Part Modeling > Base Features > Revolve > Working with the Revolved Feature > To Create a Thickened Revolved Feature
To Create a Thickened Revolved Feature
To create a thin solid using an open section, click before you sketch or select the section. Otherwise, Sketcher will consider the open section invalid.
A revolved feature must contain an axis of revolution. Create an axis of revolution either by sketching a centerline with the revolved section, or by selecting existing linear geometry.
1. Click Model > Revolve. The Revolve tab opens.
2. Select a sketch, or to create a sketch, click the Placement tab, click Define, sketch a section, if desired click Sketch > Centerline in the Datum group to create a geometry centerline, and click OK.
* You could also select a sketch first, or select a datum plane or planar surface first, and then click Model > Revolve.
3. If the sketched section does not contain a centerline, click the collector, and then select a linear reference to use as the axis of revolution.
4. To flip the direction of feature creation in relation to the sketching plane, click .
5. Select an angle option from the menu:
Variable. Type an angle value.
Symmetric. Type an angle value.
To Selected. Select a datum point, vertex,  plane, or surface as a reference.
* The terminating plane or surface must contain the axis of revolution.
6. To add thickness to the sketch, do the following:
a. Click .
b. Type a thickness value in the box to the right of .
c. To change the side where the thickness is added, click to the right of the thickness box. You can switch between three modes:
Add thickness to Side 1
Add thickness to Side 2
Add thickness to both sides
7. When the system detects at least one surface that can be used to cap the revolve feature and attach it to the solid geometry, specify how to attach the revolve feature to the model. Click the Options tab, and perform one of the following actions:
By default, the system tries to cap the thickened revolve feature with model geometry. You can cycle through the available geometry by clicking Previous and Next.
When you point to the Section end point 1 or Section end point 2 label, the corresponding end point is highlighted in the graphics window.
The sketch must intersect the solid geometry. The end point of the sketch must intersect either a reference you select, or the extension of the reference.
When the end point of the sketch does not intersect the selected reference, but intersects the extension of the reference, you must add the desired capping geometry as references to the sketch:
1. To edit the sketch, on the Placement tab, click Edit. The Sketch tab opens.
2. Click References. The References dialog box opens.
3. Select the geometry to use as references to cap the feature and attach it to the solid geometry.
4. Click Close.
5. Click OK.
If you do not want to cap the revolve feature with existing model geometry, clear the Cap with model geometry check box. This caps the thickened revolve feature with a surface that is normal to the end of the sketch.
8. To create a double-sided feature, do one of the following actions to define the depth for the second side of the sketching plane:
Click the Options tab and select a depth option for Side 2.
Right-click the drag handle, choose Other Side, and then select a depth option.
Right-click the graphics window and select Side 2.
9. Click .