Overview
Solid (continuum) elements:
- are the standard volume elements of Abaqus;
- do not include structural elements such as beams, shells, membranes, and trusses; special-purpose elements such as gap elements; or connector elements such as connectors, springs, and dashpots;
- can be composed of a single homogeneous material or, in Abaqus/Standard, can include several layers of different materials for the analysis of laminated composite solids; and
- are more accurate if not distorted, particularly for quadrilaterals and hexahedra. The triangular and tetrahedral elements are less sensitive to distortion.
Typical applications
The solid (or continuum) elements in Abaqus can be used for linear analysis and for complex nonlinear analyses involving contact, plasticity, and large deformations. They are available for stress, heat transfer, acoustic, coupled thermal-stress, coupled pore fluid-stress, piezoelectric, magnetostatic, electromagnetic, and coupled thermal-electrical analyses.
Choosing an appropriate element
There are some differences in the solid element libraries available in Abaqus/Standard and Abaqus/Explicit.
Abaqus/Standard solid element library
The Abaqus/Standard solid element library includes first-order (linear) interpolation elements and second-order (quadratic) interpolation elements in one, two, or three dimensions. Triangles and quadrilaterals are available in two dimensions; and tetrahedra, triangular prisms, and hexahedra (“bricks”) are provided in three dimensions. Modified second-order triangular and tetrahedral elements are also provided.
Curved (parabolic) edges can be used on the quadratic elements but are not recommended for pore pressure or coupled temperature-displacement elements. Cylindrical elements are provided for structures with edges that are initially circular.
In addition, reduced-integration, hybrid, and incompatible mode elements are available in Abaqus/Standard.
Electromagnetic elements, based on an edge-based interpolation of the magnetic vector potential, are provided both in two and three dimensions.
Abaqus/Explicit solid element library
The Abaqus/Explicit solid element library includes first-order (linear) interpolation elements and modified second-order interpolation elements in two or three dimensions. Triangular and quadrilateral first-order elements are available in two dimensions; and tetrahedral, triangular prism, and hexahedral (“brick”) first-order elements are available in three dimensions. The modified second-order elements are limited to triangles and tetrahedra. The acoustic elements in Abaqus/Explicit are limited to first-order (linear) interpolations. For incompatible mode elements only three-dimensional elements are available. Various two-dimensional models (plane stress, plane strain, axisymmetric) are available in both Abaqus/Standard and Abaqus/Explicit.
Given the wide variety of element types available, it is important to select the correct element for a particular application. Choosing an element for a particular analysis can be simplified by considering specific element characteristics: first- or second-order; full or reduced integration; hexahedra/quadrilaterals or tetrahedra/triangles; or normal, hybrid, or incompatible mode formulation. By considering each of these aspects carefully, the best element for a given analysis can be selected.
Choosing between first- and second-order elements
In first-order plane strain, generalized plane strain, axisymmetric quadrilateral, hexahedral solid elements, and cylindrical elements, the strain operator provides constant volumetric strain throughout the element. This constant strain prevents mesh “locking” when the material response is approximately incompressible.
Second-order elements provide higher accuracy in Abaqus/Standard than first-order elements for “smooth” problems that do not involve severe element distortions. They capture stress concentrations more effectively and are better for modeling geometric features: they can model a curved surface with fewer elements. Finally, second-order elements are very effective in bending-dominated problems.
First-order triangular and tetrahedral elements should be avoided as much as possible in stress analysis problems; the elements are overly stiff and exhibit slow convergence with mesh refinement, which is especially a problem with first-order tetrahedral elements. If they are required, an extremely fine mesh may be needed to obtain results of sufficient accuracy.
Choosing between full- and reduced-integration elements
Reduced integration uses a lower-order integration to form the element stiffness. The mass matrix and distributed loadings use full integration. Reduced integration reduces running time, especially in three dimensions. In Abaqus/Standard you can choose between full or reduced integration for quadrilateral and hexahedral (brick) elements. In Abaqus/Explicit you can choose between full or reduced integration for hexahedral (brick) elements. Only reduced-integration first-order elements are available for quadrilateral elements in Abaqus/Explicit; the elements with reduced integration are also referred to as uniform strain or centroid strain elements with hourglass control.
Second-order reduced-integration elements in Abaqus/Standard generally yield more accurate results than the corresponding fully integrated elements. However, for first-order elements the accuracy achieved with full versus reduced integration is largely dependent on the nature of the problem.
Hourglassing
Linear reduced-integration elements tend to be too flexible because they suffer from their own numerical problem called hourglassing. Consider a single reduced-integration element modeling a small piece of material subjected to pure bending as shown in figure a.
Figure a Deformation of a linear element with reduced integration subjected to bending moment M.
Hourglassing can be a problem with first-order, reduced-integration elements in stress/displacement analyses. Since the elements have only one integration point, it is possible for them to distort in such a way that the strains calculated at the integration point are all zero, which, in turn, leads to uncontrolled distortion of the mesh. First-order, reduced-integration elements in Abaqus include hourglass control, but they should be used with reasonably fine meshes. Hourglassing can also be minimized by distributing point loads and boundary conditions over a number of adjacent nodes.
Shear and volumetric locking
Shear locking causes the elements to be too stiff in bending. It is explained as follows. Consider a small piece of material in a structure subject to pure bending. The material will distort as shown in figure b
Figure b Deformation of material subjected to bending moment M.
Lines initially parallel to the horizontal axis take on constant curvature, and lines through the thickness remain straight. The angle between the horizontal and vertical lines remains at 90°.
The edges of a linear element are unable to curve; therefore, if the small piece of material is modeled using a single element, its deformed shape is like that shown in figure c
Figure c Deformation of a fully integrated, linear element subjected to bending moment M.
Shear locking only affects the performance of fully integrated, linear elements subjected to bending loads. These elements function perfectly well under direct or shear loads. Shear locking is not a problem for quadratic elements since their edges are able to curve (see figure d).
Figure d Deformation of a fully integrated, quadratic element subjected to bending moment M.
Fully integrated, linear elements should be used only when you are fairly certain that the loads will produce minimal bending in your model. Use a different element type if you have doubts about the type of deformation the loading will create. Fully integrated, quadratic elements can also lock under complex states of stress; thus, you should check the results carefully if they are used exclusively in your model. However, they are very useful for modeling areas where there are local stress concentrations.
Volumetric locking is another form of overconstraint that occurs in fully integrated elements when the material behavior is (almost) incompressible. It causes overly stiff behavior for deformations that should cause no volume changes.
Fully integrated elements in Abaqus/Standard and Abaqus/Explicit do not hourglass but may suffer from “locking” behavior: both shear and volumetric locking. Shear locking occurs in first-order, fully integrated elements that are subjected to bending. The numerical formulation of the elements gives rise to shear strains that do not really exist—the so-called parasitic shear. Therefore, these elements are too stiff in bending, in particular if the element length is of the same order of magnitude as or greater than the wall thickness.
Volumetric locking occurs in fully integrated elements when the material behavior is (almost) incompressible. Spurious pressure stresses develop at the integration points, causing an element to behave too stiffly for deformations that should cause no volume changes. If materials are almost incompressible (elastic-plastic materials for which the plastic strains are incompressible), second-order, fully integrated elements start to develop volumetric locking when the plastic strains are on the order of the elastic strains. However, the first-order, fully integrated quadrilaterals and hexahedra use selectively reduced integration (reduced integration on the volumetric terms). Therefore, these elements do not lock with almost incompressible materials. Reduced-integration, second-order elements develop volumetric locking for almost incompressible materials only after significant straining occurs. In this case, volumetric locking is often accompanied by a mode that looks like hourglassing. Frequently, this problem can be avoided by refining the mesh in regions of large plastic strain.
If volumetric locking is suspected, check the pressure stress at the integration points (printed output). If the pressure values show a checkerboard pattern, changing significantly from one integration point to the next, volumetric locking is occurring. Choosing a quilt-style contour plot in the Visualization module of Abaqus/CAE will show the effect.
👉 To know more about Solid (continuum) elemrnts, please refer to User Assistance.
📌 In the next blog we will demonstrate this concept. Stay tuned... ⏳
