Beam elements in ABAQUS make me a little confused, especially about the shear stiffness and elements for open sections. In this post, I want to make a summary of the elements in ABAQUS and give an example about the settings of beam elements.

Beam element library

Beam elements in a plane only have active degrees of freedom 1, 2, 6. Beam elements in space have active degrees of freedom 1, 2, 3, 4, 5, 6. Open section beams in space B31OS, B31OSH, B32OS, B32OSH have active degrees of freedom 1, 2, 3, 4, 5, 6, 7. The beam elements in ABAQUS Standard and Explicit (v6.14) are summarized below.

Beam elements in ABAQUS Standard

Beam elements in ABAQUS Explicit

The Abaqus beam cross-section library contains solid sections (circular, rectangular, and trapezoidal), closed thin-walled sections (box, hexagonal, and pipe), open thin-walled sections (I-shaped, T-shaped, or L-shaped), and a thick-walled pipe section. Abaqus also provides an arbitrary thin-walled section definition; Abaqus will treat this section type as a closed or open section, depending on how the section is defined.

Trapezoidal, I, and arbitrary library sections allow you to define the location of the origin of the local coordinate system. Other section types—such as rectangular, circular, L, or pipe—have preset origins.

Generalized cross section

You can specify “generalized” cross-sections by specifying the geometric quantities necessary to define the section. Such generalized sections can be used only with linear material behavior although the section response can be linear or nonlinear. Nonlinear generalized cross-sections are not supported in ABAQUS/CAE.

*Beam General Section, section=GENERAL
*Beam General Section, section=NONLINEAR GENERAL

A general beam section:

• is used to define beam section properties that are computed once and held constant for the entire analysis;
• can be used to define linear or nonlinear section behavior;
• for linear section behavior can be associated only with linear material behavior
• enables the use of meshed cross-sections (“Meshed beam cross-sections,” Section 10.6.1);
• enables the use of tapered cross-sections (Abaqus/Standard only).

In ABAQUS/CAE, you can define a beam section with generalized shape shown as below. The section geometry properties can be defined in this dialog window. The location of the centroid and shear center, the output points as well as the transverse shear stiffness are allowed to define directly as figured below. The keywords generated in input file are listed below.

** Section: pipe Profile: Profile-2

*Beam General Section, elset=_PickedSet2, poisson = 0.2, section=GENERAL
0.00531, 2.96e-05, 0., 2.96e-05, 5.92e-05
0.,0.,-1.
2e+08, 7.69231e+07

*Shear Center
0.002, 0.001

*Centroid
0.002, 0.001

*Section Points
0.002, 0.001, 0.001, 0.

*Transverse Shear
6.9591e+06, 6.9591e+06, 0.2

The Section Poisson value must be between -1.0 and 0.5 with a default value set to 0.0 so that this effect is ignored. This value is only valid for the shear flexible elements providing for a possible uniform cross-sectional area change. This effect is considered only in geometrically nonlinear analysis (see “Defining an analysis,” Section 6.1.2) and is provided to model the reduction or increase in the cross-sectional area for a beam subjected to large axial stretch. 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 rubber or if it 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. Why the cross section area increases under tensile axial strain?

If you want to get the stress and strain on integration points, you have to define the output points in “Edit Beam Section”. To locate points in the section at which output of axial strain (and, for linear section behavior, axial stress) is required, specify the local \(\left( {{x_1},{x_2}} \right)\) coordinates of the point in the cross-section: Abaqus numbers the points 1, 2, … in the order that they are given.

The variation of \(\varepsilon \) over the section is given by

where \(\left( {{x_{1c}},{x_{2c}}} \right)\) are the local coordinates of the centroid of the beam section and \({\kappa _1}\) and \({\kappa _2}\) are the changes of curvature for the section.

Meshed cross section

The response of some structures is beam-like, yet the beam cross-section geometry or multi-material makeup of the cross-section do not permit the use of a predefined library beam cross-section. In these cases a meshed cross-section can be used to model the beam cross-section and to generate beam cross-section properties appropriate for subsequent use in a Timoshenko beam analysis. The beam properties are generated assuming a thick-walled (solid) cross-section with unconstrained out-of-plane warping, so open-section beam elements cannot use the beam cross-section properties generated from the meshed section. The generated beam cross-section properties include axial, bending, torsional, and transverse shear stiffnesses; mass, rotary inertia, and damping properties; and the centroid and shear center of the cross-section. In addition, the equivalent beam cross-section properties include information on stress recovery, such as the warping function and its derivatives.

Meshed cross-sections:

• allow for the description of a beam cross-section including multiple materials and complex geometry;
• are meshed in Abaqus/Standard with two-dimensional warping elements, which have an out-of-plane warping displacement as the only degree of freedom;
• generate beam cross-section properties that can be used in a subsequent beam element analysis in either Abaqus/Standard or Abaqus/Explicit;
• allow only isotropic linear elastic material behavior or orthotropic linear elastic material behavior for warping elements;
• allow stress and strain postprocessing on the beam element model or the two-dimensional warping element model.

The procedure for analyzing and postprocessing a beam analysis using a meshed cross-section is as follows:

The cross-section is meshed using special-purpose two-dimensional elements: WARP2D3 (3-node triangular) and WARP2D4 (4-node quadrilateral). These elements have one degree of freedom per node representing the value of the out-of-plane warping function and use a solid section definition. The way to generate and use the generated cross section properties is detailed in Abaqus Analysis User’s Guide.

Keywords edition

The keywords in input files for general section and meshed cross section can be referred to Abaqus Keywords Reference Guide and summarized here.

*Beam General Section, elset=elset_name, section=GENERAL
A, \({I_{11}}\), \({I_{12}}\), \({I_{22}}\), J, \({\Gamma _0}\), \({\Gamma _W}\)
0, 0, -1 (optional)
E, G

*Beam General Section, elset=elset_name, section=NONLINEAR GENERAL
A, \({I_{11}}\), \({I_{12}}\), \({I_{22}}\), J, \({\Gamma _0}\), \({\Gamma _W}\)
0, 0, -1 (optional)
E, G
The axial and bending behaviors of the section are defined by using the *AXIAL, *M1, *M2, *TORQUE, and *THERMAL EXPANSION options.

*Beam General Section, elset=elset_name, section=MESHED
0, 0, -1
(EA), \({\left( {EI} \right)_{11}}\), \({\left( {EI} \right)_{12}}\), \({\left( {EI} \right)_{22}}\), (GJ)
\(\rho A\), \({\left( {\rho I} \right)_{11}}\), \({\left( {\rho I} \right)_{12}}\), \({\left( {\rho I} \right)_{22}}\), \({x_{1cm}}\), \({x_{2cm}}\)

Notes: (1) Sectorial moment \({\Gamma _0}\) and warping constant \({\Gamma _W}\) are only needed in ABAQUS/Standard when the section is associated with open=section beam elements. (2) (0, 0, -1) are the default values for beam orientation if the first beam section axis is not defined by an additional node in the element’s connectivity. (3) If the TAPER parameter is included, two lines of properties of node A and node B are required. (4) \({x_{1cm}}\) and \({x_{2cm}}\) are the local 1-coordinate and 2-coordinate of the center of mass.

Example of different section settings

A steel frame with pipe section is analyzed with different section settings with beam element B31. Displacement control method with a maximum vertical displacement 1m at the vertex of the frame is adopted. The pipe section has a diameter of 219.1mm and thickness of 8mm. The material possesses density of 77 and elastic module of 200GPa and the poison ratio of 0.3.

The transverse shear stiffness are specified. The keywords in input file are listed below.

*Beam Section, elset=_PickedSet2, material=pipe, section=THICK PIPE
0.10955, 0.008
0.,0.,-1.
*Transverse Shear
204059, 204059,

*Beam General Section, elset=_PickedSet2, section=GENERAL
0.00531, 2.96e-05, 0., 2.96e-05, 5.92e-05
0.,0.,-1.
2e+08, 7.69231e+07
*Transverse Shear
204059, 204059,

*Beam General Section, elset=_PickedSet2,section=MESHED
0.,0.,-1.
1.06E+06,5.92E+03,0.00E+00,5.92E+03,4.55E+03
8.18E+07 ,4.56E+05,0.00E+00,4.56E+05,0,0

*Transverse Shear
204059,204059,0

*Beam General Section, elset=_PickedSet2, section=PIPE
0.10955, 0.008
0.,0.,-1.
2e+08, 7.69231e+07

*Transverse Shear
204059, 204059,

The force-displacement curves of the vertex are illustrated in the following figure and accord well with each other.

Notes:

• The choice of section integration for generalized section beam can only be “Before analysis”.
• only thin-walled pipe section can be used in general section with keywords in input file.