<!-- source-page: 331 -->

allowed. The elastic modulus is defined by the slope of the initial line segment, so that straining beyond the point that terminates that initial line segment will be partially inelastic. If strain reversal occurs in that part of the response, it will be elastic initially. See Figure 29.3.7–2 for an example.

Input File Usage: Use the following options to define elastic-plastic axial, bending, and torsional behavior:

\*AXIAL   
\*M1   
\*M2   
\*TORQUE

Abaqus/CAE Usage: Nonlinear generalized cross-sections are not supported in Abaqus/CAE.

![](images/page-331_d0d02cfdc97e987e4f5424e0cd5a2cbd282ac20e49bead94ed07e54b0e8b095c.jpg)

<details>
<summary>line</summary>

| Curvature, K | Bending moment, M |
| ------------ | ----------------- |
| 0            | 0                 |
| 1            | 1                 |
| 2            | 2                 |
| 3            | 3                 |
| 4            | 4                 |
| 5            | 5                 |
| 6            | 6                 |
| 7            | 7                 |
| 8            | 8                 |
| 9            | 9                 |
| 10           | 10                |
</details>

Figure 29.3.7–2 Example of inelastic nonlinear beam section behavior definition.

# Defining the reference temperature for thermal expansion

The thermal expansion coefficient may be temperature dependent. In this case the reference temperature for thermal expansion, $\theta ^ { 0 }$ , must be defined.

Input File Usage: \*BEAM GENERAL SECTION, ZERO=

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis:

Basic: Specify reference temperature: $\theta ^ { 0 }$

<!-- source-page: 332 -->

# Defining the initial section forces and moments

You can define initial stresses (see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) for general beam sections that will be applied as initial section forces and moments. Initial conditions can be specified only for the axial force, the bending moments, and the twisting moment. Initial conditions cannot be prescribed for the transverse shear forces.

# Defining a change in cross-sectional area due to straining

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 “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.

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 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.

This effective Poisson’s ratio is not available for use with Euler-Bernoulli beam elements.

Input File Usage: \*BEAM GENERAL SECTION, POISSON=

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section

Category and Beam as the section Type: Section integration: Before

analysis: Basic: Section Poisson's ratio: $\nu _ { \mathrm { e f f } }$

# Defining damping

When the beam section and material behavior are defined by a general beam section, you can include mass and viscous stiffness proportional damping in the dynamic response (calculated in Abaqus/Standard with the direct time integration procedure, “Implicit dynamic analysis using direct integration,” Section 6.3.2).

See “Material damping,” Section 26.1.1, for more information about the material damping types available in Abaqus.

Input File Usage: Use both of the following options:

\*BEAM GENERAL SECTION

\*DAMPING

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category

and Beam as the section Type: Section integration: Before analysis:

Damping: Alpha, Beta, Structural, and Composite

<!-- source-page: 333 -->

# Specifying temperature and field variables

Define temperatures and field variables by giving the values at the origin of the cross-section as either predefined fields or initial conditions (see “Predefined fields,” Section 34.6.1, or “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Temperature gradients can be specified in the local 1- and 2-directions; other field-variable gradients defined through the cross-section will be ignored in the response of beam elements that use a general beam section definition.

# Output

Only the section forces, moments, and transverse shear forces and section strains, curvatures, and transverse shear strains can be output (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).

You can output stress and strain at particular points in the section. For linear section behavior defined using a standard library section or a generalized section, only axial stress and axial strain values are available. For linear section behavior defined using a meshed section, axial and shear stress and strain are available. For nonlinear generalized section behavior, axial strain output only is provided.

# Specifying the output section points for standard library sections and generalized sections

To locate points in the section at which output of axial strain (and, for linear section behavior, axial stress) is required, specify the local $( x _ { 1 } , x _ { 2 } )$ coordinates of the point in the cross-section: Abaqus numbers the points 1, $2 , \ldots$ in the order that they are given.

The variation of over the section is given by

$$
\varepsilon = \varepsilon_ {c} + \kappa_ {1} (x _ {2} - x _ {2 c}) - \kappa_ {2} (x _ {1} - x _ {1 c}),
$$

where $( x _ { 1 c } , x _ { 2 c } )$ 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.

For open-section beam element types, the variation of over the section has an additional term of the form $\psi ( x _ { 1 } , x _ { 2 } ) \chi _ { \mathrm { { ; } } }$ , where $\psi ( x _ { 1 } , x _ { 2 } )$ is the warping function. The warping function itself is undefined in the general beam section definition. Therefore, Abaqus will not take into account the axial strain due to warping when calculating section points output. Axial strains due to warping are included in the stress/strain output if a beam section integrated during the analysis is used.

Abaqus uses St. Venant torsion theory for noncircular solid sections. The torsion function and its derivatives are necessary to calculate shear stresses in the plane of the cross-section. The function and its derivatives are not stored for a general beam section. Therefore, you can request output of axial components of stress/strain only. A beam section integrated during the analysis must be used to obtain output of shear stresses.

Input File Usage: Use both of the following options to specify the output section points for general beam sections:

\*BEAM GENERAL SECTION

\*SECTION POINTS

, , ...

<!-- source-page: 334 -->

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Beam as the section Type: Section integration: Before analysis: Output Points: x1, x2, ...

Requesting output of maximum axial stress/strain in Abaqus/Standard

If you specify the output section points to obtain the maximum axial stress/strain (MAXSS) for a linear generalized section, the output value will be the maximum of the values at the user-specified section points. You must select enough section points to ensure that this is the true maximum. MAXSS output is not available for nonlinear generalized sections or for an Abaqus/Explicit analysis.

# Specifying the output section points for meshed cross-sections

For meshed cross-sections you can indicate in the two-dimensional cross-section analysis the elements and integration points where the stress and strain will be calculated during the subsequent beam analysis. Abaqus will then add the section points specification to the resulting jobname.bsp text file. This text file is then included as the data for the general beam section definition in the subsequent beam analysis. See “Meshed beam cross-sections,” Section 10.6.1, for details.

The variation of the axial strain over the meshed section is given by

$$
\varepsilon = \varepsilon_ {c} + \kappa_ {1} (x _ {2} - x _ {2 c}) - \kappa_ {2} (x _ {1} - x _ {1 c}),
$$

where $\left( { x _ { 1 c } , x _ { 2 c } } \right)$ 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.

The variations of shear components $\gamma _ { 1 }$ and $\gamma _ { 2 }$ over the meshed section are given by

$$
\gamma_ {1} = \gamma_ {s 1} + \phi \bigg (\frac {\partial \Psi}{\partial x _ {1}} - (x _ {2} - x _ {2 s}) \bigg),
$$

$$
\gamma_ {2} = \gamma_ {s 2} + \phi \left(\frac {\partial \Psi}{\partial x _ {2}} + \left(x _ {1} - x _ {1 s}\right)\right),
$$

where $\left( \boldsymbol { x } _ { 1 s } , \boldsymbol { x } _ { 2 s } \right)$ are the local coordinates of the shear center of the beam section, $\phi$ is the twist of the beam axis, $\Psi ( x _ { 1 } , x _ { 2 } )$ is the warping function, and $\gamma _ { s 1 }$ and $\gamma _ { s 2 }$ are shear strains due to the transverse shear forces.

For the case of an orthotropic composite beam material, the axial stress $\sigma$ and the two shear components $\tau _ { 1 }$ and $\tau _ { 2 }$ are calculated in the beam section (1, 2) axis as follows:

$$
\left\{ \begin{array}{c} \sigma \\ \tau_ {1} \\ \tau_ {2} \end{array} \right\} = \left[ \begin{array}{c c c} E & 0 & 0 \\ & G _ {1} (\cos \alpha) ^ {2} + G _ {2} (\sin \alpha) ^ {2} & (G _ {1} - G _ {2}) \cos \alpha \sin \alpha \\ & s y m & G _ {1} (\sin \alpha) ^ {2} + G _ {2} (\cos \alpha) ^ {2} \end{array} \right] \left\{ \begin{array}{c} \varepsilon \\ \gamma_ {1} \\ \gamma_ {2} \end{array} \right\},
$$

where determines the material orientation.

<!-- source-page: 335 -->

<table><tr><td>Input File Usage:</td><td>Use both of the following options in the two-dimensional meshed cross-section analysis to specify the output section points for the subsequent beam analysis:*BEAM SECTION GENERATE*SECTION POINTSsection_point_label, element_number, integration_point_number</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Meshed cross-sections are not supported in Abaqus/CAE.</td></tr></table>

<!-- source-page: 336 -->

<!-- source-page: 337 -->

# 29.3.8 BEAM ELEMENT LIBRARY

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Beam modeling: overview,” Section 29.3.1   
• “Choosing a beam element,” Section 29.3.3   
• \*BEAM GENERAL SECTION   
• \*BEAM SECTION

# Overview

This section provides a reference to the beam elements available in Abaqus/Standard and Abaqus/Explicit.

# Element types

Beams in a plane 

<table><tr><td>B21</td><td>2-node linear beam</td></tr><tr><td> $B21H^{(S)}$ </td><td>2-node linear beam, hybrid formulation</td></tr><tr><td>B22</td><td>3-node quadratic beam</td></tr><tr><td> $B22H^{(S)}$ </td><td>3-node quadratic beam, hybrid formulation</td></tr><tr><td> $B23^{(S)}$ </td><td>2-node cubic beam</td></tr><tr><td> $B23H^{(S)}$ </td><td>2-node cubic beam, hybrid formulation</td></tr><tr><td>PIPE21</td><td>2-node linear pipe</td></tr><tr><td> $PIPE21H^{(S)}$ </td><td>2-node linear pipe, hybrid formulation</td></tr><tr><td> $PIPE22^{(S)}$ </td><td>3-node quadratic pipe</td></tr><tr><td> $PIPE22H^{(S)}$ </td><td>3-node quadratic pipe, hybrid formulation</td></tr></table>

Active degrees of freedom

1, 2, 6

Additional solution variables

All of the cubic beam elements have two additional variables relating to axial strain.

The linear thin-walled pipe elements have one additional variable, and the quadratic thin-walled pipe elements have two additional variables relating to the hoop strain. The linear thick-walled pipe elements

<!-- source-page: 338 -->

have two additional variables, and the quadratic thick-walled pipe elements have four additional variables relating to the hoop and radial strain components.

The hybrid beam and pipe elements have additional variables relating to the axial force and transverse shear force. The linear elements have two, the quadratic elements have four, and the cubic elements have three additional variables.

Beams in space 

<table><tr><td>B31</td><td>2-node linear beam</td></tr><tr><td>B31H(S)</td><td>2-node linear beam, hybrid formulation</td></tr><tr><td>B32</td><td>3-node quadratic beam</td></tr><tr><td>B32H(S)</td><td>3-node quadratic beam, hybrid formulation</td></tr><tr><td>B33(S)</td><td>2-node cubic beam</td></tr><tr><td>B33H(S)</td><td>2-node cubic beam, hybrid formulation</td></tr><tr><td>PIPE31</td><td>2-node linear pipe</td></tr><tr><td>PIPE31H(S)</td><td>2-node linear pipe, hybrid formulation</td></tr><tr><td>PIPE32(S)</td><td>3-node quadratic pipe</td></tr><tr><td>PIPE32H(S)</td><td>3-node quadratic pipe, hybrid formulation</td></tr></table>

Active degrees of freedom

1, 2, 3, 4, 5, 6

# Additional solution variables

All of the cubic beam elements have two additional variables relating to axial strain.

The linear thin-walled pipe elements have one additional variable, and the quadratic thin-walled pipe elements have two additional variables relating to the hoop strain. The linear thick-walled pipe elements have two additional variables, and the quadratic thick-walled pipe elements have four additional variables relating to the hoop and radial strain components.

The hybrid beam and pipe elements have additional variables relating to the axial force and transverse shear force in the linear and quadratic elements and to the axial force only in the cubic elements. The linear and cubic elements have three and the quadratic elements have six additional variables.

Open-section beams in space 

<table><tr><td>B31OS(S)</td><td>2-node linear beam</td></tr><tr><td>B31OSH(S)</td><td>2-node linear beam, hybrid formulation</td></tr><tr><td>B32OS(S)</td><td>3-node quadratic beam</td></tr><tr><td>B32OSH(S)</td><td>3-node quadratic beam, hybrid formulation</td></tr></table>

<!-- source-page: 339 -->

# Active degrees of freedom

1, 2, 3, 4, 5, 6, 7

# Additional solution variables

Element type B31OSH has three additional variables and element type B32OSH has six additional variables relating to the axial force and transverse shear force.

# Nodal coordinates required

Beams in a plane: X, Y, also (optional) $N _ { x } , N _ { y }$ , the direction cosines of the normal.

Beams in space: X, Y, Z, also (optional) $N _ { x } , N _ { y } , N _ { z }$ , the direction cosines of the second local crosssection axis.

# Element property definition

For PIPE elements use the pipe section type to specify the thin-walled pipe formulation or the thick pipe section type to specify the thick-walled pipe formulation. No other section types can be used with PIPE elements.

For open-section elements use only the arbitrary, I, L, and linear generalized section types.

Local orientations defined as described in “Orientations,” Section 2.2.5, cannot be used with beam elements to define local material directions. The orientation of the local beam section axes in space is discussed in “Beam element cross-section orientation,” Section 29.3.4.

Input File Usage: Use either of the following options:

\*BEAM SECTION

\*BEAM GENERAL SECTION

Abaqus/CAE Usage: Property module: Create Section: select Beam as the section Category and Beam as the section Type

# Element-based loading

# Distributed loads

Distributed loads are specified as described in “Distributed loads,” Section 34.4.3.

<table><tr><td>Load ID(*DLOAD)</td><td>Abaqus/CAELoad/Interaction</td><td>Units</td><td>Description</td></tr><tr><td> $CENT^{(S)}$ </td><td>Not supported</td><td> $FL^{-2}$  $(ML^{-1}T^{-2})$ </td><td>Centrifugal force (magnitude is input as  $m\omega^{2}$ , where  $m$  is the mass per unit length and  $\omega$  is the angular velocity).</td></tr></table>

<!-- source-page: 340 -->

<table><tr><td>Load ID (*DLOAD)</td><td>Abaqus/CAE Load/Interaction</td><td>Units</td><td>Description</td></tr><tr><td> $\text{CENTRIF}^{(S)}$ </td><td>Rotational body force</td><td> $T^{-2}$ </td><td>Centrifugal load (magnitude is input as  $\omega^2$ , where  $\omega$  is the angular velocity).</td></tr><tr><td> $\text{CORIO}^{(S)}$ </td><td>Coriolis force</td><td> $FL^{-2}T$  $(ML^{-1}T^{-1})$ </td><td>Coriolis force (magnitude is input as  $m\omega$ , where  $m$  is the mass per unit length and  $\omega$  is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis.</td></tr><tr><td>GRAV</td><td>Gravity</td><td> $LT^{-2}$ </td><td>Gravity loading in a specified direction (magnitude is input as acceleration).</td></tr><tr><td>PX</td><td>Line load</td><td> $FL^{-1}$ </td><td>Force per unit length in global X-direction.</td></tr><tr><td>PY</td><td>Line load</td><td> $FL^{-1}$ </td><td>Force per unit length in global Y-direction.</td></tr><tr><td>PZ</td><td>Line load</td><td> $FL^{-1}$ </td><td>Force per unit length in global Z-direction (only for beams in space).</td></tr><tr><td>PXNU</td><td>Line load</td><td> $FL^{-1}$ </td><td>Nonuniform force per unit length in global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.</td></tr><tr><td>PYNU</td><td>Line load</td><td> $FL^{-1}$ </td><td>Nonuniform force per unit length in global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit.</td></tr><tr><td>PZNU</td><td>Line load</td><td> $FL^{-1}$ </td><td>Nonuniform force per unit length in global Z-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. (Only for beams in space.)</td></tr><tr><td>P1</td><td>Line load</td><td> $FL^{-1}$ </td><td>Force per unit length in beam local 1-direction (only for beams in space).</td></tr></table>
