The solid element library includes isoparametric elements: quadrilaterals in two dimensions and “bricks” (hexahedra) in three dimensions. These isoparametric elements are generally preferred for most cases because they are usually the more cost-effective of the elements that are provided in Abaqus. They are offered with first- and second-order interpolation and are described in detail in Solid isoparametric quadrilaterals and hexahedra. For practical reasons it is sometimes not possible to use isoparametric elements throughout a model; for example, some commercial mesh generators use automatic meshing techniques that rely on triangulation to fill arbitrarily shaped regions. Because of these needs Abaqus includes triangular, tetrahedron, and wedge elements. For most cases it is recommended that these elements be only used to fill in awkward parts of the mesh and, in particular, that well-shaped isoparametric elements be used in any critical region (such as an area where the strain must be predicted accurately). The isoparametric elements can also be degenerated to make simpler shapes. Generally the elements written for those particular geometries are preferred to this method. The exception to this rule occurs in cases where singularities are to be modeled (such as in fracture mechanics applications), since the degenerate second-order isoparametric elements can provide a singularity through the use of the “quarter point” technique (placing the midside nodes 1/4 of the distance along the side from the node at the singularity instead of at the middle point of the side). Solid elements are provided with first-order (linear) and second-order (quadratic) interpolation, and the user must decide which approach is more appropriate for the application. Some guidelines are as follows. Standard first-order elements are essentially constant strain elements: the isoparametric forms can provide more than constant strain response, but the higher-order content of the solutions they give is generally not accurate and, thus, of little value. The “incompatible mode” elements, described in Continuum elements with incompatible modes, are from the user's perspective lower-order elements but have internal degrees of freedom that enable the element to represent almost all linear strain patterns. These elements can represent certain important linear strain fields exactly: the most important field is the one due to bending. The second-order elements are capable of representing all possible linear strain fields. Thus, in the case of elliptic problems—problems for which the governing partial differential equations are elliptic in character, such as elasticity, heat conduction, acoustics, in which smoothness of the solution is assured—much higher solution accuracy per degree of freedom is usually available with the higher-order elements. Therefore, it is generally recommended that the highest-order elements available be used for such cases: in Abaqus this means second-order elements. This observation logically leads to the use of the “hierarchical” finite element technique or “p”-method—refining the model by increasing the interpolation order in the elements in critical regions: this approach is as yet not available in Abaqus. A case where both incompatible mode elements and second-order elements can be used effectively is the stress analysis of relatively thin members subjected to bending: such problems are often encountered in practical applications. In such cases the strain variation through the thickness must be at least linear, and constant strain (first-order) elements do a poor job of representing this variation. Fully integrated first-order isoparametric elements also suffer from “shear locking” in these geometries: they cannot provide the pure bending solution because they must shear at the numerical integration points to respond with an appropriate kinematic behavior corresponding to the bending. This shearing then locks the element—the response is far too stiff. For the isoparametric elements reduced integration provides a cure for these problems, but at the cost of allowing spurious singular modes (“hourglassing”). The use of second-order elements is a more reliable alternative, because the second-order interpolation naturally contains the linear strain field—one element through the thickness is enough to represent the behavior of a thin component subjected to bending loads quite accurately. Another alternative is formed by the incompatible mode elements: the linear strain field in these elements contains the modes required to solve the bending problem exactly if the elements are rectangular in shape. For a detailed discussion of the performance of Abaqus continuum elements in bending problems, see Performance of continuum and shell elements for linear analysis of bending problems. (It should be remembered, however, that Abaqus offers shell and beam elements that are specifically written for thin geometries: the use of solid elements for such cases should only be considered when beam or shell elements are not practical.) For all of these reasons the second-order elements are preferred in elliptic applications. The argument is readily extended to higher-order interpolation (cubic, quartic, etc), but the rapid increase in cost per element for higher-order forms means that—even though the accuracy per degree of freedom is higher—the accuracy per computational cost may not be increasing. Practical experience suggests that—except in special cases—little is gained by going beyond the second-order elements, so Abaqus does not offer any higher-order forms. Many problems of practical interest are not elliptic: localizations arise in one form or another. Plasticity applications are an example—as the solution approaches the limit load, most plasticity models tend toward hyperbolic behavior. This allows discontinuities to occur in the solution—the slip line solutions of classical perfect plasticity theory are plots of the characteristic lines of velocity discontinuities in the hyperbolic equations of the problem. If the finite element solution is to exhibit accuracy, these discontinuities in the gradient field of the solution should be reasonably well modeled. With a fixed mesh that does not use special elements that admit discontinuities in their formulation, this suggests that the lowest-order elements—the first-order elements—are likely to be the most successful, because, for a given number of nodes, they provide the most locations at which some component of the gradient of the solution can be discontinuous (the element edges). This argument is hardly rigorous, but it is, nevertheless, true that first-order elements tend to be preferred for such cases. The incompatible mode elements can represent discontinuities particularly well. They are also able to represent strain localization such as occurs in shear bands. One should realize, however, that better defined shear localization increases the strain magnitude and, hence, tends to increase the number of increments and iterations required for the analysis. All of the solid elements in Abaqus, except the infinite elements, are written to include finite-strain effects. When these elements are used with a hyperelastic (elastomeric) material definition, the constitutive behavior is calculated directly from the deformation gradient matrix, . When the elements are used for geometrically nonlinear analysis with any other material definition (at finite strain this means the material has some inelastic behavior, since all of the elasticity definitions in Abaqus except the hyperelasticity models assume that the elastic strains are small), the strains are calculated as the integral of the rate of deformation, with the effects of material rotation with respect to the coordinate system taken into consideration. In all cases the solid elements report stress as the “true” (Cauchy) stress. Unless a local orientation is specified for an element, stress and strain components are given as physical components referred to the global spatial directions. When a local orientation is defined for a solid element, the stress and strain components are given in the user-defined local system: this system rotates with the average material rotation calculated at each material point. | |||||||||||