2009

Close the file without saving.
Revolve Features
Use the Revolve tool on the Part Feature panel bar to create a feature by rotating
one or more sketched profiles around an axis. The axis and the profile must
be coplanar. If this is the first feature, it is the base feature.
Workflow overview: Create a revolved feature
1 To begin, sketch a profile that represents the cross section of the revolved
feature you want to create. Except for surfaces, profiles must be closed
loops.
2
Click the Revolve tool to display the Revolve dialog box.
If there is only one profile in the sketch, it is automatically selected.
If there are multiple profiles, on the Shape tab click Profile, and then
select the profile to extrude.
Use only unconsumed closed sketches in the active sketch plane.
3 Click Axis, and then select an axis from the active sketch plane.
4 Click Join, Cut, Intersect, or Surface. Surface outputs, along with cut and
intersect operations, are not allowed as base features.
5 In Extents, select Angle or Full.
6 Click a direction button to revolve the feature in either direction or
equally in both directions.
Results are previewed on the model.
60 | Chapter 3 Working with Sketched Features