PartDesign Revolution

Introduction
The Revolution tool creates a solid by revolving a selected sketch or 2D object about a given axis.



Above: sketch (A) is revolved 270 degrees counter-clockwise around axis (B); resulting solid (C) is shown right.

How to use

 * 1) Select the sketch to be revolved. v0.17 and above A face on the existing solid can alternatively be used.
 * 2) Press the  button.
 * 3) Set the Revolution parameters (see next section).
 * 4) Press.

Options
When creating a revolution, the Revolution parameters dialogue offers several parameters specifying how the sketch should be revolved.

{|
 * [[Image:partdesign_revolution_parameters.png|left]]

Axis
This option specifies the axis about which the sketch is to be revolved. By default only the horizontal or vertical sketch axis can be selected here. However if the sketch which defines the feature to be Revolved also contains a construction line (or lines), then the drop down list will contain one custom sketch axis for each construction line. The first construction line created in the sketch will be labelled Sketch axis 0.

v0.17 and above Other selectable options are:
 * Base (X/Y/Z) axis: selects the X, Y or Z axis of the Body's Origin;
 * Select reference...: allows selection in the 3D view of an edge on the Body, or a datum line.

Angle
This controls the angle through which the revolution is to be formed, e.g. 360° would be a full, contiguous revolution. The images in the examples section demonstrate some of the possibilities with specifying different angles. It is not possible to specify negative angles (use the Reversed option instead) or angles greater than 360°.

Symmetric to plane
If checked, the revolution will extend half of the specified angle in both directions from the sketch plane.

Reversed
If checked, the direction of revolution is reversed from default clockwise to counterclockwise.
 * }

Properties
Below are properties which can be defined after creation of the feature. Data properties Base, Axis and Angle are uneditable.


 * : name given to the operation, this name can be changed at convenience.
 * : true or false. See Symmetric to plane.
 * : true or false. See Reversed.
 * : v0.17 and above true or false. If set to true, cleans the solid from residual edges left by features. See Part RefineShape for more details.

Useful links
A detailed example of use on the forum.