To Create a Revolved Wall
Use the Revolve tool to create a revolved wall.
1. Click > > 
Revolve. The Revolve tab opens.
Revolve. The Revolve tab opens.2. Select a sketch or click > and create an internal sketch to revolve.
3. Under Axis, click the collector and select an axis of revolution. When you define the sketch, the centerline of the sketch is selected as the axis of revolution.
The axis of revolution can be a geometry centerline created as part of the sketched section. The centerline is automatically detected during feature creation. You can also select any existing linear geometry that lies on the sketch plane, such as an axis, or a straight edge or curve to define the axis of revolution.
4. Select an angle of revolution option from the Angle list:
◦ 
Variable—Revolves a section from the sketching plane by a specified angle.
Variable—Revolves a section from the sketching plane by a specified angle.◦ 
Symmetric—Revolves a section on each side of the sketching plane by half of the specified angle in each direction.
Symmetric—Revolves a section on each side of the sketching plane by half of the specified angle in each direction.◦ 
To Reference—Revolves a section to a selected point, plane, or surface.
To Reference—Revolves a section to a selected point, plane, or surface.5. Set the angle value in the Angle box. Click 
to flip the direction of the revolve creation in relation to the sketching plane.
to flip the direction of the revolve creation in relation to the sketching plane.6. The thickness of a first wall can be changed only when the body is not linked to the part. Type a value for the wall thickness in the Thickness 
box, or accept the default value. Click 
to change the side the thickness is added.
box, or accept the default value. Click to change the side the thickness is added.7. To create a two-sided feature that is constructed on both sides of the sketching plane, perform the following actions:
a. Click Options. The Options tab opens.
b. Select an option to constrain the angle of revolution for Side 1 and Side 2.
c. Set the angle value or the reference plane for each side.
8. To create the new wall as a new body or to add the new wall to a different body, click Body Options. The Body Options tab opens.
◦ To create a new body, select the Create new body check box. A new body is created.
Click Link to part to link the preferences of the new body to the part preferences.
◦ To add the new wall to a different, existing body, select the body in the Model Tree or graphics window. The name updates in the body collector.
9. To set sheetmetal-specific options, use the Options tab to perform one or more of the following actions:
◦ Click Add bends on sharp edges to round sharp edges when the sketch includes nontangent geometry. Set the value of the radius and the location for dimensioning the radius.
◦ To set options for merging an additional wall to the model, set the options below:
▪ Select Merge to body to merge the wall to an existing wall in the body. You now have the option to keep the edges of merged geometry and edges of bend surfaces. This option is not available for a first wall.
▪ Select Do not merge to body to keep the new geometry as a disjoint volume. You now have the option to flip the driving surface of the sheet metal.
10. To set feature-specific bend allowance and calculate the developed length using a different method from that of the body, perform the following operations:
a. Click Bend Allowance. The Bend Allowance tab opens.
b. Click Use feature settings.
c. Perform one of the following operations:
▪ Click By K factor or By Y factor and type a new factor value or select one from the list.
▪ To use a bend table to calculate developed length for arcs, click By bend table. Use the default table, select a new one from the list, or click Browse to browse to a different table.
 | Only bend tables copied to the part are available. |
11. Click 
.
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