Solid (continuum) 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 (see Solid isoparametric quadrilaterals and hexahedra for a more detailed discussion).

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.

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. For example, element type C3D20 has 27 integration points, while C3D20R has only 8; therefore, element assembly is roughly 3.5 times more costly for C3D20 than for C3D20R.

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.

You can specify a nondefault hourglass control formulation or scale factor for reduced-integration first-order elements (4-node quadrilaterals and 8-node bricks with one integration point). See Section controls for more information about section controls.

In Abaqus/Explicit section controls can also be used to specify a nondefault kinematic formulation for 8-node brick elements, the accuracy order of the element formulation, and distortion control for either 4-node quadrilateral or 8-node brick elements. Section controls are also used with coupled temperature-displacement elements in Abaqus/Explicit to change the default values for the mechanical response analysis.

In Abaqus/Standard you can specify nondefault hourglass stiffness factors based on the default total stiffness approach for reduced-integration first-order elements (4-node quadrilaterals and 8-node bricks with one integration point) and modified tetrahedral and triangular elements.

There are no hourglass stiffness factors or scale factors for the nondefault enhanced hourglass control formulation. See Section controls for more information about hourglass control.

SECTION CONTROLS, NAME=name
SOLID SECTION, CONTROLS=name

SOLID SECTION
HOURGLASS STIFFNESS

Mesh module: 
Element Type: Element Controls
Element Type: Hourglass stiffness: Specify

Triangular and tetrahedral elements are geometrically versatile and are used in many automatic meshing algorithms. It is very convenient to mesh a complex shape with triangles or tetrahedra, and the second-order and modified triangular and tetrahedral elements (CPE6, CPE6M, C3D10, C3D10M, etc.) in Abaqus are suitable for general usage. However, a good mesh of hexahedral elements usually provides a solution of equivalent accuracy at less cost. Quadrilaterals and hexahedra have a better convergence rate than triangles and tetrahedra, and sensitivity to mesh orientation in regular meshes is not an issue. However, triangles and tetrahedra are less sensitive to initial element shape, whereas first-order quadrilaterals and hexahedra perform better if their shape is approximately rectangular. The elements become much less accurate when they are initially distorted (see Performance of continuum and shell elements for linear analysis of bending problems).

First-order triangles and tetrahedra are usually overly stiff, and extremely fine meshes are required to obtain accurate results. As mentioned earlier, fully integrated first-order triangles and tetrahedra in Abaqus/Standard also exhibit volumetric locking in incompressible problems. As a rule, these elements should not be used except as filler elements in noncritical areas. Therefore, try to use well-shaped elements in regions of interest.

A family of modified 6-node triangular and 10-node tetrahedral elements is available that provides improved performance over the first-order triangular and tetrahedral elements and that occasionally provides improved behavior to regular second-order triangular and tetrahedral elements. In Abaqus/Explicit these modified triangular and tetrahedral elements are the only 6-node triangular and 10-node tetrahedral elements available. Regular second-order triangular and tetrahedral elements are typically preferable in Abaqus/Standard; however, regular second-order triangular and tetrahedral elements may exhibit “volumetric locking” when incompressibility is approached, such as in problems with a large amount of plastic deformation. As discussed in Three-dimensional surfaces with second-order faces and a node-to-surface formulation, regular second-order tetrahedral elements cannot underly a slave surface for the node-to-surface contact formulation with strict enforcement of a “hard” contact relationship. This limitation is typically not significant because the surface-to-surface contact formulation and penalty contact enforcement are generally recommended.

Modified triangular and tetrahedral elements work well in contact, exhibit minimal shear and volumetric locking, and are robust during finite deformation (see The Hertz contact problem and Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis). These elements use a lumped matrix formulation for dynamic analysis. Modified triangular elements are provided for planar and axisymmetric analysis, and modified tetrahedra are provided for three-dimensional analysis. In addition, hybrid versions of these elements are provided in Abaqus/Standard for use with incompressible and nearly incompressible constitutive models.

When the total stiffness approach is chosen, modified tetrahedral and triangular elements (C3D10M, CPS6M, CAX6M, etc.) use hourglass control associated with their internal degrees of freedom. The hourglass modes in these elements do not usually propagate; hence, the hourglass stiffness is usually not as significant as for first-order elements.

For most Abaqus/Standard analysis models the same mesh density appropriate for the regular second-order triangular and tetrahedral elements can be used with the modified elements to achieve similar accuracy. For comparative results, see the following:

• Geometrically nonlinear analysis of a cantilever beam

• Performance of continuum and shell elements for linear analysis of bending problems

• LE1: Plane stress elements—elliptic membrane

• LE10: Thick plate under pressure

• FV32: Cantilevered tapered membrane

• FV52: Simply supported “solid” square plate

However, in analyses involving thin bending situations with finite deformations (see Pressurized rubber disc) and in frequency analyses where high bending modes need to be captured accurately (see FV41: Free cylinder: axisymmetric vibration), the mesh has to be more refined for the modified triangular and tetrahedral elements (by at least one and a half times) to attain accuracy comparable to the regular second-order elements.

The modified triangular and tetrahedral elements might not be adequate to be used in the coupled pore fluid diffusion and stress analysis in the presence of large pore pressure fields if enhanced hourglass control is used.

The modified elements are more expensive computationally than lower-order quadrilaterals and hexahedron and sometimes require a more refined mesh for the same level of accuracy. However, in Abaqus/Explicit they are provided as an attractive alternative to the lower-order triangles and tetrahedron to take advantage of automatic triangular and tetrahedral mesh generators.

Hybrid elements are intended primarily for use with incompressible and almost incompressible material behavior; these elements are available only in Abaqus/Standard. When the material response is incompressible, the solution to a problem cannot be obtained in terms of the displacement history only, since a purely hydrostatic pressure can be added without changing the displacements.

The C3D10HS tetrahedron has been developed for improved bending results in coarse meshes while avoiding pressure locking in metal plasticity and quasi-incompressible and incompressible rubber elasticity. These elements are available only in Abaqus/Standard. Internal pressure degrees of freedom are activated automatically for a given element once the material exhibits behavior approaching the incompressible limit (i.e., an effective Poisson's ratio above .45). This unique feature of C3D10HS elements make it especially suitable for modeling metal plasticity, since it activates the pressure degrees of freedom only in the regions of the model where the material is incompressible. Once the internal degrees of freedom are activated, C3D10HS elements have more internal variables than either hybrid or nonhybrid elements and, thus, are more expensive. This element also uses a unique 11-point integration scheme, providing a superior stress visualization scheme in coarse meshes as it avoids errors due to the extrapolation of stress components from the integration points to the nodes.

The C3D8S and C3D8HS linear brick elements have been developed to provide a superior stress visualization on the element surface by avoiding errors due to the extrapolation of stress components from the integration points to the nodes. These elements are available only in Abaqus/Standard. The C3D8S and C3D8HS elements have the same degrees of freedom and use the same element linear interpolation as C3D8 and C3D8H, respectively. These elements use a 27-point integration scheme consisting of 8 integration points at the elements' nodes, 12 integration points on the elements' edges, 6 integration points on the elements' sides, and one integration point inside the element. To reduce the size of the output database, you can request element output at the nodes. Because these elements have integration points at the nodes, there is no error associated with extrapolating integration point output variables to the nodes.

Incompatible mode elements (CPS4I, CPE4I, CAX4I, CPEG4I, and C3D8I and the corresponding hybrid elements) are first-order elements that are enhanced by incompatible modes to improve their bending behavior; all of these elements are available in Abaqus/Standard and only element C3D8I is available in Abaqus/Explicit.

In addition to the standard displacement degrees of freedom, incompatible deformation modes are added internally to the elements. The primary effect of these modes is to eliminate the parasitic shear stresses that cause the response of the regular first-order displacement elements to be too stiff in bending. In addition, these modes eliminate the artificial stiffening due to Poisson's effect in bending (which is manifested in regular displacement elements by a linear variation of the stress perpendicular to the bending direction). In the nonhybrid elements—except for the plane stress element, CPS4I—additional incompatible modes are added to prevent locking of the elements with approximately incompressible material behavior. For fully incompressible material behavior the corresponding hybrid elements must be used.

Because of the added internal degrees of freedom due to the incompatible modes (4 for CPS4I; 5 for CPE4I, CAX4I, and CPEG4I; and 13 for C3D8I), these elements are somewhat more expensive than the regular first-order displacement elements; however, they are significantly more economical than second-order elements. The incompatible mode elements use full integration and, thus, have no hourglass modes.

Incompatible mode elements are discussed in more detail in Continuum elements with incompatible modes.

Continuum solid shell elements (CSS8) are first-order elements with seven incompatible modes to improve bending behavior and an assumed strain to mitigate locking. The formulation is based on work by Vu-Quoc and Tan (2003). The CSS8 elements are well suited for thin structural applications, including composites, where you want a full three-dimensional constitutive response. They fill a gap between incompatible mode elements, which use three-dimensional constitutive laws but tend to lock in bending for large aspect ratios, and continuum shell elements, which have a very good bending response for large aspect ratios but are restricted to two-dimensional plane stress constitutive behaviors. The continuum solid shell elements are available only in Abaqus/Standard.

Continuum solid shell elements have only displacement degrees of freedom and are fully compatible with regular continuum elements. They use full integration and have no hourglass modes. The assumed strain leads to a through-thickness response that is different from the in-plane response; therefore, while these elements pass in-plane membrane and out-of-plane bending patch tests, they do not pass the standard three-dimensional patch test.

Normal definition for continuum solid shell elements

Figure 1 illustrates a key modeling feature of continuum solid shell elements. Since the behavior in the thickness direction is different from that in the in-plane directions, it is important that the continuum solid shell elements are oriented properly. The element top and bottom faces (and, hence, the element normal, stacking direction, and thickness) are defined by the nodal connectivity. For continuum solid shell element CSS8 the face with corner nodes 1, 2, 3, and 4 is the bottom face, and the face with corner nodes 5, 6, 7, and 8 is the top face. The stacking direction and thickness direction are both defined to be the direction from the bottom to the top face. The thickness direction and the stacking direction should always be in the third direction of the element's isoparametric directions.

Figure 1. Normal and thickness direction for continuum solid shell elements.

Variable node elements (such as C3D27 and C3D15V) allow midface nodes to be introduced on any element face (on any rectangular face only for the triangular prism C3D15V). The choice is made by the nodes specified in the element definition. These elements are available only in Abaqus/Standard and can be used quite generally in any three-dimensional model. The C3D27 family of elements is frequently used as the ring of elements around a crack line.

Cylindrical elements (CCL9, CCL9H, CCL12, CCL12H, CCL18, CCL18H, CCL24, CCL24H, and CCL24RH) are available only in Abaqus/Standard for precise modeling of regions in a structure with circular geometry, such as a tire. The elements make use of trigonometric functions to interpolate displacements along the circumferential direction and use regular isoparametric interpolation in the radial or cross-sectional plane of the element. All the elements use three nodes along the circumferential direction and can span angles between 0 and 180°. Elements with both first-order and second-order interpolation in the cross-sectional plane are available.

The geometry of the element is defined by specifying nodal coordinates in a global Cartesian system. The default nodal output is also provided in a global Cartesian system. Output of stress, strain, and other material point output quantities are done, by default, in a fixed local cylindrical system where direction 1 is the radial direction, direction 2 is the axial direction, and direction 3 is the circumferential direction. This default system is computed from the reference configuration of the element. An alternative local system can be defined (see Orientations). In this case the output of stress, strain, and other material point quantities is done in the oriented system.

The cylindrical elements can be used in the same mesh with regular elements. In particular, regular solid elements can be connected directly to the nodes on the cross-sectional plane of cylindrical elements. For example, any face of a C3D8 element can share nodes with the cross-sectional faces (faces 1 and 2; see Cylindrical solid element library for a description of the element faces) of a CCL12 element. Regular elements can also be connected along the circular edges of cylindrical elements by using a surface-based tie constraint (Mesh tie constraints) provided that the cylindrical elements do not span a large segment. However, such usage may result in spurious oscillations in the solution near the tied surfaces and should be avoided when an accurate solution in this region is required.

Compatible membrane elements (Membrane elements) and surface elements with rebar (Surface elements) are available for use with cylindrical solid elements.

All elements with first-order interpolation in the cross-sectional plane use full integration for the deviatoric terms and reduced integration for the volumetric terms and, thus, have no hourglass modes and do not lock with almost incompressible materials. The hybrid elements with first-order and second-order interpolation in the cross-sectional plane use an independent interpolation for hydrostatic pressure.

The following recommendations apply to both Abaqus/Standard and Abaqus/Explicit:

• Make all elements as “well shaped” as possible to improve convergence and accuracy.

• If an automatic tetrahedral mesh generator is used, use the second-order elements C3D10 (in Abaqus/Standard) or C3D10M (in Abaqus/Explicit). Use the modified tetrahedral element C3D10M in Abaqus/Standard in analyses with large amounts of plastic deformation.

• If possible, use hexahedral elements in three-dimensional analyses since they give the best results for the minimum cost.

Abaqus/Standard users should also consider the following recommendations:

• For linear and “smooth” nonlinear problems use reduced-integration, second-order elements if possible.

• Use second-order, fully integrated elements close to stress concentrations to capture the severe gradients in these regions. However, avoid these elements in regions of finite strain if the material response is nearly incompressible.

• Use first-order quadrilateral or hexahedral elements or the modified triangular and tetrahedral elements for problems involving large distortions. If the mesh distortion is severe, use reduced-integration, first-order elements.

• If the problem involves bending and large distortions, use a fine mesh of first-order, reduced-integration elements.

• Hybrid elements must be used if the material is fully incompressible (except when using plane stress elements). Hybrid elements should also be used in some cases with nearly incompressible materials.

• Incompatible mode elements can give very accurate results in problems dominated by bending.