Specifying properties for general beam sections

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. For more information on naming objects, see Using basic dialog box components.
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.
From the Beam shape along length options, do one of the following:
- To maintain the same cross-sectional profile along the entire length of the beam, select Constant and select a beam profile from the Beam Shape options. If desired, click to create a profile; see Creating profiles, for more information.
- To define different cross-sectional profiles at each end of the beam, select Tapered and select starting and ending profiles from the Beam Start and Beam End options, respectively. If desired, click to create a profile; see Creating profiles, for more information. The starting and ending profiles must be the same shape.
  
  Tapered beams are supported for Abaqus/Standard analyses only. Abaqus/CAE scales beam profiles linearly between the starting and ending profiles.
If you selected a generalized profile, you can offset the beam section from its node by specifying how far and in which direction along the cross-section axes to move the section centroid and/or shear center. Enter the local $x_{1}$ - and $x_{2}$ -coordinates for the Centroid and/or the Shear Center as desired.
On the Basic tabbed page:
1. To define the section thermal expansion coefficient, toggle on Use thermal expansion data.
  A column labeled Thermal Expansion appears in the data table.
2. To define section data that depend on temperature, toggle on Use temperature-dependent data.
  A column labeled Temperature appears in the data table.
3. 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.
4. Enter values for the section Young's Modulus and torsional Shear Modulus in the data table.
5. 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.
6. To define a density for the beam section, toggle on Specify section material density and enter a value in the field provided. 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.
7. If the thermal expansion coefficient is temperature dependent, toggle on Specify reference temperature and enter a value for the thermal expansion in the field provided.
On the Damping tabbed page, specify damping properties to include mass and stiffness proportional damping in the dynamic response of the section:
1. Enter a value in the Alpha field for the $α_{R}$ factor to create mass proportional damping in direct-integration dynamics. This value is ignored in modal dynamics.
2. Enter a value in the Beta field for the $β_{R}$ factor to create stiffness proportional damping in direct-integration dynamics. This value is ignored in modal dynamics.
3. 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.
On the Stiffness tabbed page, do the following:
1. Select Use consistent mass matrix formulation to let Abaqus calculate the mass formulation for the beam section using the McCalley-Archer consistent mass matrix based on the cubic interpolation of deflections and quadratic interpolation of rotations. If you toggle off this option, Abaqus performs this calculation using a lumped mass formulation.
2. Toggle on Specify transverse shear to include nondefault transverse shear stiffness effects in the section definition and specify the Slenderness compensation:
  - Select Use analysis product default to let Abaqus calculate the shear stiffness and the slenderness compensation factor from the elastic material definition for the beam section.
  - Select Value to specify the transverse shear stiffness effects directly.
    - Enter a slenderness compensation factor in the field provided.
    - Enter values for the $K_{23}$ and $K_{13}$ shear stiffnesses of the section in the fields provided.
On the Fluid Inertia tabbed page, toggle on Specify fluid inertia effects to simulate the inertial effects of the beam being submerged in a fluid. For details, see Additional inertia due to immersion in fluid.
1. Specify whether the beam is Fully submerged or Half submerged in the fluid. If you select Half submerged, the added inertia per unit length is reduced by a factor of one-half.
2. Specify the Fluid density.
3. Enter the effective radius of the wetted cross-section in the Section radius field.
4. Specify $C_{A}$ , the added mass coefficient for Lateral motions of the beam.
5. Specify $C_{A - E}$ , the added mass coefficient for Motions along beam axis.
6. If the beam cross-section origin is different than the centroid of the wetted cross-section, specify the centroid's X and Y coordinates relative to the cross-section origin.
On the Output Points tabbed page, you can locate points in the beam section for which stress and strain output are required. Enter the local $x_{1}$ - and $x_{2}$ -positions of as many section points as needed.
Click OK to save your changes and to close the beam section editor.