Products: ABAQUS/Standard ABAQUS/Explicit ABAQUS/CAE
A beam section integrated during the analysis:
is used when section properties must be recomputed as the beam deforms over the course of the analysis; and
can be associated with linear or nonlinear material behavior.
Use a beam section integrated during the analysis to define the section behavior when numerical integration over the section is required as the beam deforms. You can choose a section shape from the library of beam section shapes provided (see “Beam cross-section library,” Section 15.3.9) and define the section's dimensions. In addition, you can specify the number of section points to use for integration. The default number of section points is adequate for monotonic loading that causes plasticity. If reversed plasticity will occur, more section points are required.
Use a material definition (“Material data definition,” Section 9.1.2) to define the material properties of the section, and associate these properties with the section definition. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, the more economic approach is to use a general beam section (see “Using a general beam section to define the section behavior,” Section 15.3.7).
You must associate the section properties with a region of your model.
| Input File Usage: | *BEAM SECTION, ELSET=name, SECTION=library_section, MATERIAL=name |
| The ELSET parameter is used to associate the section properties with a set of beam elements. |
| ABAQUS/CAE Usage: | Property module:
Create Profile: Name: library_section
Create Section: select Beam as the section Category and Beam as the section |
In the shear flexible elements ABAQUS provides for a possible uniform cross-sectional area change by allowing you to specify an effective Poisson's ratio for the section. This effect is considered only in geometrically nonlinear analysis (see “Procedures: overview,” Section 6.1.1) and is provided to model the reduction or increase in the cross-sectional area for a beam subjected to large axial stretch.
The value of the effective Poisson's ratio must be between –1.0 and 0.5. By default, this effective Poisson's ratio for the section is set to 0.0 so that this effect is ignored. Setting the effective Poisson's ratio to 0.5 implies that the overall response of the section is incompressible. This behavior is appropriate if the beam is made of a typical metal whose overall response at large deformation is essentially incompressible (because it is dominated by plasticity). Values between 0.0 and 0.5 mean that the cross-sectional area changes proportionally between no change and incompressibility, respectively. A negative value of the effective Poisson's ratio will result in an increase in the cross-sectional area in response to tensile axial strains.
This effective Poisson's ratio is not available for use with Euler-Bernoulli beam elements.
| Input File Usage: | *BEAM SECTION, POISSON= |
| ABAQUS/CAE Usage: | Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Section Poisson's ratio: |
When a beam section integrated during the analysis is used, damping can be introduced through the material behavior definition. See “Material damping,” Section 12.1.1, for more information about the material damping types available in ABAQUS.
Temperature and field variables can be specified at specific points through the section or by defining the value at the origin of the cross-section and specifying the gradients in the local 1- and 2-directions. The actual values of the temperature and field variables are specified as either predefined fields or initial conditions (see “Predefined fields,” Section 19.6.1, or “Initial conditions,” Section 19.2.1).
In any element it is assumed that the temperature definitions at all the nodes of the element are compatible with the temperature definition method chosen for the element. For cases in which the temperature definition method changes from one element to the next, separate nodes must be used on the interface between elements with different temperature definition methods and MPCs must be applied to make the displacements and rotations the same at the nodes.
Temperatures and field variables can be defined by giving the value at the origin of the cross-section and the gradients in the 2- and 1-directions of the cross-section (that is, give 
and 
in the predefined field or initial condition definition). For beams in a plane only 
and 
need be given; gradients in the 1-direction are ignored in this case.
| Input File Usage: | *BEAM SECTION, TEMPERATURE=GRADIENTS |
| ABAQUS/CAE Usage: | Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Linear by gradients |
Temperatures and field variables can be defined at a set of points on the section, as indicated for each cross-section in “Beam cross-section library,” Section 15.3.9.
| Input File Usage: | *BEAM SECTION, TEMPERATURE=VALUES |
| ABAQUS/CAE Usage: | Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: During analysis, Interpolated from temperature points |
Beam section properties such as cross-sectional area, moments of inertia, etc. are printed in the model data output. When a beam section integrated during the analysis is used, section forces, moments, and transverse shear forces and section strains, curvatures, and transverse shear strains can be output for the section (see “Element output” in “Output to the data and results files,” Section 4.1.2, and “Element output” in “Output to the output database,” Section 4.1.3). In addition, stress and strain can be output at each section point. “Beam element library,” Section 15.3.8, lists some of the element output quantities that are available for beam elements.
Axial strains due to warping are included in the stress/strain output from ABAQUS/Standard if a beam section integrated during the analysis is used.
Temperature output at the section points can be obtained using the element variable TEMP. If the temperatures are given at specific points through the section, output at the temperature points can be obtained using the nodal variable NTxx. The nodal variable NTxx should not be used for output at the temperature points if the temperatures are specified by defining the value at the origin of the cross-section and specifying the gradients in the local 1- and 2-directions. In this case output variable NT should be requested; NT11 (the reference temperature value) and NT12 and NT13 (the temperature gradients in the local 1- and 2-directions, respectively) will be output automatically.
Section: select regions