Part Revolve/pt-br

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:

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

1. Optionally select one or more shapes in the 3D View or in the Tree View.
2. There are several ways to invoke the command:
   • Press the Revolve button.
   • Select the Part → Revolve option from the menu.
3. 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).
4. Press OK to close the task panel.
5. 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

• DadosSource (Link): The shape to revolve.
• DadosBase (Vector): The base point of the revolution axis.
• DadosAxis (Vector): The direction of the revolution axis.
• DadosAxis Link (LinkSub): Link to the edge to use as the revolution axis. Overrides DadosBase and DadosAxis if set.
• DadosAngle (Angle): The angle span of the revolution. If zero and an arc is used for the DadosAxis Link, the arc's span will be used.
• DadosSymmetric (Bool): If true, the revolution is extended symmetrically from the profile.
• DadosSolid (Bool): If true, revolving a closed edge or a closed wire will yield a solid. If False, a shell will result.
• DadosFace Maker Class (String): If DadosSolid is true, the facemaker class to use when converting wires to faces, otherwise ignored.