manage before patterning.
- Section Analysis is an effective quality-control tool.
- Designing around the origin simplifies patterning and positioning.
- Through-all cuts are usually more robust than fixed-depth cuts.
- Fast concept workflows are valuable when exploring design ideas.
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Interested in more Fusion workflows for product design, surface modeling, and 3D printable parts? These tutorials explore different approaches to creating functional products, organic forms, and prototype-ready geometry using many of the same sketching, modeling, and refinement techniques used in this bevel gear project.
Each project focuses on practical Fusion workflows that can be applied to product development, prototyping, and 3D printing. The techniques transfer well between mechanical parts, consumer products, and custom designs intended for manufacturing or digital distribution.
Chapters:
00:10 Fusion Sketching: How to Create a 2-Point Rectangle
00:37 Make a Sketch for Revolve in Fusion (formerly Fusion 360)
00:48 Add Parametric Dimensions to a Sketch
00:58 Understand Sketch Color: Blue vs Black Lines
01:19 Automatic Sketch Constraints in Fusion
01:33 Draw and Dimension an Arc
02:10 Trim Tool in Fusion: Clean Up Sketch Lines
02:48 How to Fully Define a Sketch with Constraints
03:06 Refine Sketch and Use the Revolve Tool
03:28 Apply an Appearance to a Face in Fusion
03:52 Project a Sketch for Linked Geometry
04:50 Extrude a New Solid Body from a Sketch
05:14 How to Add a Full Round Fillet
05:29 Create a Parametric Circular Pattern
05:59 Model a Bevel Gear Head in Fusion
06:20 Generate Gears with the Spur Gear Add-In
07:00 Use Point-to-Point Move for Component Placement
08:03 Modify the Spur Gear Component
08:38 Rotate a Body Precisely in Fusion
09:14 Set a New Pivot Point for Rotation
09:40 Create a 3D Sketch for Complex Geometry
10:10 Add a Construction Line in 3D Sketch Mode
11:00 Loft to a Point for Tapered Geometry
11:52 Apply a Parametric Fillet
12:08 Create a Full Circular Pattern (Full Distribution)
12:39 Loft to a Point at Vertex
13:15 Use Section Analysis to Inspect Your Model
13:44 Set Up an Offset Plane in Fusion
14:18 Extrude Cut the Top Using a Center Rectangle on an Offset Plane
14:59 Cut a Hole to the Bottom Using a Circle Sketch
15:37 Add Appearance and Finalize Your Gear Project