Overview#
Revolve sweeps a profile around an axis. Anything that could be made on a lathe is a candidate: shafts, pulleys, bottles, vases, bearings housings, knobs, wheels, and chess pieces. Revolve is also the simplest way to build a cone, torus or sphere with exact control over the profile.
A revolve needs two things: a profile (coplanar sketch profiles or planar faces) and an axis (Autodesk lists a linear sketch curve, an edge, a cylindrical face, or an axis). The axis may lie in the sketch plane, or may be a model edge. It cannot cross through the interior of the profile if you want a valid solid; the profile must sit on one side of the axis.
Where to find it#
- Workspace: Design.
- Tab / panel: Solid tab > Create > Revolve.
- Shortcut: none listed in Autodesk's shortcut reference. Press S (Model Toolbox) and type "Revolve".
- Surface tab: Surface > Create > Revolve produces a surface body from an open profile.
Step by step#
- Sketch the profile. On the XY plane, draw the half cross-section of the part. For a shaft with a shoulder, draw the outline of the upper half only, including the segment that lies on the centerline.
- Add an axis line. Draw a line along the rotation axis. Convert it to a construction line (X) if you do not want it to count as profile boundary. A construction line is still selectable as the axis.
- Dimension. Use diameters by selecting the axis line and the far point with the Sketch Dimension tool, then dragging the dimension to the other side of the axis so Fusion shows a diameter. Dimensioning by diameter makes the sketch match shop drawings.
Note: not confirmed in Autodesk's documentation: the drag-across-the-axis diameter behavior. Check the value Fusion shows when you place the dimension.
- Finish the sketch.
- Start Revolve. Choose Create > Revolve. The profile selector is active.
- Select the profile. Click the shaded region.
- Select the Axis. Click the axis selector, then click the axis line, a construction axis, or an edge.
- Choose the Extent Type. Full revolves 360 degrees. Partial revolves by an Angle you drag or type, with Direction One Side, Two Sides or Symmetric. To Object revolves up to a body, face, plane or vertex (Direction One Side or Two Sides).
- Choose the Operation (Join, Cut, Intersect, New Body, New Component) and confirm.
Worked example: a stepped shaft#
- Sketch on XY: a horizontal construction line from the origin to 100 mm along X.
- Draw a closed profile above it: 0,0 to 100,0 (on the axis), up 10 mm to y = 10 at x = 100, back to x = 60 at y = 10, up to y = 15 at x = 60, back to x = 0 at y = 15, close to the origin.
- Revolve, profile = the region, axis = the construction line, Full.
Result: a 30 mm diameter shoulder (0 to 60) and a 20 mm diameter end (60 to 100). To change diameters later, edit the sketch dimensions, not the revolve.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Project Axis | Projects the axis onto the same plane as the profile. | Uncheck it to keep the axis in its original location. |
| Profile | The sketch region(s) or planar face to rotate. | Open profiles produce surfaces only on the Surface tab. |
| Axis | A linear sketch curve, edge, cylindrical face, or axis. | Must not cross the profile interior. |
| Extent Type: Full | 360 degree revolve. | Default. |
| Extent Type: Partial | Revolve by a specified angle. | Direction One Side, Two Sides or Symmetric. Symmetric revolves the profile symmetrically on each side of the profile plane. |
| Extent Type: To Object | Revolve up to a body, face, plane or vertex. | Direction One Side or Two Sides. |
| Direction: Two Sides | Revolves the profile on each side of the profile plane. | |
| Operation | Join, Cut, Intersect, New Body, New Component. | Revolve Cut is how you make grooves and recesses. New Component is Hybrid design only. |
| Objects to Cut | Cut/Intersect only: Auto-Select recomputes the bodies from visibility; "# Bodies" keeps the original ones. | Only active when editing. At creation, visible bodies participate and hidden ones do not. |
Tips and pitfalls#
Tip: Use a revolved Cut to make O-ring grooves, snap-ring grooves, and retaining-ring seats. Sketch only the small rectangle in the groove location on a plane through the shaft axis, and revolve it around the shaft centerline.
Tip: Sketch on a plane that contains the axis. If your axis is the model's Z axis, the profile must lie on the XZ or YZ plane (or any plane containing Z).
Warning: If the profile crosses the axis, the revolve fails or produces a self-intersecting solid. Trim the profile at the axis.
Warning: A profile that only touches the axis at a single point produces a singular vertex at the tip. This is fine for a cone or sphere, but can cause trouble later with fillets or shells at that vertex.
- Revolve around an edge of a body to create features that swing about an existing edge, such as a hinge knuckle.
- A circle drawn in the profile whose center is off the axis revolves into a torus. The distance of the center from the axis is the major radius.
- When you need a sphere, revolve a semicircle 360 degrees; for a hemisphere dome, revolve a quarter circle.
- For threads or helical features, use Coil (Create > Coil) rather than Revolve; Revolve cannot advance along the axis.
- A full revolve creates a seam edge on the cylinder face. Surface tools that run across the seam, such as a loft, may need the seam moved. You can rotate the profile start by sketching on a different plane.
- For parts with true diameters, remember sketch dimensions measured from the axis are radii unless you use the diameter dimension option.
Planning a revolve with real numbers#
Radius versus diameter. Sketch dimensions from the axis are radii unless you dimension across the axis. A shaft listed as 30 mm diameter is a 15 mm dimension from the axis. A frequent error is a 30 mm dimension producing a 60 mm shaft.
Volume check. Once revolved, a quick sanity check with Properties catches radius errors. A 30 mm diameter, 60 mm long cylinder has volume pi x 15^2 x 60 = 42,412 mm3. A 20 mm diameter, 40 mm long end adds pi x 10^2 x 40 = 12,566 mm3. The stepped shaft in the worked example should total about 55,000 mm3 (note the example earlier puts a 30 mm diameter section from x = 0 to 60 and a 20 mm section from 60 to 100). If the volume is four times too large, you dimensioned diameters as radii.
Partial angles. A 90 degree Partial revolve of a rectangle 10 mm tall and 5 mm wide, 20 mm from the axis, makes an elbow section of a rectangular duct with a 20 mm inner bend radius. Direction Symmetric spreads the revolve across both sides of the profile plane, which is handy for features centered on a plane, such as a curved slot; the docs do not say whether the Angle is the total or per side, so check the preview.
To Object. Revolve a rib profile until it meets a selected face; if the face moves, the extent follows. Good for features that must end at a mating surface.
Axis choices#
The axis may be a sketch line, a construction axis, a model edge, or a cylindrical face (the help lists linear sketch curve, edge, cylindrical face or axis). A cylindrical face gives you the true center automatically, so a revolved groove around an existing bore stays concentric even when the bore moves. By default Fusion projects the axis onto the profile's plane; if the axis sits in a different location, uncheck Project Axis to keep it where it is.
Worked example: an O-ring groove and snap-ring seat#
On a 30 mm diameter shaft:
- Sketch on a plane through the axis, drawing a rectangle 3.0 mm wide (along the shaft) located 8 mm from the shaft end. As general guidance (not Autodesk data), an O-ring of 2.4 mm cross-section with about 15 percent squeeze needs a groove roughly 2.0 mm deep (2.4 x 0.85), so the rectangle goes 2.0 mm down from the shaft surface.
- Revolve with Operation Cut around the shaft centerline, Full.
- For a 1.2 mm wide snap-ring seat on a 30 mm shaft, a groove diameter of 28.6 mm (depth 0.7 mm) is a plausible figure for external retaining rings; this is general guidance, so confirm against the ring supplier's table.
Revolve versus other tools#
| Shape | Best choice | Reason |
|---|---|---|
| Shaft, wheel, knob | Revolve | One profile, exact diameters |
| Sphere or torus | Revolve (or primitives) | Exact surfaces |
| Spring, thread | Coil | Revolve cannot advance along the axis |
| Hollow bowl of constant wall | Revolve a closed offset profile, or revolve a solid and Shell | Both work; offset profile gives exact control |
| Square or hex shaft | Extrude | Not rotationally symmetric |
Hollow parts#
For a hollow revolved part (a pipe fitting, a bearing housing), draw both the outer and inner outline in the profile and select the region between them. The wall then stays a sketch dimension. If you instead revolve a solid and Shell, fillets become offset surfaces automatically but the wall is less directly editable.
Failure modes and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| Revolve fails or self-intersects | Part of the profile crosses to the other side | Trim at the axis; the profile must sit on one side |
| Revolve produces a surface, not a solid | The profile is open | Close the sketch (a line along the axis counts) |
| Result is twice the size expected | Radius entered as diameter | Re-dimension; check Properties volume |
| Axis not selectable | Axis lives in a hidden sketch or is not linear | Show the sketch, use a construction axis |
| Cut revolve removes from the wrong body | Several bodies overlap | Hide the others before cutting, or edit and use Objects to Cut |
| Tiny sliver around the seam | Profile touches the axis at a point that is not on the axis exactly | Add a Coincident constraint to the axis line |
| Fillet fails at a cone tip | Singular vertex | Fillet before revolving, in the sketch, or end the tip with a small flat |
Practice exercise#
Model a wine glass and a shaft with grooves, validating each by numbers.
- Sketch the glass profile on the XY plane about a vertical axis at x = 0: a base disc 40 mm radius and 3 mm tall, a stem 4 mm radius running 60 mm high, and a bowl rising to 35 mm radius at 90 mm above the base. Draw the bowl as a closed region between an outer spline and an inner offset 1.5 mm inside (use Sketch > Offset).
- Revolve 360 degrees as a New Body.
- Use Inspect > Section Analysis through the center to check the 1.5 mm wall. Use Properties to read the volume and then Material of glass (density about 2.5 g/cm3) to estimate the mass.
- Edit the bowl radius in the sketch to 30 mm and observe the update.
- Shaft: revolve a 30 mm diameter, 100 mm long profile. Add an O-ring groove for a 2.4 mm cord (depth 2.0 mm, width 3.0 mm) 10 mm from the end, using a Revolve Cut. Add a 1.2 mm retaining ring seat 15 mm from the other end.
- Create a 90 degree elbow by revolving a 10 x 5 mm rectangle 20 mm from an axis using Partial, One Side, Angle 90 degrees.
- Break it: let the profile cross the axis by 1 mm and read the error, then trim it.
Expected result: a hollow glass with a measured wall, a grooved shaft, an elbow, and a documented axis-crossing error.
Related#
- Extrude for straight prisms
- Sweep for profile-along-path shapes
- Coil for helical shapes
- Construction geometry for creating the axes you revolve around