One-dimensional heat transfer, coupled thermal/electrical, and acoustic elements are
available only in Abaqus/Standard. In addition, structural link (truss) elements are available in both Abaqus/Standard and Abaqus/Explicit. These elements can be used in two- or three-dimensional space to transmit loads or
fluxes along the length of the element.
Two-Dimensional Elements
Abaqus provides several different types of two-dimensional elements. For structural applications
these include plane stress elements and plane strain elements. Abaqus/Standard also provides generalized plane strain elements for structural applications.
Plane Stress Elements
Plane stress elements can be used when the thickness of a body or domain is small
relative to its lateral (in-plane) dimensions. The stresses are functions of planar
coordinates alone, and the out-of-plane normal and shear stresses are equal to zero.
Plane stress elements must be defined in the
X–Y plane, and all loading and deformation are
also restricted to this plane. This modeling method generally applies to thin, flat
bodies. For anisotropic materials the Z-axis must be a principal
material direction.
In Abaqus/Standard the output for the volume of a plane stress solid element is always the initial volume,
irrespective of the level of deformation. However, the volume that is utilized for the
finite element calculations depends on the material response. The formulation enforces
kinematic incompressibility of the element when it is used with a linear elastic material
model (or nonlinear material models whose elastic behavior is defined as linear elastic)
and the initial volume is used for all the calculations. This approach is consistent with
the intended use of linear elastic materials for applications involving small elastic
strains (and small volume changes) only. However, when plane stress solid elements are
used with a compressible hyperelastic material model (or other material models whose
elastic behavior is defined as compressible hyperelastic), the volume of the element
evolves based on the compressibility of the material. The finite element calculations
(that is, residual calculations) in this case utilize the current volume.
In Abaqus/Explicit the formulation of a plane stress solid element generally accounts for compressibility
of the material response, and the current volume is used for all the calculations. The
output of the element volume also corresponds to the current volume.
Plane Strain Elements
Plane strain elements can be used when it can be assumed that the strains in a loaded
body or domain are functions of planar coordinates alone and the out-of-plane normal and
shear strains are equal to zero.
Plane strain elements must be defined in the
X–Y plane, and all loading and deformation are
also restricted to this plane. This modeling method is generally used for bodies that are
very thick relative to their lateral dimensions, such as shafts, concrete dams, or walls.
Plane strain theory might also apply to a typical slice of an underground tunnel that lies
along the Z-axis. For anisotropic materials the
Z-axis must be a principal material direction.
Since plane strain theory assumes zero strain in the thickness direction, isotropic
thermal expansion might cause large stresses in the thickness direction.
Generalized Plane Strain Elements
Generalized plane strain elements provide for the modeling of cases in Abaqus/Standard where the structure has constant curvature (and, hence, no gradients of solution
variables) with respect to one material direction—the “axial” direction of the model. The
formulation, thus, involves a model that lies between two planes that can move with
respect to each other and, hence, cause strain in the axial direction of the model that
varies linearly with respect to position in the planes, the variation being due to the
change in curvature. In the initial configuration the bounding planes can be parallel or
at an angle to each other, the latter case allowing the modeling of initial curvature of
the model in the axial direction. The concept is illustrated in Figure 1. Generalized plane strain elements are typically used to model a section of a long
structure that is free to expand axially or is subjected to axial loading.
Figure 1. Generalized plane strain model.
Each generalized plane strain element has three, four, six, or eight conventional nodes,
at each of which x- and y-coordinates,
displacements, etc. are stored. These nodes determine the position and motion of the
element in the two bounding planes. Each element also has a reference node, which is
usually the same node for all the generalized plane strain elements in the model. The
reference node of a generalized plane strain element should not be used as a conventional
node in any element in the model. The reference node has three degrees of freedom 3, 4,
and 5: (, , and ). The first degree of freedom () is the change in length of the axial material fiber connecting this
node and its image in the other bounding plane. This displacement is positive as the
planes move apart; therefore, there is a tensile strain in the axial fiber. The second and
third degrees of freedom (, ) are the components of the relative rotation of one bounding plane with
respect to the other. The values stored are the two components of rotation about the
X- and Y-axes in the bounding planes (that is,
in the cross-section of the model). Positive rotation about the
X-axis causes increasing axial strain with respect to the
y-coordinate in the cross-section; positive rotation about the
Y-axis causes decreasing axial strain with respect to the
x-coordinate in the cross-section. The x- and
y-coordinates of a generalized plane strain element reference node ( and discussed below) remain fixed throughout all steps of an analysis. From
the degrees of freedom of the reference node, the length of the axial material fiber
passing through the point with current coordinates (x,
y) in a bounding plane is defined as
where
t
is the current length of the fiber,
is the initial length of the fiber passing through the reference node (given as
part of the element section definition),
is the displacement at the reference node (stored as degree of freedom 3 at the
reference node),
and
are the total values of the components of the angle between the bounding planes
(the original values of , are given as part of the element section definition—see Defining the Elements Section Properties: the changes in these
values are the degrees of freedom 4 and 5 of the reference node), and
and
are the coordinates of the reference node in a bounding plane.
The strain in the axial direction is defined immediately from this axial fiber length.
The strain components in the cross-section of the model are computed from the
displacements of the regular nodes of the elements in the usual way. Since the solution is
assumed to be independent of the axial position, there are no transverse shear strains.
Three-Dimensional Elements
Three-dimensional elements are defined in the global X,
Y, Z space. These elements are used when the
geometry and/or the applied loading are too complex for any other element type with fewer
spatial dimensions.
Cylindrical Elements
Cylindrical elements are three-dimensional elements defined in the global
X, Y, Z space. These elements
are used to model bodies with circular or axisymmetric geometry subjected to general,
nonaxisymmetric loading. Cylindrical elements are available only in Abaqus/Standard.
Cylindrical elements are useful in situations where the expected solution over a relatively
large angle is nearly axisymmetric. In this case a very coarse mesh of cylindrical elements
is often sufficient. Footprint and steady-state rolling analyses of tires are good examples
of where cylindrical elements have distinct advantages over conventional continuum elements
(see Steady-state rolling analysis of a tire). If, however, the
expected solution has significant nonaxisymmetric components, a finer mesh of cylindrical
elements will be needed and it might be more economical to use conventional continuum
elements.
Axisymmetric Elements
Axisymmetric elements provide for the modeling of bodies of revolution under axially
symmetric loading conditions. A body of revolution is generated by revolving a plane
cross-section about an axis (the symmetry axis) and is readily described in cylindrical
polar coordinates r, z, and . Figure 2 shows a typical reference cross-section at . The radial and axial coordinates of a point on this cross-section are
denoted by r and z, respectively. At , the radial and axial coordinates coincide with the global Cartesian
X- and Y-coordinates.
Figure 2. Reference cross-section and element in an axisymmetric solid.
Abaqus does not apply boundary conditions automatically to nodes that are located on the
symmetry axis in axisymmetric models. If required, you should apply them directly. Radial
boundary conditions at nodes located on the z-axis are appropriate for
most problems because without them nodes might displace across the symmetry axis, violating
the principle of compatibility. However, there are some analyses, such as penetration
calculations, where nodes along the symmetry axis should be free to move; boundary
conditions should be omitted in these cases.
If the loading and material properties are independent of , the solution in any r–z plane
completely defines the solution in the body. Consequently, axisymmetric elements can be used
to analyze the problem by discretizing the reference cross-section at . Figure 2 shows an element of an axisymmetric body. The nodes i,
j, k, and l are actually
nodal “circles,” and the volume of material associated with the element is that of a body of
revolution, as shown in the figure. The value of a prescribed nodal load or reaction force
is the total value on the ring; that is, the value integrated around the circumference.
Regular Axisymmetric Elements
Regular axisymmetric elements for structural applications allow for only radial and axial
loading and have isotropic or orthotropic material properties, with being a principal direction. Any radial displacement in such an element
will induce a strain in the circumferential direction (“hoop” strain); and since the
displacement must also be purely axisymmetric, there are only four possible nonzero
components of strain (, , , and ).
Generalized Axisymmetric Stress/Displacement Elements with Twist
Axisymmetric solid elements with twist are available only in Abaqus/Standard for the analysis of structures that are axially symmetric but can twist about their
symmetry axis. This element family is similar to the axisymmetric elements discussed
above, except that it allows for a circumferential loading component (which is independent
of ) and for general material anisotropy. Under these conditions, there
might be displacements in the -direction that vary with r and
z but not with . The problem remains axisymmetric because the solution does not vary as
a function of so that the deformation of any
r–z plane characterizes the deformation in the
entire body. Initially the elements define an axisymmetric reference geometry with respect
to the r–z plane at , where the r-direction corresponds to the global
X-direction and the z-direction corresponds to
the global Y-direction. Figure 3 shows an axisymmetric model consisting of two elements. The figure also shows the local
cylindrical coordinate system at node 100.
Figure 3. Reference and deformed cross-section in an axisymmetric solid with twist.
The motion at a node of an axisymmetric element with twist is described by the radial
displacement , the axial displacement , and the twist (in radians) about the z-axis, each of which is
constant in the circumferential direction, so that the deformed geometry remains
axisymmetric. Figure 3(b) shows the deformed geometry of the reference model shown in Figure 3(a) and the local cylindrical coordinate system at the displaced location of node 100,
for a twist .
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 and .
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 might be obtained. It is recommended that rigid constraints on axisymmetric
elements with twist be modeled with kinematic coupling (see Kinematic Coupling Constraints).
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 .
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:
Number of Fourier modes N
Number of nodal planes
Nodal plane locations with respect to
1
2
2
3
3
4
4
5
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 4.
Figure 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.