Select Shape
SolidRevolve from the main menu bar to add a revolved solid feature to the part in the current viewport. You can add a revolved solid feature only to three-dimensional parts.
You add a revolved solid feature by sketching a two-dimensional cross-section and a construction line on a selected face. The construction line serves as an axis of revolution, and Abaqus/CAE creates the solid feature by rotating the cross-section about the axis using a specified angle of revolution. In addition, you can specify a pitch and a direction along the axis of revolution that Abaqus/CAE uses to translate the sketch along the axis of revolution as it revolves the profile. A sketch and the resulting feature, revolved through an angle of 180° with pitch, are illustrated in the following figure:
To add a revolved solid feature:
From the main menu bar, select ShapeSolidRevolve.
Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.
Tip:
You can also add a revolved solid feature using the 
tool, located with the solid tools in the Part module toolbox. For a diagram of the tools in the Part module toolbox, see “Using the Part module toolbox,” Section 11.17.
If desired, specify the method you want to use to select an origin for your sketch of the revolved solid feature. Select one of the following options from the Sketch Origin field in the prompt area:
Select Auto-Calculate to place the sketch origin automatically.
Select Specify to define a custom sketch origin.
Select Session Default to use the custom origin you specified earlier in the session.
Select the planar face from which the solid will be revolved. If no suitable face exists, you can select a datum plane or an orphan element face.
Tip: If you are unable to select the desired planar face, you can use the Selection toolbar to change the selection behavior. For more information, see “Using the selection options,” Section 6.3.
The selected face is highlighted in the viewport.
If you selected Specify as the Sketch Origin method, specify the origin location by clicking a point in the viewport or by entering the three-dimensional coordinates of the origin in the prompt area. You can also set this custom origin as the default origin for all sketches in your session by toggling on Set as session default.
Select an edge and the orientation of the edge on the Sketcher grid. The edge must not be perpendicular to the selected face. By default, the selected edge will appear vertical and on the right side of the Sketcher grid. To choose a different orientation for the edge, click the arrow on the right side of the dialog box and choose an orientation from the list that appears.
Tip: If there is no straight edge with the desired orientation, you can create a datum axis. You can then select the datum axis to control the orientation of the part on the Sketcher grid.
Abaqus/CAE highlights the selected edge, enters the Sketcher, and rotates the part until the selected face aligns with the plane of the Sketcher grid and the selected edge aligns with the grid in the desired orientation.
If you are unsure of the part's orientation relative to the Sketcher grid, use the view manipulation tools from the View Manipulation toolbar to view its position. Use the reset view tool 
to return to the original view.
Use the horizontal 
, vertical 
, angle 
, or oblique 
construction line tools to sketch the axis of rotation. You can position the construction line by selecting a datum axis from the underlying part. You cannot select the datum axis directly; you must select a point from either end of the datum axis.
Use the Sketcher to sketch the two-dimensional profile of the revolved feature; the sketch must not cross the axis of revolution.
In the prompt area, click Done to indicate you have finished sketching the profile and the axis. If the sketch contains more than one construction line, Abaqus/CAE prompts you to select the construction line that will serve as the axis of rotation.
Abaqus/CAE displays the part view that was active prior to entering the Sketcher. The part includes your sketched profile and an arrow indicating the direction of revolution. The Edit Revolution dialog box appears.
In the Edit Revolution dialog box, enter the desired angle of revolution or accept the default value.
Click 
next to Revolve direction to change the arrow direction and the associated direction of revolution.
If desired, toggle on Include translation and enter a positive value for the pitch. The pitch value is the distance through which the profile is translated along the axis of revolution during a rotation of 360°.
An arrow appears to show the axis of revolution and to indicate the direction of sketch translation along the axis. Click next to Pitch direction in the Edit Revolution dialog box to reverse the arrow, if necessary.
If desired, toggle on Sweep sketch normal to path to rotate the sketched profile normal to the path of revolution. This option is available only when Include translation is toggle on.
The initial profile of the feature will be rotated from the sketch plane to create the feature.
Toggle on Keep internal boundaries to maintain any faces or edges that are generated between the revolved solid feature and the existing part. The internal boundaries may create regions that can be structured or swept meshed without having to resort to partitioning.
Click OK to accept the indicated direction and to create the revolved solid feature.
Abaqus/CAE creates the revolved feature using your selected parameters.
