<!-- source-page: 51 -->

Generalized axisymmetric elements with twist cannot be used in contour integral calculations and in dynamic analysis. Elastic foundations are applied only to degrees of freedom $u _ { r }$ and $u _ { z }$ .

These elements should not be mixed with three-dimensional elements.

Axisymmetric elements with twist and the nodes of these elements should be used with caution within rigid bodies. If the rigid body undergoes large rotations, incorrect results may be obtained. It is recommended that rigid constraints on axisymmetric elements with twist be modeled with kinematic coupling (see “Kinematic coupling constraints,” Section 35.2.3).

Stabilization should not be used with these elements if the deformation is dominated by twist, since stabilization is applied only to the in-plane deformation.

# Axisymmetric elements with nonlinear, asymmetric deformation

These elements are intended for the linear or nonlinear analysis of structures that are initially axisymmetric but undergo nonlinear, nonaxisymmetric deformation. They are available only in Abaqus/Standard.

The elements use standard isoparametric interpolation in the r–z plane, combined with Fourier interpolation with respect to . The deformation is assumed to be symmetric with respect to the r–z plane at $\theta = 0 , \pi$ .

Up to four Fourier modes are allowed. For more general cases, full three-dimensional modeling or cylindrical element modeling is probably more economical because of the complete coupling between all deformation modes.

These elements use a set of nodes in each of several r–z planes: the number of such planes depends on the order N of Fourier interpolation used with respect to , as follows:

<table><tr><td>Number of Fourier modes N</td><td>Number of nodal planes</td><td>Nodal plane locations with respect to θ</td></tr><tr><td>1</td><td>2</td><td>0, π</td></tr><tr><td>2</td><td>3</td><td>0, π/2, π</td></tr><tr><td>3</td><td>4</td><td>0, π/3, 2π/3, π</td></tr><tr><td>4</td><td>5</td><td>0, π/4, π/2, 3π/4, π</td></tr></table>

Each element type is defined by a name such as CAXA8RN (continuum elements) or SAXA1N (shell elements). The number N should be given as the number of Fourier modes to be used with the element (N=1, 2, 3, or 4). For example, element type CAXA8R2 is a quadrilateral in the r–z plane with biquadratic interpolation in this plane and two Fourier modes for interpolation with respect to . The nodal planes associated with various Fourier modes are illustrated in Figure 27.1.2–4.

<!-- source-page: 52 -->

![](images/page-052_660ef34de9a499bb30fcb68814df9f935b9a8e73030938743436c48ca6b9c31c.jpg)  
Figure 27.1.2–4 Nodal planes of a second-order axisymmetric element with nonlinear, asymmetric deformation and (a) 1, (b) 2, (c) 3, or (d) 4 Fourier modes.

<!-- source-page: 53 -->

# 27.1.3 CHOOSING THE APPROPRIATE ELEMENT FOR AN ANALYSIS TYPE

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE

# References

• “Element library: overview,” Section 27.1.1   
• “Element type assignment,” Section 17.5.3 of the Abaqus/CAE User’s Guide

# Overview

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;   
• incompressible flow 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 same rule applies to Abaqus/CFD.

# 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

<!-- source-page: 54 -->

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:

• static and quasi-static analysis (“Static stress analysis procedures: overview,” Section 6.2.1);   
• implicit transient dynamic, explicit transient dynamic, modal dynamic, and steady-state dynamic analysis (“Dynamic analysis procedures: overview,” Section 6.3.1);   
• “Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1; and   
• “Fracture mechanics: overview,” Section 11.4.1.

# Active degrees of freedom

Stress/displacement elements have only displacement degrees of freedom. See “Conventions,” Section 1.2.2, for a discussion of the degrees of freedom in Abaqus.

# Choosing a stress/displacement element

Stress/displacement elements are available in several different element families.

# Continuum elements

• “Solid (continuum) elements,” Section 28.1.1; and   
• “Infinite elements,” Section 28.3.1.

# Structural elements

• “Membrane elements,” Section 29.1.1;   
• “Truss elements,” Section 29.2.1;   
• “Beam modeling: overview,” Section 29.3.1;   
• “Frame elements,” Section 29.4.1;   
• “Pipes and pipebends with deforming cross-sections: elbow elements,” Section 29.5.1; and   
• “Shell elements: overview,” Section 29.6.1.

# Rigid elements

• “Point masses,” Section 30.1.1;   
• “Rotary inertia,” Section 30.2.1; and   
• “Rigid elements,” Section 30.3.1.

# Connector elements

• “Connector elements,” Section 31.1.2;   
• “Springs,” Section 32.1.1;   
• “Dashpots,” Section 32.2.1;

<!-- source-page: 55 -->

• “Flexible joint element,” Section 32.3.1;   
• “Tube support elements,” Section 32.8.1; and   
• “Drag chains,” Section 32.11.1.

# Special-purpose elements

• “Cohesive elements: overview,” Section 32.5.1;   
• “Gasket elements: overview,” Section 32.6.1;   
• “Surface elements,” Section 32.7.1;   
• “Line spring elements for modeling part-through cracks in shells,” Section 32.9.1;   
• “Elastic-plastic joints,” Section 32.10.1;   
• “Eulerian elements,” Section 32.14.1;   
• “Fluid pipe connector elements,” Section 32.16.1; and   
• “Fluid pipe elements,” Section 32.15.1.

# Contact elements

• “Gap contact elements,” Section 40.2.1;   
• “Tube-to-tube contact elements,” Section 40.3.1;   
• “Slide line contact elements,” Section 40.4.1; and   
• “Rigid surface contact elements,” Section 40.5.1.

# 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:

• soils analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); and   
• geostatic analysis (“Geostatic stress state,” Section 6.8.2).

# 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,” Section 1.2.2, 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

<!-- source-page: 56 -->

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:

• “Solid (continuum) elements,” Section 28.1.1.

# 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,” Section 6.5.3).

# 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,” Section 1.2.2, 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:

• “Solid (continuum) elements,” Section 28.1.1;   
• “Truss elements,” Section 29.2.1;   
• “Shell elements: overview,” Section 29.6.1;   
• “Gap contact elements,” Section 40.2.1; and   
• “Slide line contact elements,” Section 40.4.1.

<!-- source-page: 57 -->

# 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,” Section 6.7.4).

# 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,” Section 1.2.2, 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:

• “Solid (continuum) elements,” Section 28.1.1.

# 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.

<!-- source-page: 58 -->

# Analysis types

Coupled temperature–pore pressure elements are for use in fully coupled temperature–pore pressure analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1).

# Active degrees of freedom

Coupled temperature–pore pressure elements have displacement, pore pressure, and temperature degrees of freedom. See “Conventions,” Section 1.2.2, 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:

• “Solid (continuum) elements,” Section 28.1.1.

# Diffusive (heat transfer) elements

Diffusive elements are provided in Abaqus/Standard for use in heat transfer analysis (“Uncoupled heat transfer analysis,” Section 6.5.2), 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,” Section 6.9.1) 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,” Section 1.2.2, 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:

• “Solid (continuum) elements,” Section 28.1.1;

<!-- source-page: 59 -->

• “Shell elements: overview,” Section 29.6.1 (these elements cannot be used in a mass diffusion analysis); and   
• “Gap contact elements,” Section 40.2.1.

# 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,” Section 6.5.2), including cavity radiation modeling (“Cavity radiation,” Section 41.1.1). 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,” Section 1.2.2, 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:

• “Solid (continuum) elements,” Section 28.1.1.

# Incompressible flow elements

Hybrid elements suitable for incompressible flow are available in Abaqus/CFD. These elements permit the automatic addition of degrees of freedom for the optional energy equation and turbulence models. The names of all fluid elements begin with the letters FC.

# Analysis types

The incompressible flow elements can be used in a variety of flow analyses (“Incompressible fluid dynamic analysis,” Section 6.6.2), including laminar or turbulent flows, heat transfer, and fluid-solid interaction.

<!-- source-page: 60 -->

# Active degrees of freedom

The incompressible flow elements provide primarily pressure and velocity degrees of freedom. See “Fluid element library,” Section 28.2.2, for more information on the degrees of freedom in Abaqus/CFD.

# Interpolation

The incompressible flow elements use only first-order (linear) interpolation in one, two, or three dimensions.

# Choosing an incompressible flow element

The incompressible flow elements are available only in the following element family:

• “Fluid (continuum) elements,” Section 28.2.1.

# 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:

• soils analysis (“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1); and   
• geostatic analysis (“Geostatic stress state,” Section 6.8.2).

# Active degrees of freedom

The fluid pipe and fluid pipe connector elements provide primarily pore pressure degree of freedom. See “Conventions,” Section 1.2.2, 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:

• “Fluid pipe elements,” Section 32.15.1.

# Choosing a fluid pipe connector element

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

• “Fluid pipe connector elements,” Section 32.16.1.

# 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).
