김경종
32 KiB
28.1.1 SOLID (CONTINUUM) ELEMENTS
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
References
• “Choosing the element’s dimensionality,” Section 27.1.2
• “One-dimensional solid (link) element library,” Section 28.1.2
• “Two-dimensional solid element library,” Section 28.1.3
• “Three-dimensional solid element library,” Section 28.1.4
• “Cylindrical solid element library,” Section 28.1.5
• “Axisymmetric solid element library,” Section 28.1.6
• “Axisymmetric solid elements with nonlinear, asymmetric deformation,” Section 28.1.7
• *SOLID SECTION
• *HOURGLASS STIFFNESS
• “Creating homogeneous solid sections,” Section 12.13.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Creating composite solid sections,” Section 12.13.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Creating electromagnetic solid sections,” Section 12.13.5 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• “Assigning a material orientation” in “Assigning a material orientation or rebar reference orientation,” Section 12.15.4 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Guide
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 (see “Choosing the appropriate element for an analysis type,” Section 27.1.3).
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. See “Choosing the element’s dimensionality,” Section 27.1.2, for details.
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 (see “Solid isoparametric quadrilaterals and hexahedra,” Section 3.2.4 of the Abaqus Theory Guide, 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.
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. 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.
Hourglassing
Hourglassing can be a problem with first-order, reduced-integration elements (CPS4R, CAX4R, C3D8R, etc.) 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.
In Abaqus/Standard the second-order reduced-integration elements, with the exception of the 27-node C3D27R and C3D27RH elements, do not have the same difficulty and are recommended in all cases when the solution is expected to be smooth. The C3D27R and C3D27RH elements have three
unconstrained, propagating hourglass modes when all 27 nodes are present. These elements should not be used with all 27 nodes, unless they are sufficiently constrained through boundary conditions. First-order elements are recommended when large strains or very high strain gradients are expected.
Shear and volumetric locking
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 (CPS4, CPE4, C3D8, etc.) 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. See “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Guide, for further discussion of the bending behavior of solid elements.
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.
Specifying nondefault section controls
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,” Section 27.1.4, 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 temperaturedisplacement 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,” Section 27.1.4, for more information about hourglass control.
Input File Usage: Use both of the following options to associate a section control definition with the element section definition:
*SECTION CONTROLS, NAME=name
*SOLID SECTION, CONTROLS=name
Use both of the following options in Abaqus/Standard to specify nondefault hourglass stiffness factors for the total stiffness approach:
*SOLID SECTION
*HOURGLASS STIFFNESS
Abaqus/CAE Usage: Mesh module:
Element Type: Element Controls
Element Type: Hourglass stiffness: Specify
Choosing between bricks/quadrilaterals and tetrahedra/triangles
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,” Section 2.3.5 of the Abaqus Benchmarks Guide).
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.
Tetrahedral and wedge elements
For stress/displacement analyses the first-order tetrahedral element C3D4 is a constant stress tetrahedron, which should be avoided as much as possible; the element exhibits slow convergence with mesh refinement. This element provides accurate results only in general cases with very fine meshing. Therefore, C3D4 is recommended only for filling in regions of low stress gradient in meshes of C3D8 or C3D8R elements, when the geometry precludes the use of C3D8 or C3D8R elements throughout the model. For tetrahedral element meshes the second-order or the modified tetrahedral elements, C3D10 or C3D10M, should be used.
Similarly, the linear version of the wedge element C3D6 should generally be used only when necessary to complete a mesh, and, even then, the element should be far from any areas where accurate results are needed. This element provides accurate results only with very fine meshing.
Modified triangular and tetrahedral elements
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” in “Common difficulties associated with contact modeling in Abaqus/Standard,” Section 39.1.2, 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,” Section 1.1.11 of the Abaqus Benchmarks Guide, and “Upsetting of a cylindrical billet: coupled temperature-displacement and adiabatic analysis,” Section 1.3.16 of the Abaqus Example Problems Guide). 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,” Section 2.1.2 of the Abaqus Benchmarks Guide
• “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Guide
• “LE1: Plane stress elements—elliptic membrane,” Section 4.2.1 of the Abaqus Benchmarks Guide
• “LE10: Thick plate under pressure,” Section 4.2.10 of the Abaqus Benchmarks Guide
• “FV32: Cantilevered tapered membrane,” Section 4.4.7 of the Abaqus Benchmarks Guide
• “FV52: Simply supported “solid” square plate,” Section 4.4.10 of the Abaqus Benchmarks Guide
However, in analyses involving thin bending situations with finite deformations (see “Pressurized rubber disc,” Section 1.1.7 of the Abaqus Benchmarks Guide) and in frequency analyses where high bending modes need to be captured accurately (see “FV41: Free cylinder: axisymmetric vibration,” Section 4.4.8 of the Abaqus Benchmarks Guide), 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 secondorder 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.
Compatibility with other elements
The modified triangular and tetrahedral elements are incompatible with the regular second-order solid elements in Abaqus/Standard. Thus, they should not be connected with these elements in a mesh.
Surface stress output
In areas of high stress gradients, stresses extrapolated from the integration points to the nodes are not as accurate for the modified elements as for similar second-order triangles and tetrahedra in Abaqus/Standard. In cases where more accurate surface stresses are needed, the surface can be coated with membrane elements that have a significantly lower stiffness than the underlying material. The stresses in these membrane elements will then reflect more accurately the surface stress and can be used for output purposes.
Fully constrained displacements
In Abaqus/Standard if all the displacement degrees of freedom on all the nodes of a modified element are constrained with boundary conditions, a similar boundary condition is applied to an internal node in the element. If a distributed load is subsequently applied to this element, the reported reaction forces at the nodes you defined will not sum up to the applied load since some of the applied load is taken by the internal node whose reaction force is not reported.
Choosing between regular and hybrid elements
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.
Almost incompressible material behavior
Near-incompressible behavior occurs when the bulk modulus is very much larger than the shear modulus (for example, in linear elastic materials where the Poisson’s ratio is greater than .48) and exhibits behavior approaching the incompressible limit: a very small change in displacement produces
extremely large changes in pressure. Therefore, a purely displacement-based solution is too sensitive to be useful numerically (for example, computer round-off may cause the method to fail).
This singular behavior is removed from the system by treating the pressure stress as an independently interpolated basic solution variable, coupled to the displacement solution through the constitutive theory and the compatibility condition. This independent interpolation of pressure stress is the basis of the hybrid elements. Hybrid elements have more internal variables than their nonhybrid counterparts and are slightly more expensive. See “Hybrid incompressible solid element formulation,” Section 3.2.3 of the Abaqus Theory Guide, for further details.
Fully incompressible material behavior
Hybrid elements must be used if the material is fully incompressible (except in the case of plane stress since the incompressibility constraint can be satisfied by adjusting the thickness). If the material is almost incompressible and hyperelastic, hybrid elements are still recommended. For almost incompressible, elastic-plastic materials and for compressible materials, hybrid elements offer insufficient advantage and, hence, should not be used.
For Mises and Hill plasticity the plastic deformation is fully incompressible; therefore, the rate of total deformation becomes incompressible as the plastic deformation starts to dominate the response. All of the quadrilateral and brick elements in Abaqus/Standard can handle this rate-incompressibility condition except for the fully integrated quadrilateral and brick elements without the hybrid formulation: CPE8, CPEG8, CAX8, CGAX8, and C3D20. These elements will “lock” (become overconstrained) as the material becomes more incompressible.
Elastic strains in hybrid elements
Hybrid elements use an independent interpolation for the hydrostatic pressure, and the elastic volumetric strain is calculated from the pressure. Hence, the elastic strains agree exactly with the stress, but they agree with the total strain only in an element average sense and not pointwise, even if no inelastic strains are present. For isotropic materials this behavior is noticeable only in second-order, fully integrated hybrid elements. In these elements the hydrostatic pressure (and, thus, the volumetric strain) varies linearly over the element, whereas the total strain may exhibit a quadratic variation.
For anisotropic materials this behavior also occurs in first-order, fully integrated hybrid elements. In such materials there is typically a strong coupling between volumetric and deviatoric behavior: volumetric strain will give rise to deviatoric stresses and, conversely, deviatoric strains will give rise to hydrostatic pressure. Hence, the constant hydrostatic pressure enforced in the fully integrated, first-order hybrid elements does not generally yield a constant elastic strain; whereas the total volume strain is always constant for these elements, as discussed earlier in this section. Therefore, hybrid elements are not recommended for use with anisotropic materials unless the material is approximately incompressible, which usually implies that the coupling between deviatoric and volume behavior is relatively weak.
Using hybrid elements with material models that exhibit volumetric plasticity
If the material model exhibits volumetric plasticity, such as the (capped) Drucker-Prager model, slow convergence or convergence problems may occur if second-order hybrid elements are used. In that case good results can usually be obtained with regular (nonhybrid) second-order elements.
Determining the need for hybrid elements
For nearly incompressible materials a displaced shape plot that shows a more or less homogeneous but nonphysical pattern of deformation is an indication of mesh locking. As previously discussed, fully integrated elements should be changed to reduced-integration elements in this case. If reduced-integration elements are already being used, the mesh density should be increased. Finally, hybrid elements can be used if problems persist.
Hybrid triangular and tetrahedral elements
The following hybrid, triangular, two-dimensional and axisymmetric elements should be used only for mesh refinement or to fill in regions of meshes of quadrilateral elements: CPE3H, CPEG3H, CAX3H, and CGAX3H. Hybrid, three-dimensional tetrahedral elements C3D4H and prism elements C3D6H should be used only for mesh refinement or to fill in regions of meshes of brick-type elements. Since each C3D6H element introduces a constraint equation in a fully incompressible problem, a mesh containing only these elements will be overconstrained. Abutting regions of C3D4H elements with different material properties should be tied rather than sharing nodes to allow discontinuity jumps in the pressure and volumetric fields.
In addition, the second-order three-dimensional hybrid elements C3D10H, C3D10MH, C3D15H, and C3D15VH are significantly more expensive than their nonhybrid counterparts.
Multi-purpose, improved surface stress visualization tetrahedra
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.
Improved surface stress visualization bricks
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
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 secondorder 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,” Section 3.2.5 of the Abaqus Theory Guide.
Shape considerations
The incompatible mode elements perform almost as well as second-order elements in many situations if the elements have an approximately rectangular shape. The performance is reduced considerably if the elements have a parallelogram shape. The performance of trapezoidal-shaped incompatible mode elements is not much better than the performance of the regular, fully integrated, first-order interpolation elements; see “Performance of continuum and shell elements for linear analysis of bending problems,” Section 2.3.5 of the Abaqus Benchmarks Guide, which illustrates the loss of accuracy associated with distorted elements.
Using incompatible mode elements in large-strain applications
Incompatible mode elements should be used with caution in applications involving large compressive strains. Convergence may be slow at times, and inaccuracies may accumulate in hyperelastic applications. Hence, erroneous residual stresses may sometimes appear in hyperelastic elements that are unloaded after having been subjected to a complex deformation history.
Using incompatible mode elements with regular elements
Incompatible mode elements can be used in the same mesh with regular solid elements. Generally the incompatible mode elements should be used in regions where bending response must be modeled accurately, and they should be of rectangular shape to provide the most accuracy. While these elements