A stringer reinforcement defines a stringer that is bonded to the edge of an existing part and specifies its engineering properties. You can select an edge of a three-dimensional solid part or an edge of a two-dimensional planar part. The part can be an Abaqus native part, or it can be an orphan mesh part. You should think of a stringer as a property of a part or region, in the same way a section is a property of a part or region.

The steel-reinforced beam shown in Figure 33–2 is an example of how you might use stringer reinforcements in your model.

The beam has a concrete core with four cylindrical extrusions that run the length of the beam. A steel stringer with a circular profile has been created in each extrusion to provide support along the length of the beam. You can create a solid part representing the beam and add four stringer reinforcements representing the steel reinforcements. In the Mesh module you assign solid elements to the concrete and line elements to the stringers. The solid and line elements share the same nodes.

Select SpecialStringerCreate from the main menu bar in the Property module to define one or more stringers. Select Edit from the same menu to make changes to an existing definition. All stringers you create also appear in the Model Tree in a Stringers container under the part. Different stringers can share the same section, and multiple stringers can be placed on an edge of a part. Stringers are not displayed in the viewport by default, but you can make them visible by color coding them in the viewport. See “Coloring geometry and mesh elements,” Section 73.4, for more information.

If you create a stringer on an Abaqus native part, Abaqus/CAE updates the stringer if you make minor modifications to the underlying part. If you edit an orphan mesh part with a stringer, Abaqus/CAE updates the stringer if you edit or delete nodes or elements; however, it does not update the stringer if you create new nodes or elements.

You may need to select the stringer in subsequent modeling operations; for example, to:

• Assign a section, beam section orientation, material orientation, or tangent direction to a stringer. All of these activities are performed in the Property module.

• Prescribe a body force or line load to the stringer in the Load module.

• Prescribe a thermal flux on the stringer in the Load module. In practice, you perform this modeling operation by applying a thermal flux load to the underlying edge or edges. Abaqus/CAE applies the load to all stringers on that edge during the analysis.

• Assign an element type to the stringer in the Mesh module.

• Request field data output or history data output for the stringer in the Step module.

• Create a display group to view the stress values on the stringer elements in the Visualization module. While you cannot specifically select stringers by name in the Create Display Group dialog box, you can find them in this dialog box by searching for elements that share the same element type, section assignment, or another property as the stringer elements in your model. This process can help you narrow down the list of elements to the stringers you want to include.

When you are prompted to select a region for these modeling operations, select Stringers from the list of object types in the Selection toolbar, and select the stringer from the viewport. For more information, see “Filtering your selection based on the type of object,” Section 6.3.2.

Abaqus/CAE does not consider an edge's stringer reinforcements when it performs contact calculations. If your model includes interactions between edges that have stringer reinforcements, this approach can affect your results if the thickness of the stringers is significant.

For detailed information on creating a stringer, see “Creating and editing stringer reinforcements,” Section 33.9.