About the Abaqus element library

All elements use numerical integration to allow complete generality in material behavior. Shell and beam element properties can be defined as general section behaviors, or each cross-section of the element can be integrated numerically, so that nonlinear response can be tracked accurately when needed. A composite layered section can be specified, with different materials at different heights through the section. Some special elements (such as line springs) use an approximate analytical solution to model nonlinear behavior.

All of the elements in Abaqus are formulated in a global Cartesian coordinate system except the axisymmetric elements, which are formulated in terms of r–z coordinates. In almost all elements, primary vector quantities (such as displacements $u$ and rotations $ϕ$ ) are defined in terms of nodal values with scalar interpolation functions. For example, in elements with a two-dimensional topology the interpolation can be written as

u (g, h) = N^{N} (g, h) u^{N},

where the interpolation functions $N^{N} (g, h)$ are written in terms of the parametric coordinates g and h. In most element types the same parametric interpolation is used for the coordinate vector $x$ :

x (g, h) = N^{N} (g, h) x^{N} .

Such isoparametric elements are guaranteed to be able to represent all rigid body modes and homogeneous deformation modes exactly, a necessary condition for convergence to the exact solution as the mesh is refined.

All elements in Abaqus are integrated numerically. Hence, the virtual work integral as described in Nonlinear solution methods in Abaqus/Standard will be replaced by a summation:

\int_{V} σ : δ D d V \to \overset{n}{\sum_{i = 1}} σ_{i} : δ D_{i} V_{i},

where n is the number of integration points in the element and $V_{i}$ is the volume associated with integration point i. Abaqus will use either “full” or “reduced” integration. For full integration the number of integration points is sufficient to integrate the virtual work expression exactly, at least for linear material behavior. All triangular and tetrahedral elements in Abaqus use full integration. Reduced integration can be used for quadrilateral and hexahedral elements; in this procedure the number of integration points is sufficient to integrate exactly the contributions of the strain field that are one order less than the order of interpolation. The (incomplete) higher-order contributions to the strain field present in these elements will not be integrated.

The advantage of the reduced integration elements is that the strains and stresses are calculated at the locations that provide optimal accuracy, the so-called Barlow points (Barlow, 1976). A second advantage is that the reduced number of integration points decreases CPU time and storage requirements. The disadvantage is that the reduced integration procedure can admit deformation modes that cause no straining at the integration points. These zero-energy modes make the element rank-deficient and cause a phenomenon called “hourglassing,” where the zero energy mode starts propagating through the mesh, leading to inaccurate solutions. This problem is particularly severe in first-order quadrilaterals and hexahedra. To prevent these excessive deformations, an additional artificial stiffness is added to the element. In this so-called hourglass control procedure, a small artificial stiffness is associated with the zero-energy deformation modes. This procedure is used in many of the solid and shell elements in Abaqus.

Most fully integrated solid elements are unsuitable for the analysis of (approximately) incompressible material behavior. The reason for this is that the material behavior forces the material to deform (approximately) without volume changes. Fully integrated solid element meshes, and in particular lower-order element meshes, do not allow such deformations (other than purely homogeneous deformation). For that reason Abaqus uses “selectively reduced” integration in these elements: reduced integration is used for the volume strain and full integration for the deviatoric strains. As a consequence the lower-order elements give an acceptable performance for approximately incompressible behavior. For fully incompressible material behavior, another complication occurs: the bulk modulus and, hence, the stiffness matrix becomes infinitely large. For this case a mixed (hybrid) formulation is required, where the displacement field is augmented with a hydrostatic pressure field. In this formulation only the inverse of the bulk modulus appears, and, consequently, the contribution to the operator matrix vanishes. The hydrostatic pressure field plays the role of a Lagrange multiplier field enforcing the incompressibility constraints.

Abaqus/Standard also provides elements for multifield problems. Examples are the pore pressure elements used for the analysis of porous solids with fluid diffusion, coupled temperature-displacement elements that couple heat transfer with stress analysis, and piezoelectric elements that couple electrical conduction with stress analysis. In these multifield elements the scalar variable (such as the temperature) is usually interpolated with different scalar functions as the displacement field; i.e.,

T (g, h) = M^{N} (g, h) T^{N},

where $M^{N} (g, h)$ may differ from $N^{N} (g, h)$ . The coupling of the fields will generally occur at the integration points; for example, in coupled temperature-displacement elements the coupling is due to temperature-dependent mechanical properties and heat generation is due to inelastic work. Finally, Abaqus offers a complete set of diffusion elements to analyze conductive and convective heat transfer. In these elements only temperatures appear as nodal degrees of freedom. The temperatures are interpolated with essentially the same interpolation function, $M^{N} (g, h)$ , as used in the coupled temperature-displacement elements.