Revolve Features
Revolves add or remove material
by revolving one or more profiles around a centerline. You can create
revolved boss/bases, revolved cuts, or revolved surfaces.
The revolve feature can be a solid, a thin feature, or a surface.
To create a revolve feature,
use the following guidelines:
The sketch
for a thin or surface revolved feature can contain multiple open or closed
intersecting profiles.
The profile
sketch must be a 2D sketch; 3D sketches are not supported for profiles.
The Axis of Revolution can be
a 3D sketch.
Profiles
cannot cross the centerline. If the sketch contains more than one centerline,
select the centerline you want to use as the axis of revolution. For revolved
surfaces and revolved thin features only, the sketch cannot lie on the
centerline.
When you
dimension a revolve feature inside the centerline, you produce a radius
dimension for the revolve feature. When you dimension across the centerline,
you produce a diameter dimension for the revolve feature.
You must rebuild the model to display the radius or diameter
dimension symbol.
To create a revolve feature:
Create
a sketch that contains one or more profiles and a centerline, line, or
edge to use as the axis around which the feature revolves.
Click one
of the following revolve tools:
Revolved Boss/Base 
(Features
toolbar) or Insert,
Boss/Base, Revolve
Revolved Cut 
(Features
toolbar) or Insert,
Cut, Revolve
Revolved Surface 
(Surfaces
toolbar) or Insert,
Surface, Revolve
In the
PropertyManager,
set the options.
Click 
.
