Part Revolve
Appearance
|
|
| Menu location |
|---|
| Part → Revolve |
| Workbenches |
| Part |
| Default shortcut |
| None |
| Introduced in version |
| - |
| See also |
| None |
Description
The Part Revolve command revolves the selected object around a given axis. The following shape types are allowed, and lead to the listed output shapes:
| Input shape | Output shape |
|---|---|
| Vertex | Edge |
| Edge | Face |
| Wire | Shell |
| Face | Solid |
| Shell | Compound solid (Compsolid) |
A Sketch can be used as well. Solids or compound solids are not allowed as input shapes. Normal compounds are currently not allowed either.
Example of revolution
Usage
- Optionally select one or more shapes in the 3D View or in the Tree View.
- There are several ways to invoke the command:
- Press the
Revolve button.
- Select the Part →
Revolve option from the menu.
- Press the
- The Revolve task panel opens.
- Optionally click on an item in the Shape list to (re-) select a shape.
- Optionally keep Shift pressed and click on an item in the Shape list to either add the shape to the selection, or to remove it from the selection.
- Set the revolution axis and angle and optionally other parameters (see Properties for more details).
- Press OK to close the task panel.
- One Revolve object will be created for each selected shape.
Each input shape is placed underneath its Revolve object.
Task panel

- OK button creates the revolution, and closes the panel.
- Cancel button closes the panel, without doing anything.
- Shape list: here you select which shapes to revolve. If multiple objects are selected, multiple Revolve objects are created.
- Revolution Axis section: specifies the revolution axis.
- Center X/Y/Z fields: set the base point of the revolution axis.
- X-/Y-/Z-Direction fields: set the direction of the revolution axis. Click a button to set the direction to corresponding axis.
- Select Reference button: click it, and then pick an edge in the 3D View. That edge will appear in text field below the button, in the format "ObjectName:EdgeN". You can also type the link manually or erase it. Values X-/Y-/Z-Direction will be filled according to the edge direction.
- Angle field: set angle of revolution in degrees.
- Symmetric angle: if checked, revolution will extend forwards and backwards by half the specified angle.
- Create solid checkbox: if checked, revolving a closed wire or edge will yield a solid. It is checked by default, if a closed wire was preselected before invoking Part Revolve.
Notes
- The Angle argument specifies how far the object is to be turned. The coordinates move the origin of the axis of revolving, relative to the origin of the coordinate system.
- If you select a user defined axis, the numbers define the direction of the revolving axis with respect to the coordinate system: if the Z-coordinate is 0 and the Y and X-coordinates are non-zero, then the axis will lie in the X-Y plane. Its angle is such that its tangent is the ratio of the given X and Y-coordinates.
- App Link objects linked to the appropriate object types can also be used as shapes and to specify the axis.
- If the object to revolve intersects the rotation axis the operation will fail in most cases.
Properties
See also: Property View.
A Part Revolve object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:
Data
Extrude
- DataSource (
Link): The shape to revolve. - DataBase (
Vector): The base point of the revolution axis. - DataAxis (
Vector): The direction of the revolution axis. - DataAxis Link (
LinkSub): Link to the edge to use as the revolution axis. Overrides DataBase and DataAxis if set. - DataAngle (
Angle): The angle span of the revolution. If zero and an arc is used for the DataAxis Link, the arc's span will be used. - DataSymmetric (
Bool): If true, the revolution is extended symmetrically from the profile. - DataSolid (
Bool): If true, revolving a closed edge or a closed wire will yield a solid. If False, a shell will result. - DataFace Maker Class (
String): If DataSolid is true, the facemaker class to use when converting wires to faces, otherwise ignored.
- Creation and modification: New Sketch, Extrude, Revolve, Mirror, Scale, Fillet, Chamfer, Face From Wires, Ruled Surface, Loft, Sweep, Section, Cross-Sections, 3D Offset, 2D Offset, Thickness, Project on Surface, Appearance per Face
- Boolean: Compound, Explode Compound, Compound Filter, Boolean Operation, Cut, Union, Intersection, Connect Shapes, Embed Shapes, Cutout Shape, Boolean Fragments, Slice Apart, Slice to Compound, Boolean XOR, Check Geometry, Defeaturing
- Other tools: Box Selection, Shape From Mesh, Points From Shape, Convert to Solid, Reverse Shapes, Simple Copy, Transformed Copy, Shape Element Copy, Refine Shape, Set Tolerance, Persistent Section Cut, Attachment
- Preferences: Preferences, Fine tuning
- Getting started
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