Choosing the appropriate element for an analysis type

The Abaqus element library contains the following:

  • stress/displacement elements, including contact elements, connector elements such as springs, and special-purpose elements such as Eulerian elements and surface elements;

  • pore pressure elements;

  • coupled temperature-displacement elements;

  • coupled thermal-electrical-structural elements;

  • coupled temperature–pore pressure displacement elements;

  • heat transfer or mass diffusion elements;

  • forced convection heat transfer elements;

  • fluid pipe and fluid pipe connector elements;

  • coupled thermal-electrical elements;

  • piezoelectric elements;

  • electromagnetic elements;

  • acoustic elements; and

  • user-defined elements.

Each of these element types is described below.

Within Abaqus/Standard or Abaqus/Explicit, a model can contain elements that are not appropriate for the particular analysis type chosen; such elements will be ignored. However, an Abaqus/Standard model cannot contain elements that are not available in Abaqus/Standard; likewise, an Abaqus/Explicit model cannot contain elements that are not available in Abaqus/Explicit.

The following topics are discussed:

Related Topics
About the element library
In Other Guides
Element type assignment

ProductsAbaqus/StandardAbaqus/ExplicitAbaqus/CAE

Stress/displacement elements

Stress/displacement elements are used in the modeling of linear or complex nonlinear mechanical analyses that possibly involve contact, plasticity, and/or large deformations. Stress/displacement elements can also be used for thermal-stress analysis, where the temperature history can be obtained from a heat transfer analysis carried out with diffusive elements.

Analysis types

Stress/displacement elements can be used in the following analysis types:

Active degrees of freedom

Stress/displacement elements have only displacement degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Pore pressure elements

Pore pressure elements are provided in Abaqus/Standard for modeling fully or partially saturated fluid flow through a deforming porous medium. The names of all pore pressure elements include the letter P (pore pressure). These elements cannot be used with hydrostatic fluid elements.

Analysis types

Pore pressure elements can be used in the following analysis types:

Active degrees of freedom

Pore pressure elements have both displacement and pore pressure degrees of freedom. In second-order elements the pore pressure degrees of freedom are active only at the corner nodes. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

These elements use either linear- or second-order (quadratic) interpolation for the geometry and displacements in two or three directions. The pore pressure is interpolated linearly from the corner nodes. Curved element edges should be avoided; exact linear spatial pore pressure variations cannot be obtained with curved edges.

For output purposes the pore pressure at the midside nodes of second-order elements is determined by linear interpolation from the corner nodes.

Choosing a pore pressure element

Pore pressure elements are available only in the following element family:

Coupled temperature-displacement elements

Coupled temperature-displacement elements are used in problems for which the stress analysis depends on the temperature solution and the thermal analysis depends on the displacement solution. An example is the heating of a deforming body whose properties are temperature dependent by plastic dissipation or friction. The names of all coupled temperature-displacement elements include the letter T.

Analysis types

Coupled temperature-displacement elements are for use in fully coupled temperature-displacement analysis (Fully coupled thermal-stress analysis).

Active degrees of freedom

Coupled temperature-displacement elements have both displacement and temperature degrees of freedom. In second-order elements the temperature degrees of freedom are active at the corner nodes. In modified triangle and tetrahedron elements the temperature degrees of freedom are active at every node. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

Coupled temperature-displacement elements use either linear or parabolic interpolation for the geometry and displacements. The temperature is always interpolated linearly. In second-order elements curved edges should be avoided; exact linear spatial temperature variations for these elements cannot be obtained with curved edges.

For output purposes the temperature at the midside nodes of second-order elements is determined by linear interpolation from the corner nodes.

Choosing a coupled temperature-displacement element

Coupled temperature-displacement elements are available in the following element families:

Coupled thermal-electrical-structural elements

Coupled thermal-electrical-structural elements are used when a solution for the displacement, electrical potential, and temperature degrees of freedom must be obtained simultaneously. In these types of problems, coupling between the temperature and displacement degrees of freedom arises from temperature-dependent material properties, thermal expansion, and internal heat generation, which is a function of inelastic deformation of the material. The coupling between the temperature and electrical degrees of freedom arises from temperature-dependent electrical conductivity and internal heat generation (Joule heating), which is a function of the electrical current density. The names of the coupled thermal-electrical-structural elements begin with the letter Q.

Analysis types

Coupled thermal-electrical-structural elements are for use in a fully coupled thermal-electrical-structural analysis (Fully coupled thermal-electrical-structural analysis).

Active degrees of freedom

Coupled thermal-electrical-structural elements have displacement, electrical potential, and temperature degrees of freedom. In second-order elements the electrical potential and temperature degrees of freedom are active at the corner nodes. In modified tetrahedron elements the electrical potential and temperature degrees of freedom are active at every node. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

Coupled thermal-electrical-structural elements use either linear or parabolic interpolation for the geometry and displacements. The electrical potential and temperature are always interpolated linearly. In second-order elements curved edges should be avoided; exact linear spatial electrical potential and temperature variations for these elements cannot be obtained with curved edges.

For output purposes the electrical potential and temperature at the midside nodes of second-order elements are determined by linear interpolation from the corner nodes.

Choosing a coupled thermal-electrical-structural element

Coupled thermal-electrical-structural elements are available only in the following element family:

Coupled temperature–pore pressure elements

Coupled temperature–pore pressure elements are used in Abaqus/Standard  for modeling fully or partially saturated fluid flow through a deforming porous medium in which the stress, fluid pore pressure, and temperature fields are fully coupled to one another. The names of all coupled temperature–pore pressure elements include the letters T and P. These elements cannot be used with hydrostatic fluid elements.

Analysis types

Coupled temperature–pore pressure elements are for use in fully coupled temperature–pore pressure analysis (Coupled pore fluid diffusion and stress analysis).

Active degrees of freedom

Coupled temperature–pore pressure elements have displacement, pore pressure, and temperature degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

These elements use either linear- or second-order (quadratic) interpolation for the geometry and displacements. The temperature and pore pressure are always interpolated linearly.

Choosing a coupled temperature–pore pressure element

Coupled temperature–pore pressure elements are available in the following element family:

Diffusive (heat transfer) elements

Diffusive elements are provided in Abaqus/Standard for use in heat transfer analysis (Uncoupled heat transfer analysis), where they allow for heat storage (specific heat and latent heat effects) and heat conduction. They provide temperature output that can be used directly as input to the equivalent stress elements. The names of all diffusive heat transfer elements begin with the letter D.

Analysis types

The diffusive elements can be used in mass diffusion analysis (Mass diffusion analysis) as well as in heat transfer analysis.

Active degrees of freedom

When used for heat transfer analysis, the diffusive elements have only temperature degrees of freedom. When they are used in a mass diffusion analysis, they have normalized concentration, instead of temperature, degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

The diffusive elements use either first-order (linear) interpolation or second-order (quadratic) interpolation in one, two, or three dimensions.

Choosing a diffusive element

Diffusive elements are available in the following element families:

Forced convection heat transfer elements

Forced convection heat transfer elements are provided in Abaqus/Standard to allow for heat storage (specific heat) and heat conduction, as well as the convection of heat by a fluid flowing through the mesh (forced convection). All forced convection heat transfer elements provide temperature output, which can be used directly as input to the equivalent stress elements. The names of all forced convection heat transfer elements begin with the letters DCC.

Analysis types

The forced convection heat transfer elements can be used in heat transfer analyses (Uncoupled heat transfer analysis), including cavity radiation modeling (Cavity Radiation in Abaqus/Standard). The forced convection heat transfer elements can be used together with the diffusive elements.

Active degrees of freedom

The forced convection heat transfer elements have temperature degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

The forced convection heat transfer elements use only first-order (linear) interpolation in one, two, or three dimensions.

Choosing a forced convection heat transfer element

Forced convection heat transfer elements are available only in the following element family:

Fluid pipe and fluid pipe connector elements

Fluid pipe elements suitable for modeling incompressible pipe flow and fluid pipe connector elements suitable for modeling the junction between two pipes are available in Abaqus/Standard. These elements have only pore pressure degree of freedom. The names of all fluid pipe elements begin with the letters FP. The names of all fluid pipe connector elements begin with the letters FPC.

Analysis types

The fluid pipe and fluid pipe connector elements can be used in the following analyses:

Active degrees of freedom

The fluid pipe and fluid pipe connector elements provide primarily pore pressure degree of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Choosing a fluid pipe element

The fluid pipe elements are available only in the following element family:

Choosing a fluid pipe connector element

The fluid pipe connector elements are available only in the following element family:

Coupled thermal-electrical elements

Coupled thermal-electrical elements are provided in Abaqus/Standard for use in modeling heating that arises when an electrical current flows through a conductor (Joule heating).

Analysis types

The Joule heating effect requires full coupling of the thermal and electrical problems (see Coupled thermal-electrical analysis). The coupling arises from two sources: temperature-dependent electrical conductivity and the heat generated in the thermal problem by electric conduction.

These elements can also be used to perform uncoupled electric conduction analysis in all or part of the model. In such analysis only the electric potential degree of freedom is activated, and all heat transfer effects are ignored. This capability is available by omitting the thermal conductivity from the material definition.

The coupled thermal-electrical elements can also be used in heat transfer analysis (Uncoupled heat transfer analysis), in which case all electric conduction effects are ignored. This feature is quite useful if a coupled thermal-electrical analysis is followed by a pure heat conduction analysis (such as a welding simulation followed by cool down).

The elements cannot be used in any of the stress/displacement analysis procedures.

Active degrees of freedom

Coupled thermal-electrical elements have both temperature and electrical potential degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Interpolation

Coupled thermal-electrical elements are provided with first- or second-order interpolation of the temperature and electrical potential.

Choosing a coupled thermal-electrical element

Coupled thermal-electrical elements are available only in the following element family:

Piezoelectric elements

Piezoelectric elements are provided in Abaqus/Standard for problems in which a coupling between the stress and electrical potential (the piezoelectric effect) must be modeled.

Analysis types

Piezoelectric elements are for use in piezoelectric analysis (Piezoelectric analysis).

Active degrees of freedom

The piezoelectric elements have both displacement and electric potential degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus. The piezoelectric effect is discussed further in Piezoelectric analysis.

Interpolation

Piezoelectric elements are available with first- or second-order interpolation of displacement and electrical potential.

Choosing a piezoelectric element

Piezoelectric elements are available in the following element families:

Electromagnetic elements

Electromagnetic elements are provided in Abaqus/Standard for problems that require the computation of the magnetic fields (such as a magnetostatic analysis) or for problems in which a coupling between electric and magnetic fields must be modeled (such as an eddy current analysis).

Analysis types

Electromagnetic elements are for use in magnetostatic and eddy current analyses (Magnetostatic analysis and Eddy current analysis).

Active degrees of freedom

Electromagnetic elements have magnetic vector potential as the degree of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus. Magnetostatic analysis is discussed further in Magnetostatic analysis, while the electromagnetic coupling that occurs in an eddy current analysis is discussed further in Eddy current analysis.

Interpolation

Electromagnetic elements are available with zero-order element edge–based interpolation of the magnetic vector potential.

Choosing an electromagnetic element

Electromagnetic elements are available in the following element family:

Acoustic elements

Acoustic elements are used for modeling an acoustic medium undergoing small pressure changes. The solution in the acoustic medium is defined by a single pressure variable. Impedance boundary conditions representing absorbing surfaces or radiation to an infinite exterior are available on the surfaces of these acoustic elements.

Acoustic infinite elements, which improve the accuracy of analyses involving exterior domains, and acoustic-structural interface elements, which couple an acoustic medium to a structural model, are also provided.

Analysis types

Acoustic elements are for use in acoustic and coupled acoustic-structural analysis (Acoustic, shock, and coupled acoustic-structural analysis).

Active degrees of freedom

Acoustic elements have acoustic pressure as a degree of freedom. Coupled acoustic-structural elements also have displacement degrees of freedom. See Conventions for a discussion of the degrees of freedom in Abaqus.

Choosing an acoustic element

Acoustic elements are available in the following element families:

The acoustic elements can be used alone but are often used with a structural model in a coupled analysis. Acoustic interface elements describes interface elements that allow this acoustic pressure field to be coupled to the displacements of the surface of the structure. Acoustic elements can also interact with solid elements through the use of surface-based tie constraints; see Acoustic, shock, and coupled acoustic-structural analysis.

Using the same mesh with different analysis or element types

You may want to use the same mesh with different analysis or element types. This may occur, for example, if both stress and heat transfer analyses are intended for a particular geometry or if the effect of using either reduced- or full-integration elements is being investigated. Care should be taken when doing this since unexpected error messages may result for one of the two element types if the mesh is distorted. For example, a stress analysis with C3D10 elements may run successfully, but a heat transfer analysis using the same mesh with DC3D10 elements may terminate during the datacheck portion of the analysis with an error message stating that the elements are excessively distorted or have negative volumes. This apparent inconsistency is caused by the different integration locations for the different element types. Such problems can be avoided by ensuring that the mesh is not distorted excessively.