Beam Element Library

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

This page discusses:

See Also
About Beam Modeling
Choosing a Beam Element
In Other Guides
*BEAM GENERAL SECTION
*BEAM SECTION

ProductsAbaqus/StandardAbaqus/Explicit

Element Types

Beams in a Plane

B21

2-node linear beam

B21H(S)

2-node linear beam, hybrid formulation

B22

3-node quadratic beam

B22H(S)

3-node quadratic beam, hybrid formulation

B23(S)

2-node cubic beam

B23H(S)

2-node cubic beam, hybrid formulation

PIPE21

2-node linear pipe

PIPE21H(S)

2-node linear pipe, hybrid formulation

PIPE22(S)

3-node quadratic pipe

PIPE22H(S)

3-node quadratic pipe, hybrid formulation

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 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

B31

2-node linear beam

B31H(S)

2-node linear beam, hybrid formulation

B32

3-node quadratic beam

B32H(S)

3-node quadratic beam, hybrid formulation

B33(S)

2-node cubic beam

B33H(S)

2-node cubic beam, hybrid formulation

PIPE31

2-node linear pipe

PIPE31H(S)

2-node linear pipe, hybrid formulation

PIPE32(S)

3-node quadratic pipe

PIPE32H(S)

3-node quadratic pipe, hybrid formulation

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

B31OS(S)

2-node linear beam

B31OSH(S)

2-node linear beam, hybrid formulation

B32OS(S)

3-node quadratic beam

B32OSH(S)

3-node quadratic beam, hybrid formulation

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) Nx, Ny, the direction cosines of the normal.

Beams in space: X, Y, Z, also (optional) Nx, Ny, Nz, the direction cosines of the second local cross-section 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, channel, hat, I, L, and linear generalized section types.

Local orientations defined as described in Orientations 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.

Input File Usage

Use either of the following options:

BEAM SECTION
BEAM GENERAL SECTION

Element-Based Loading

Distributed Loads

Distributed loads are specified as described in Distributed Loads.

*dload
  1. Load ID (*DLOAD): CENT(S)
  2. FL−2 (ML−1T−2)

  3. Centrifugal force (magnitude is input as m⁢ω2, where m is the mass per unit length and ω is the angular velocity).

  1. Load ID (*DLOAD): CENTRIF(S)
  2. T−2

  3. Centrifugal load (magnitude is input as ω2, where ω is the angular velocity).

  1. Load ID (*DLOAD): CORIO(S)
  2. FL−2T (ML−1T−1)

  3. Coriolis force (magnitude is input as m⁢ω, where m is the mass per unit length and ω is the angular velocity). The load stiffness due to Coriolis loading is not accounted for in direct steady-state dynamics analysis.

  1. Load ID (*DLOAD): GRAV
  2. LT−2

  3. Gravity loading in a specified direction (magnitude is input as acceleration).

  1. Load ID (*DLOAD): PX
  2. FL−1

  3. Force per unit length in global X-direction.

  1. Load ID (*DLOAD): PY
  2. FL−1

  3. Force per unit length in global Y-direction.

  1. Load ID (*DLOAD): PZ
  2. FL−1

  3. Force per unit length in global Z-direction (only for beams in space).

  1. Load ID (*DLOAD): PXNU
  2. FL−1

  3. Nonuniform force per unit length in global X-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard  and VDLOAD in Abaqus/Explicit.

  1. Load ID (*DLOAD): PYNU
  2. FL−1

  3. Nonuniform force per unit length in global Y-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard  and VDLOAD in Abaqus/Explicit.

  1. Load ID (*DLOAD): PZNU
  2. FL−1

  3. 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.)

  1. Load ID (*DLOAD): P1
  2. FL−1

  3. Force per unit length in beam local 1-direction (only for beams in space).

  1. Load ID (*DLOAD): P2
  2. FL−1

  3. Force per unit length in beam local 2-direction.

  1. Load ID (*DLOAD): P1NU
  2. FL−1

  3. Nonuniform force per unit length in beam local 1-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard and VDLOAD in Abaqus/Explicit. (Only for beams in space.)

  1. Load ID (*DLOAD): P2NU
  2. FL−1

  3. Nonuniform force per unit length in beam local 2-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard  and VDLOAD in Abaqus/Explicit.

  1. Load ID (*DLOAD): ROTA(S)
  2. T−2

  3. Rotary acceleration load (magnitude is input as α, where α is the rotary acceleration).

  1. Load ID (*DLOAD): ROTDYNF(S)
  2. T−1

  3. Rotordynamic load (magnitude is input as ω, where ω is the angular velocity).

*dload

The following load types are available only for PIPE elements:

  1. Load ID (*DLOAD): HPI
  2. FL−2

  3. Hydrostatic internal pressure (closed-end condition), varying linearly with the global Z-coordinate.

  1. Load ID (*DLOAD): HPE
  2. FL−2

  3. Hydrostatic external pressure (closed-end condition), varying linearly with the global Z-coordinate.

  1. Load ID (*DLOAD): PI
  2. FL−2

  3. Uniform internal pressure (closed-end condition).

  1. Load ID (*DLOAD): PE
  2. FL−2

  3. Uniform external pressure (closed-end condition).

  1. Load ID (*DLOAD): PENU
  2. FL−2

  3. Nonuniform external pressure (closed-end condition) with magnitude supplied via user subroutine DLOAD.

  1. Load ID (*DLOAD): PINU
  2. FL−2

  3. Nonuniform internal pressure (closed-end condition) with magnitude supplied via user subroutine DLOAD.

Abaqus/Aqua Loads

Abaqus/Aqua loads are specified as described in Abaqus/Aqua Analysis. They are not available for open-section beams and do not apply to beams that are defined to have additional inertia due to immersion in fluid (see Additional Inertia due to Immersion in Fluid). In Abaqus/Explicit, Aqua loads can be applied only on linear beam and pipe elements.

*cload/ *dload
  1. Load ID (*CLOAD/ *DLOAD): FDD
  2. FL−1

  3. Transverse fluid drag load.

  1. Load ID (*CLOAD/ *DLOAD): FD1
  2. F

  3. Fluid drag force on the first end of the beam (node 1).

  1. Load ID (*CLOAD/ *DLOAD): FD2
  2. F

  3. Fluid drag force on the second end of the beam (node 2 or node 3).

  1. Load ID (*CLOAD/ *DLOAD): FDT
  2. FL−1

  3. Tangential fluid drag load.

  1. Load ID (*CLOAD/ *DLOAD): FI
  2. FL−1

  3. Transverse fluid inertia load.

  1. Load ID (*CLOAD/ *DLOAD): FI1
  2. F

  3. Fluid inertia force on the first end of the beam (node 1).

  1. Load ID (*CLOAD/ *DLOAD): FI2
  2. F

  3. Fluid inertia force on the second end of the beam (node 2 or node 3).

  1. Load ID (*CLOAD/ *DLOAD): PB
  2. FL−1

  3. Buoyancy load (closed-end condition).

  1. Load ID (*CLOAD/ *DLOAD): WDD
  2. FL−1

  3. Transverse wind drag load.

  1. Load ID (*CLOAD/ *DLOAD): WD1
  2. F

  3. Wind drag force on the first end of the beam (node 1).

  1. Load ID (*CLOAD/ *DLOAD): WD2
  2. F

  3. Wind drag force on the second end of the beam (node 2 or node 3).

Foundations

Foundations are available only in Abaqus/Standard and are specified as described in Element Foundations.

*foundation
  1. Load ID (*FOUNDATION): FX(S)
  2. FL−2

  3. Stiffness per unit length in global X-direction.

  1. Load ID (*FOUNDATION): FY(S)
  2. FL−2

  3. Stiffness per unit length in global Y-direction.

  1. Load ID (*FOUNDATION): FZ(S)
  2. FL−2

  3. Stiffness per unit length in global Z-direction (only for beams in space).

  1. Load ID (*FOUNDATION): F1(S)
  2. FL−2

  3. Stiffness per unit length in beam local 1-direction (only for beams in space).

  1. Load ID (*FOUNDATION): F2(S)
  2. FL−2

  3. Stiffness per unit length in beam local 2-direction.

Surface-Based Loading

Distributed Loads

Surface-based distributed loads are specified as described in Distributed Loads.

*dsload
  1. Load ID (*DSLOAD): P
  2. FL−1

  3. Force per unit length in beam local 2-direction. The distributed surface force is positive in the direction opposite to the surface normal.

  1. Load ID (*DSLOAD): PNU
  2. FL−1

  3. Nonuniform force per unit length in beam local 2-direction with magnitude supplied via user subroutine DLOAD in Abaqus/Standard  and VDLOAD in Abaqus/Explicit. The distributed surface force is positive in the direction opposite to the surface normal.

Incident Wave Loading

Incident wave loading is also available for these elements, with some restrictions. See Acoustic and Shock Loads.

Element Output

See Beam Cross-Section Library for a description of the beam element output locations.

Stress, Strain, and Other Tensor Components

Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors, except for meshed sections, have the same components. For example, the stress components are as follows:

S11

Axial stress.

S22

Hoop stress (available only for pipe elements).

S33

Radial stress (available only for thick-walled pipe elements).

S12

Shear stress caused by torsion (available only for beam-type elements in space). This component is not available when thin-walled, open sections are employed (I-section, L-section, and arbitrary open section).

Stress and strain for section points for meshed sections

S11

Axial stress.

S12

Shear stress along the second cross-section axis caused by shear force and, for beam elements in space, torsion.

S13

Shear stress along the first cross-section axis caused by shear force and torsion (available only for beams in space).

Section Forces, Moments, and Transverse Shear Forces

SF1

Axial force.

SF2

Transverse shear force in the local 2-direction (not available for B23, B23H, B33, B33H).

SF3

Transverse shear force in the local 1-direction (available only for beams in space, not available for B33, B33H).

SM1

Bending moment about the local 1-axis.

SM2

Bending moment about the local 2-axis (available only for beams in space).

SM3

Twisting moment about the beam axis (available only for beams in space).

BIMOM

Bimoment due to warping (available only for open-section beams in space).

ESF1

Effective axial force for beams subjected to pressure loading (available for all Abaqus/Standard stress/displacement analysis types except response spectrum and random response).

See Beam element formulation for the definitions of the section forces and moments.

The effective axial section force for beams subjected to pressure loading is defined as

ESF1=SF1+pe⁢Ae-pi⁢Ai,

where pe and pi are the external and the internal pressures, respectively, and Ae and Ai are the external and the internal pipe areas as defined in the load definition. The pressure loadings (with a closed-end condition) that are relevant to the effective axial force are external/internal pressure (load types PE, PI, PENU, and PINU); external/internal hydrostatic pressure (load types HPE and HPI); and, in an Abaqus/Aqua environment, buoyancy pressure, PB, which includes dynamic pressure if waves are present.

For beams that are not subjected to pressure loading, the effective axial force ESF1 is equal to the usual axial force SF1.

Section Strains, Curvatures, and Transverse Shear Strains

SE1

Axial strain.

SE2

Transverse shear strain in the local 2-direction (not available for B23, B23H, B33, and B33H).

SE3

Transverse shear strain in the local 1-direction (available only for beams in space, not available for B33 and B33H).

SK1

Curvature change about the local 1-axis.

SK2

Curvature change about the local 2-axis (available only for beams in space).

SK3

Twist of the beam (available only for beams in space).

BICURV

Bicurvature due to warping (available only for open-section beams in space).

Beam Radius

BRADIUS
Original beam radius for a solid circular beam.

Node Ordering on Elements



For beams in space an additional node may be given after a beam element's connectivity (in the element definition—see Element Definition) to define the approximate direction of the first cross-section axis, n1. See Beam Element Cross-Section Orientation for details.

Numbering of Integration Points for Output