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.

Select the planar face from which the solid will be extruded. If no suitable face exists, you can select a datum plane.

Tip:  If you are unable to select the desired planar face, you can change the selection behavior by clicking the selection options tool in the prompt area. For more information, see “Using the selection options,” Section 6.3.

The selected face is highlighted in the viewport.

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 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 Flip 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, choose one of the following:

Select 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.

Select 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.

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.

ABAQUS/CAE creates the extruded solid feature.