Revolve
Available in: Sketch, Part Studio
Shortcut: Shift+w
Create, add to, subtract from, or intersect parts by revolving sketch regions or planar faces about a central axis, or surfaces by revolving lines and curves about a central axis.
Video example
Video transcript
The Revolve feature moves selected entities in a curved path around an axis.
Start a new Revolve feature. Select a sketch, a sketch region, sketch entities, a planar face, or a curve as the entities to revolve. Click in the Revolve axis field. Select a linear sketch entity, a linear edge, a linear curve, a cylindrical edge, a circular sketch entity, an arc, or a Mate connector.
Click the Mate connector icon to create a Mate connector in the graphics area. After placing the Mate connector, edit its definition by clicking the Mate connector icon.
Full revolve is checked by default and revolves the selection 360 degrees. Uncheck Full revolve to set an End type. Blind revolves in one direction to a specified angle value. Toggle the Opposite direction arrow to change the direction. Check Symmetric to center the revolve angle on the revolve axis. Up to next terminates the feature when it encounters other geometry, such as a face, vertex, mate connector, part, or the next entity.
Check Offset to set a distance by which the feature falls short of the end condition. Toggle the Flip offset icon to have the distance extend beyond the end condition. Check Second End Position to define independent end conditions for the other end of the revolve. Up to Face revolves up to the infinite face underlying the selected face or plane. Up to Part revolves up to the next part or surface encountered in the specified direction. Up to Vertex revolves up to a selected point, vertex, or Mate connector.
Select the Thin option to revolve a thin solid. Select the faces and sketch regions to revolve, then set the thickness on either side of the selected regions. Toggle the Flip wall arrow to swap which side Thickness 1 and Thickness 2 apply to. Check Mid plane to create symmetry.
Steps for creating solids
From the Sketch or Feature toolbar:
- Click
.
- Select
the tab for the Solid
Creation type:
When Solid is selected at the time a sketch is open, Onshape automatically selects all the closed regions in the sketch.
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
- Select a line, cylindrical edge, or arc to revolve around an axis, or Mate connector (implicit or explicit).
- Activate the Revolve axis field, then click the axis or click
to select an implicit Mate connector about which to revolve.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (see red arrow below) to open a dialog with which to edit the Mate connector:
Click the Mate connector icon to create an implicit Mate connector in the graphics area
- Choose whether you want to:
- New - Create a new solid
- Add - Add to an existing solid
- Remove - Subtract from an existing solid
- Intersect - Keep the intersection of two (or more) solids
- Select an End type. By default, Full revolve is selected, which revolves the selection about the axis 360 degrees. To specify a different revolve end type, deselect the Full revolve checkbox and select one of the following:
- Blind
- To a specified angle (as entered in the Revolve angle field).
- Optionally, click the Tolerance options icon (
) and then the dropdown arrow icon (
) to the left of the parameter in order to set the tolerance Precision and Type. See Tolerance options for more information.
- Optionally, click the Tolerance options icon (
- Up to next - Up to the next face or faces encountered in the specified direction. If it doesn’t completely terminate, then the Extrude fails.
- Up to face - Up to the infinite face underlying the selected face or plane.
- Up to part - Up to the next part or surface encountered in the specified direction.
- Up to vertex
- Up to a selected point (vertex) or Mate connector (implicit or explicit). Click the
in order to select implicit Mate connectors.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (outlined below) to open a dialog with which to edit the Mate connector:
Up to next, Up to Face, Up to part (includes surfaces), and Up to vertex all support revolving with an Offset by a number of degrees.
With Up to face, Up to part (or surface), and Up to vertex, checking Offset to specify a distance for the revolve to fall short of the part, face, vertex, or next entity by the specified distance.
The offset can be inverted by clicking the Flip offset icon (
).See End type examples for details.
- Blind
- To a specified angle (as entered in the Revolve angle field).
- If necessary, select a Merge scope (or Merge with all) to select parts or surfaces with which to merge the new (additional) part or surface. See Merge scope for details.
-
Click
.
Steps for creating surfaces
From the Sketch or Feature toolbar:
-
Click
.
- Select the Surface creation type:
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
- Choose whether you want to:
- New - Create a new surface
- Add - Add to an existing surface
- Select edges or a sketch to revolve.
- Activate the Revolve axis field, then click the axis or Mate connector (implicit or explicit) about which to revolve.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (see red arrow below) to open a dialog with which to edit the Mate connector:
- Select an End type. By default, Full revolve is selected, which revolves the selection about the axis 360 degrees. To specify a different revolve end type, deselect the Full revolve checkbox and select one of the following:
- Blind
- To a specified angle (as entered in the Revolve angle field).
- Optionally, click the Tolerance options icon () and then the dropdown arrow icon () to the left of the parameter in order to set the tolerance Precision and Type. See Tolerance options for more information.
- Optionally, click the Tolerance options icon (
- Up to next - Up to the next face or faces encountered in the specified direction. If it doesn’t completely terminate, then the Extrude fails.
- Up to face - Up to the infinite face underlying the selected face or plane.
- Up to part - Up to the next part or surface encountered in the specified direction.
- Up to vertex
- Up to a selected point (vertex) or Mate connector (implicit or explicit). Click the
in order to select implicit Mate connectors.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (outlined below) to open a dialog with which to edit the Mate connector:
Up to next, Up to Face, Up to part (includes surfaces), and Up to vertex all support revolving with an Offset by a number of degrees.
With Up to face, Up to part (or surface), and Up to vertex, checking Offset to specify a distance for the revolve to fall short of the part, face, vertex, or next entity by the specified distance.
The offset can be inverted by clicking the Flip offset icon (
).See End type examples for details.
- Blind
- To a specified angle (as entered in the Revolve angle field).
- If necessary, select a Merge scope (or Merge with all) to select surfaces with which to merge the new (additional) surface. See Merge scope below for details.
-
Click
.
Steps for creating thin revolves
From the Sketch or Feature toolbar:
-
Click
.
- Select the Thin creation type:
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
- Choose whether you want to:
- New- Create a new solid
- Add- Add to an existing solid
- Remove- Subtract from an existing solid
- Intersect- Keep the intersection of two (or more) solids
- Select faces or sketch region to revolve.
- Do one of the following:
- To create a revolve with a symmetric thickness, check the Mid plane option and then enter the Thickness value.
Optionally, click the Tolerance options icon (
) and then the dropdown arrow icon () to the left of the parameter in order to set the tolerance Precision and Type. See Tolerance options for more information.
- To specify individual wall thicknesses, uncheck the Mid plane option. Then, enter the Thickness 1 wall value and Thickness 2 wall value. Click the Flip wall arrow to flip Thickness 1 with Thickness 2.
Optionally, click the Tolerance options icon (
) and then the dropdown arrow icon () to the left of the parameter in order to set the tolerance Precision and Type. See Tolerance options for more information.
- To create a revolve with a symmetric thickness, check the Mid plane option and then enter the Thickness value.
- Activate the Revolve axis field, then click the axis or Mate connector (implicit or explicit) about which to revolve.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (see red arrow below) to open a dialog with which to edit the Mate connector:
- Select an End type. By default, Full revolve is selected, which revolves the selection about the axis 360 degrees. To specify a different revolve end type, deselect the Full revolve checkbox and select one of the following:
- Blind
- To a specified angle (as entered in the Revolve angle field).
- Optionally, click the Tolerance options icon () and then the dropdown arrow icon () to the left of the parameter in order to set the tolerance Precision and Type. See Tolerance options for more information.
- Optionally, click the Tolerance options icon (
- Up to next - Up to the next face or faces encountered in the specified direction. If it doesn’t completely terminate, then the Extrude fails.
- Up to face - Up to the infinite face underlying the selected face or plane.
- Up to part - Up to the next part or surface encountered in the specified direction.
- Up to vertex
- Up to a selected point (vertex) or Mate connector (implicit or explicit). Click the
in order to select implicit Mate connectors.
Once a Mate connector is selected, click the Mate connector icon in the dialog field (outlined below) to open a dialog with which to edit the Mate connector:
Up to next, Up to Face, Up to part (includes surfaces), and Up to vertex all support revolving with an Offset by a number of degrees.
With Up to face, Up to part (or surface), and Up to vertex, checking Offset to specify a distance for the revolve to fall short of the part, face, vertex, or next entity by the specified distance.
The offset can be inverted by clicking the Flip offset icon (
).See End type examples for details.
- Blind
- To a specified angle (as entered in the Revolve angle field).
- If necessary, select a Merge scope (or Merge with all) to select solids with which to merge the new (additional) solid. See Merge scope for details.
-
Click
.
Revolve: New/Add
New - Create new material that results in a new part.
Add - Create material and add to the existing material.
When adding material, you have the option to merge that material with other parts that touch or intersect its geometry:
- If the geometry touches or intersects with only one part then that part is automatically added to the merge scope.
- If multiple parts touch or intersect the geometry, then there is ambiguity and you must select which parts to merge with (the merge scope).
- A shortcut to selecting multiple touching or intersecting parts, you have the ability to check Merge with all to add all touching or intersecting parts to the merge scope.
If the Boolean is set to Add, Remove, or Intersect and nothing is set in the merge scope, the feature will result in an error. For New, no merge scope is available since New does not boolean the result.
Revolve: Remove
Take material away:
Revolve: Intersect
Leave material only where intersections exist:
End type examples
Full revolve
Revolve about the axis 360 degrees:
Blind
Revolve in one direction for a specified angle:
Blind, Symmetric
Revolve in both directions for the same angle:
Project a selected region or planar face about an axis or Mate connector (implicit or explicit). Create a new part or modify an existing one by adding or removing material, or intersecting parts in its path. You also have the ability to create parts or surfaces.
Up to Entity
Revolves up to a face, vertex, mate connector, part, or the next entity.
Offset
Offset the end by the specified distance. Available for Up to Entity end types.
Second end position
Revolve in two directions for specific angles. Available for Blind and Up to Entity end types.
Merge scope
Merge scope is available with parts and surfaces and allows you to select the specific part or surface with which to merge the newly created part or surface. By default, Merge all is selected. You are able to uncheck that box to access the Merge scope field, then select the part or surface with which to merge. Surfaces must be merged with surfaces and parts with parts.
Merge scope: with all
Merge with all parts that touch or intersect the geometry being created:
Merge scope: with specific part
Merge with selected part:
