Select Shape
SolidExtrude from the main menu bar to add an extruded solid feature to the part in the current viewport. You can add an extruded solid feature only to three-dimensional parts.
You add an extruded solid feature by sketching a two-dimensional cross-section and defining the distance over which to extrude it. A sketch and the resulting extruded solid feature are illustrated in the following figure:
In addition, you can select a center point and specify a pitch that Abaqus/CAE uses to twist the cross-section as it is extruded. Alternatively, Abaqus/CAE can expand or contract the cross-section along a specified draft angle as the cross-section is extruded. For more information, see “Including twist in an extrusion,” Section 11.13.3, and “Including draft in an extrusion,” Section 11.13.4.
To add an extruded solid feature:
From the main menu bar, select ShapeSolidExtrude.
Abaqus/CAE displays prompts in the prompt area to guide you through the procedure.
Tip:
You can also add an extruded 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 extruded 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 extruded. 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 Sketcher to sketch the two-dimensional profile of the extrusion. In the prompt area, click Done to exit the Sketcher and to open the Edit Extrusion dialog box.
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 extrusion direction.
Click 
in the Edit Extrusion dialog box to reverse the extrusion direction, if necessary.
If the arrow direction is difficult to see, use the rotate tool to rotate the part.
Select one of the following end conditions:
Select Blind and enter a value in the Depth field to specify the distance through which Abaqus/CAE will extrude the sketched profile.
Select Up to Face to specify that Abaqus/CAE will extrude the profile up to a selected face.
If desired, do one of the following:
Toggle on Include twist, and enter the pitch. The pitch is the extrusion distance in which a 360° twist would occur. The sketched extrusion profile must include an isolated point that indicates the center of twist.
Toggle on Include draft, and enter the draft angle (greater than –90° and less than 90°). A positive draft angle indicates that external faces of the profile expand and internal faces contract.
Toggle on Keep internal boundaries to maintain any faces or edges that are generated between the extruded 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 extrude the profile.
If you selected the twist option and your sketch includes a single isolated point, Abaqus/CAE uses that point as the center of twist. If your sketch does not include an isolated point, Abaqus/CAE returns to the Sketcher for you to create one. If your sketch contains more than one isolated point, Abaqus/CAE returns to the Sketcher and prompts you to select an isolated point as the center of twist.
If you selected Up to Face, Abaqus/CAE prompts you to select the face to which to extrude the profile. Select a face to meet the following requirements:
the selected face does not have to be parallel to the sketch plane,
it can be a nonplanar face,
it must completely contain the extruded selection, and
it cannot be a datum plane.
