Degrees of freedom (directly related to the element family)
Number of nodes
Formulation
Integration
Each element in
Abaqus
has a unique name, such as T2D2, S4R, or C3D8I. The element name identifies each of the five aspects of an
element. The naming convention is explained in this chapter.
Family
Figure 1
shows the element families most commonly used in a stress analysis. One of the
major distinctions between different element families is the geometry type that
each family assumes.
Figure 1. Commonly used element families.
The element families that you will use in this guide—continuum, shell, beam,
truss, and rigid elements—are discussed in detail in other chapters. The other
element families are not covered in this guide; if you are interested in using
them in your models, read about them in
Abaqus Elements Guide.
The first letter or letters of an element's name indicate to which family
the element belongs. For example, the S in S4R indicates this is a shell element, while the C in C3D8I indicates this is a continuum element.
Degrees of
freedom
The degrees of freedom (dof) are the fundamental variables calculated during
the analysis. For a stress/displacement simulation the degrees of freedom are
the translations at each node. Some element families, such as the beam and
shell families, have rotational degrees of freedom as well. For a heat transfer
simulation the degrees of freedom are the temperatures at each node; a heat
transfer analysis, therefore, requires the use of different elements than a
stress analysis, since the degrees of freedom are not the same.
The following numbering convention is used for the degrees of freedom in
Abaqus:
1
Translation in direction 1
2
Translation in direction 2
3
Translation in direction 3
4
Rotation about the 1-axis
5
Rotation about the 2-axis
6
Rotation about the 3-axis
7
Warping in open-section beam elements
8
Acoustic pressure, pore pressure, or
hydrostatic fluid pressure
9
Electric potential
10
Connector material flow (units of length)
11
Temperature (or normalized
concentration in mass diffusion analysis) for continuum elements or temperature
at the first point through the thickness of beams and shells
12+
Temperature at other points through
the thickness of beams and shells
Directions 1, 2, and 3 correspond to the global 1-, 2-, and 3-directions,
respectively, unless a local coordinate system has been defined at the nodes.
Axisymmetric elements are the exception, with the displacement and rotation
degrees of freedom referred to as follows:
1
Translation in the
r-direction
2
Translation in the
z-direction
6
Rotation in the
r–z plane
Directions r (radial) and z
(axial) correspond to the global 1- and 2-directions, respectively, unless a
local coordinate system has been defined at the nodes. See
Using Shell Elements
for a discussion of defining a local coordinate system at the nodes.
In this guide our attention is restricted to structural applications.
Therefore, only elements with translational and rotational degrees of freedom
are discussed. For information on other types of elements (for example, heat
transfer elements), consult the
Abaqus Elements Guide.
By default,
Abaqus/CAE
uses the alphabetical option, x-y-z, for labeling the view
orientation triad. In general, this guide adopts the numerical option, 1-2-3,
to permit direct correspondence with degree of freedom and output labeling. For
more information on labeling of axes, see
Customizing the view triad.
Number of
nodes—order of interpolation
Displacements, rotations, temperatures, and the other degrees of freedom
mentioned in the previous section are calculated only at the nodes of the
element. At any other point in the element, the displacements are obtained by
interpolating from the nodal displacements. Usually the interpolation order is
determined by the number of nodes used in the element, as illustrated in the
examples in
Figure 2.
Figure 2. Linear brick, quadratic brick, and modified tetrahedral
elements.
Elements that have nodes only at their corners, such as the 8-node brick
shown in
Figure 2(a),
use linear interpolation in each direction and are often called linear elements
or first-order elements.
Elements with midside nodes, such as the 20-node brick shown in
Figure 2(b),
use quadratic interpolation and are often called quadratic elements or
second-order elements.
Modified triangular or tetrahedral elements with midside nodes, such as
the 10-node tetrahedron shown in
Figure 2(c),
use a modified second-order interpolation and are often called modified
elements or modified second-order elements.
Abaqus/Standard
offers a wide selection of both linear and quadratic elements.
Abaqus/Explicit
offers only linear elements, with the exception of the quadratic beam,
quadratic tetrahedral, and modified tetrahedron and triangle elements.
Typically, the number of nodes in an element is clearly identified in its
name. The 8-node brick element, as you have seen, is called C3D8; and the 8-node general shell element is called S8R. The beam element family uses a slightly different convention:
the order of interpolation is identified in the name. Thus, a first-order,
three-dimensional beam element is called B31, whereas a second-order, three-dimensional beam element is called
B32. A similar convention is used for axisymmetric shell and membrane
elements.
Formulation
An element's formulation refers to the mathematical theory used to define
the element's behavior. In the absence of adaptive meshing all of the
stress/displacement elements in
Abaqus
are based on the Lagrangian or
material description of behavior: the material
associated with an element remains associated with the element throughout the
analysis, and material cannot flow across element boundaries. In the
alternative Eulerian or
spatial description, elements are fixed in space as
the material flows through them. Eulerian methods are used commonly in fluid
mechanics simulations.
Abaqus/Standard
uses Eulerian elements to model convective heat transfer. Adaptive meshing
combines the features of pure Lagrangian and Eulerian analyses and allows the
motion of the element to be independent of the material. Eulerian elements and
adaptive meshing are not discussed in this guide.
To accommodate different types of behavior, some element families in
Abaqus
include elements with several different formulations. For example, the shell
element family has three classes: one suitable for general-purpose shell
analysis, another for thin shells, and yet another for thick shells. (These
shell element formulations are explained in
Using Shell Elements.)
Some
Abaqus/Standard
element families have a standard formulation as well as some alternative
formulations. Elements with alternative formulations are identified by an
additional character at the end of the element name. For example, the
continuum, beam, and truss element families include members with a hybrid
formulation in which the pressure (continuum elements) or axial force (beam and
truss elements) is treated as an additional unknown; these elements are
identified by the letter “H” at the end of the name (C3D8H or B31H).
Some element formulations allow coupled field problems to be solved. For
example, elements whose names begin with the letter C and end with the letter T
(such as C3D8T) possess both mechanical and thermal degrees of freedom and are
intended for coupled thermomechanical simulations.
Several of the most commonly used element formulations are discussed later
in this guide.
Integration
Abaqus
uses numerical techniques to integrate various quantities over the volume of
each element. Using Gaussian quadrature for most elements,
Abaqus
evaluates the material response at each integration point in each element. Some
elements in
Abaqus
can use full or reduced integration, a choice that can have a significant
effect on the accuracy of the element for a given problem, as discussed in
detail in
Element formulation and integration.
Abaqus
uses the letter “R” at the end of the element name to distinguish
reduced-integration elements (unless they are also hybrid elements, in which
case the element name ends with the letters
“RH”). For example, CAX4 is the 4-node, fully integrated, linear, axisymmetric solid
element; and CAX4R is the reduced-integration version of the same element.
Abaqus/Standard
offers both full and reduced-integration elements;
Abaqus/Explicit
offers only reduced-integration elements with the exception of the modified
tetrahedron and triangle elements and the fully integrated first-order shell,
membrane, and brick elements.
