Beam section behavior is defined in terms of the response of the beam section to stretching, bending, shear, and torsion. For more information, see “Beam section behavior,” Section 23.3.5 of the ABAQUS Analysis User's Manual.
When you create beam sections, you must choose a section integration method. You can choose to provide the section property data before the analysis (a general beam section) or to have ABAQUS calculate (integrate) the cross-sectional behavior from section integration points during the analysis. The following sections describe how to define a beam section for each integration method:
In general beam sections the cross-section properties are calculated only once, during preprocessing. All section computations during the analysis are performed in terms of the precomputed values. No material definition is needed for a general beam section. Use this type of beam section when the response of the beam is linear or when it is nonlinear and the nonlinearity arises from more than just material nonlinearity, such as in cases when section collapse occurs. For more information, see “Using a general beam section to define the section behavior,” Section 23.3.7 of the ABAQUS Analysis User's Manual.
To specify properties for general beam sections:
From the main menu bar, select Section
Create.
A Create Section dialog box appears.
Tip:
You can also click Create in the Section Manager or select the create section tool 
in the Property module toolbox.
Enter a section name of your choice. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select Beam as the section Category and Beam as the section Type, and click Continue.
The beam section editor appears.
Select Before analysis as the Section integration method.
Select a profile for the beam section. If desired, click Create to create a profile; see “Creating profiles,” Section 12.11.14, for more information.
The Profile shape field is updated to reflect your choice.
On the Basic tabbed page:
To define the section thermal expansion coefficient, toggle on Use thermal expansion data.
A column labeled Thermal Expansion appears in the data table.
To define section data that depend on temperature, toggle on Use temperature-dependent data.
A column labeled Temperature appears in the data table.
To define section data that depend on field variables, click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables.
Field variable columns appear in the data table.
Enter values for the section Young's Modulus and torsional Shear Modulus in the data table.
Enter a value for the Section Poisson's ratio to provide uniform strain in the section due to strain of the beam axis (so that the cross-sectional area changes when the beam is stretched). This value must be between –1.0 and 0.5. A value of 0.5 will enforce incompressible behavior. The default value is 0.
Enter a value for the Section material density. This value is required in an ABAQUS/Explicit analysis. In an ABAQUS/Standard analysis it is needed only when the mass is required, such as in dynamic analysis or gravity loading.
If the thermal expansion coefficient is temperature dependent, enter a value for the Reference temperature for thermal expansion.
On the Advanced tabbed page:
Specify Damping properties to include mass and stiffness proportional damping in the dynamic response of the section:
Enter a value in the Alpha field for the 
factor to create mass proportional damping in direct-integration dynamics. This value is ignored in modal dynamics.
Enter a value in the Beta field for the 
factor to create stiffness proportional damping in direct-integration dynamics. This value is ignored in modal dynamics.
Enter a value in the Composite field for the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics). This value is applicable only to ABAQUS/Standard analysis and is ignored in direct-integration dynamics.
For most beam sections ABAQUS will calculate the transverse shear stiffness values required. If desired, toggle on Specify transverse shear to include nondefault transverse shear stiffness effects in the section definition, and enter values for the 
and 
shear stiffnesses of the section and the slenderness compensation factor.
To offset a general beam section from its node, you must specify how far and in which direction along the cross-section axes to move the section centroid and/or shear center. Enter the local 
- and 
-coordinates for the Centroid and/or the Shear Center as desired.
To locate points in the beam section for which stress and strain output are required, on the Output Points tabbed page specify the local 
- and 
-positions of as many section points as needed.
Click OK to save your changes and to close the beam section editor.
Beam sections integrated during analysis allow the cross-sectional behavior to be calculated by numerical integration of the stress over the cross-section to define the beam's response as the analysis proceeds. The material behavior is evaluated independently at each point on the section. This type of beam section should be used when the section nonlinearity is caused only be nonlinear material response. For more information, see “Using a beam section integrated during the analysis to define the section behavior,” Section 23.3.6 of the ABAQUS Analysis User's Manual.
To specify properties for beam sections integrated during analysis:
From the main menu bar, select SectionCreate.
A Create Section dialog box appears.
Tip:
You can also click Create in the Section Manager or select the create section tool in the Property module toolbox.
Enter a section name of your choice. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select Beam as the section Category and Beam as the section Type, and click Continue.
The beam section editor appears.
Choose During analysis as the Section integration method.
Select a profile for the beam section. If desired, click Create to create a profile; see “Creating profiles,” Section 12.11.14, for more information.
The Profile shape field is updated to reflect your choice.
Select a Material name to be used with this beam section definition.
Enter a value for the Section Poisson's ratio to provide uniform strain in the section due to strain of the beam axis (so that the cross-sectional area changes when the beam is stretched). This value must be between –1.0 and 0.5. A value of 0.5 will enforce incompressible behavior.
Select a method for defining the Temperature variation through the section:
Choose Linear by gradients to indicate that the temperature at the cross-section origin and the temperature gradient or gradients through the section are specified. You can use the Load module to specify these temperatures.
Choose Interpolated from temperature points to indicate that the shape of the beam section profile determines the number and location of the temperature points. (For more information on temperature points, see “Beam cross-section library,” Section 23.3.9 of the ABAQUS Analysis User's Manual.) You can use the Load module to specify the temperature at each of these points.
For most beam sections ABAQUS will calculate the transverse shear stiffness values required. If desired, toggle on Specify transverse shear to include nondefault transverse shear stiffness effects in the section definition, and enter values for the and shear stiffnesses of the section and the slenderness compensation factor.
Click OK to save your changes and to close the beam section editor.