The SOLID164 element is an 8-node brick element. By default, it uses reduced (one point) integration plus viscous hourglass control for faster element formulation. One point integration is advantageous due to savings on computer time and robustness in cases of large deformations. A fully integrated solid formulation (KEYOPT(1) = 2) is also available; see the element description for SOLID164 in the Element Referenceand Section 3.3 of the LS-DYNA Theoretical Manual. If hourglass phenomenon is a concern, such as with foams, the fully integrated formulation may perform better because hourglass control is not required; but it is about four times more costly in terms of CPU time.
KEYOPT(5) defines the element continuum treatment. Two different formulations are available: Lagrangian (default) and Arbitrary Lagrangian-Eulerian (ALE). See Arbitrary Lagrangian-Eulerian Formulation in the ANSYS LS-DYNA User's Guide for more information.
Wedge, pyramid, and tetrahedra shaped SOLID164 elements are simply degenerate bricks (i.e., some of the nodes are repeated). These shapes are often too stiff in bending and cause problems in some situations. Therefore, these degenerate shapes should be avoided. If a tetrahedron mesh is desired, it is recommended that SOLID168 elements be used instead of degenerated SOLID164 elements.
You can use any of the following material models for solid elements:
Isotropic Elastic
Orthotropic Elastic
Anisotropic Elastic
Bilinear Kinematic
Plastic Kinematic
Viscoelastic
Blatz-Ko Rubber
Bilinear Isotropic
Power Law Plasticity
Strain Rate Dependent Plasticity
Composite Damage
Concrete Damage
Geological Cap
Piecewise Linear Plasticity
Honeycomb
Mooney-Rivlin Rubber
Barlat Anisotropic Plasticity
Elastic-Plastic Hydrodynamic
Rate Sensitive Powerlaw Plasticity
Elastic Viscoplastic Thermal
Closed Cell Foam
Low Density Foam
Viscous Foam
Crushable Foam
Johnson-Cook Plasticity
Null
Zerilli-Armstrong
Bamman
Steinberg
Elastic Fluid
Twelve different formulations are available for the SHELL163 element. Use KEYOPT(1) to specify the desired formulation. As with solid elements, the number of integration points per element directly impacts CPU time. Therefore, for general analyses, the reduced integration shell formulations are recommended. The following is an outline of the different formulations available for SHELL163. Coordinate systems for output of quantities associated with SHELL163 may vary for different formulations. See the Element Reference for more information.
Belytschko-Tsay (KEYOPT(1) = 0 or 2) - default
Very fast and is recommended for most applications
Uses reduced integration (one point)
Should not be used when elements experience excessive warping
Belytschko-Wong-Chiang (KEYOPT(1) = 10)
25% slower than Belytschko-Tsay
Uses reduced integration (one point)
Generally gives correct results for warping
Belytschko-Leviathan (KEYOPT(1) = 8)
40% slower than Belytschko-Tsay
Reduced integration formulation (one point)
Includes physical hourglass control automatically
Fully integrated Belytschko-Tsay (KEYOPT(1) = 12)
2.5 times slower than reduced integration Belytschko-Tsay shell.
Has four integration points in plane and does not need hourglass control.
Shear locking is remedied by assumed strain for the transverse shear.
Recommended if hourglass modes are a problem in the analysis.
Hughes-Liu (KEYOPT(1) = 1, 6, 7, 11) = > four different formulations which can offset the mid-plane of element away from the nodes.
KEYOPT(1) = 1 General Hughes-Liu. Has one-point integration and is 2.5 times slower that Belytschko-Tsay.
KEYOPT(1) = 11 Fast (corotational) Hughes-Liu. Has one-point integration and is 1.5 times slower than Belytschko-Tsay.
KEYOPT(1) = 6 S/R Hughes-Liu. Has four integration points with no hourglassing but is 20 times slower that Belytschko-Tsay.
KEYOPT(1) = 7 S/R corotational Hughes-Liu. Has four integration points with no hourglassing. 8.8 times slower than Belytschko-Tsay. Recommended if hourglassing is a problem in an analysis.
Belytschko-Tsay Membrane (KEYOPT(1) = 5)
Fast and recommended for most membrane applications
Reduced (one-point) integration
Good for fabrics where wrinkling is a concern (i.e., where large in-plane compressive stresses try to collapse the thin fabric elements)
Fully integrated Belytschko-Tsay Membrane (KEYOPT(1) = 9)
Significantly slower than general membrane (KEYOPT(1) = 5)
Four integration points in plane
No hourglassing
C0 triangular shell (KEYOPT(1) = 4)
Based on Mindlin-Reissner Plate Theory
Formulation is rather stiff, so not recommended for entire mesh
Reduced integration formulation
BCIZ Triangular Shell (KEYOPT(1) = 3)
Based on Kirchhoff Plate Theory
Slower than C0 triangular shells
Reduced integration formulation
The description of SHELL163 in the ANSYS LS-DYNA User's Guide also has a complete list of available shell formulations.
Degenerate quadrilateral shell elements are prone to lock under transverse
shear; therefore, C0 triangular shell elements (based
on work by Belytschko and coworkers) have been implemented. Triangular shells
can be mixed with quadrilateral shells within the same material property set,
provided that the element sorting flag (the ITRST
field on the EDSHELL command) is set to 1 (which is the
default).
You can use any of the following material models for shell elements:
Isotropic Elastic
Orthotropic Elastic
Bilinear Kinematic
Plastic Kinematic
Blatz-Ko Rubber
Bilinear Isotropic
Power Law Plasticity
Strain Rate Dependent Plasticity
Composite Damage
Piecewise Linear Plasticity
Modified Piecewise Linear Plasticity
Mooney-Rivlin Rubber (see note below)
Barlat Anisotropic Plasticity
3 Parameter Barlat Plasticity
Transversely Anisotropic Elastic Plastic
Rate Sensitive Powerlaw Plasticity
Transversely Anisotropic FLD
Elastic Viscoplastic Thermal
Johnson-Cook Plasticity
Bamman
Note: When the Mooney-Rivlin Rubber material model is used with SHELL163 elements, the LS-DYNA code will automatically use a total Lagrangian modification of the Belytschko-Tsay formulation instead of using the formulation you specify via KEYOPT(1). This program-chosen formulation is required to address the special needs of the hyperelastic material.
All shell element formulations can have an arbitrary number of integration points through the thickness. Typically, 2 integration points (default) are required through the thickness for elastic behavior, while 3 or more integration points are required for plastic behavior. The number of integration points through the thickness is controlled using the second real constant:
R,NSET,,R2 where R2 = number of integration points (NIP)
3-D plane stress constitutive subroutines are implemented for the shell elements; these update the stress tensor such that the stress component normal to the shell mid surface is zero. The integration points are stacked vertically at the centroid of the element, as shown in Figure 2.1: Integration Points.
Through-thickness directions at each node are initially normal to the element surface but rotate with the nodes. The through-the-thickness integration is needed to calculate bending moments and in-plane forces. The distribution of strain is always linear; whereas the stress is more complicated in nature and depends on the material law.
Two integration points are sufficient for linear elastic materials, while more points are required for nonlinear materials. Stress output is given at the outermost integration points, not at the surfaces (despite the nomenclature of postprocessors, which refer to top and bottom surfaces), so care is needed in interpretation of results. For elastic materials, stresses can be extrapolated to the surfaces. For nonlinear materials the usual procedure is to choose four or five integration points through the thickness and to ignore the inaccuracy (i.e., the difference in stress between the surface and the outermost integration point). The locations of the outermost integration points of Gauss quadrature are given in the following table:
| Mid Plane | 0 | |
| 2 points | 0.5774 | |
| Outermost Point | 3 points | 0.7746 |
| 4 points | 0.8611 | |
| 5 points | 0.9062 | |
| Outer Surface | 1.0000 |
Note: Keep in mind that this integration could be made exactly beforehand when linear elastic material is used, but it is not done in ANSYS LS-DYNA because nonlinear behavior is generally being modeled.
Also, for elements using full integration, the output stress is the averaged stress values from the 2x2 integration points of the same layer.
The PLANE162 element is a 2-D, 4-node solid element that can be used either as a planar (X-Y plane) or as an axisymmetric (Y-axis of symmetry) element. KEYOPT(3) allows you to specify a plane stress, axisymmetric, or plane strain option for the element. For the axisymmetric element formulation, you can specify either an area or volume weighted option using KEYOPT(2).
KEYOPT(5) defines the element continuum treatment. Two different formulations are available: Lagrangian (default) and Arbitrary Lagrangian-Eulerian (ALE). See Arbitrary Lagrangian-Eulerian Formulation in the ANSYS LS-DYNA User's Guide for more information.
The PLANE162 element is typically defined by four-nodes. A three-node triangle option is also available, but not recommended because it is often too stiff. There are no real constants for this element. It is important to note that models containing PLANE162 elements must consist only of this element type. ANSYS LS-DYNA does not allow a mixed 2-D and 3-D finite element model. Furthermore, all PLANE162 elements in the model must be the same type (plane stress, plane strain, or axisymmetric).
The material models available to use with this element will depend on the KEYOPT(3) setting. For KEYOPT(3) = 0, 1, or 2 (plane stress, plane strain, or axisymmetric), you can choose the following materials:
Isotropic Elastic
Orthotropic Elastic
Elastic Fluid
Viscoelastic
Bilinear Isotropic
Temperature Dependent Bilinear Isotropic
Bilinear Kinematic
Plastic Kinematic
Power Law Plasticity
Rate Sensitive Powerlaw Plasticity
Strain Rate Dependent Plasticity
Piecewise Linear Plasticity
Composite Damage
Johnson-Cook Plasticity
Bamman
For the plane stress option (KEYOPT(3) = 0), you can also choose the following materials:
3-Parameter Barlat Plasticity
Barlat Anisotropic Plasticity
Transversely Anisotropic Elastic Plastic
Transversely Anisotropic FLD
For the axisymmetric and plane strain options (KEYOPT(3) = 1 or 2), you can also choose the following materials:
Blatz-Ko Rubber
Mooney-Rivlin Rubber
Elastic-Plastic Hydrodynamic
Closed Cell Foam
Low Density Foam
Crushable Foam
Honeycomb
Null
Zerilli-Armstrong
Steinberg
The SOLID168 element is a 10-node tetrahedron element. It uses either a quadratic displacement interpolation with five point integration (KEYOPT(1) = 0 or 1) or a composite assemblages of sub-tetrahedral shapes (KEYOPT(1) = 2); see the element description for SOLID168 in the Element Reference.
You can use any of the following material models for solid elements:
Isotropic Elastic
Isotropic Elastic
Orthotropic Elastic
Anisotropic Elastic
Bilinear Kinematic
Plastic Kinematic
Viscoelastic
Blatz-Ko Rubber
Bilinear Isotropic
Power Law Plasticity
Strain Rate Dependent Plasticity
Composite Damage
Concrete Damage
Geological Cap
Piecewise Linear Plasticity
Honeycomb
Mooney-Rivlin Rubber
Barlat Anisotropic Plasticity
Elastic-Plastic Hydrodynamic
Rate Sensitive Power Law Plasticity
Elastic Viscoplastic Thermal
Closed Cell Foam
Low Density Foam
Viscous Foam
Crushable Foam
Johnson-Cook Plasticity
Null
Zerilli-Armstrong
Bamman
Steinberg
Elastic Fluid
SOLID168 elements are well suited to modeling irregular meshes such as those produced from various CAD/CAM systems and the ANSYS Workbench. It is important to note, however, that models made up entirely of SOLID168 elements may not be as accurate as hexahedral (SOLID164) models. For this reason, we recommend using a combination of SOLID168 and SOLID164 elements within a model as a good modeling practice. The SOLID168 elements could be used for the irregular portions of the model while the SOLID164 elements could be used to mesh the more uniform features.
Although SOLID164 and SOLID168 elements can be used in the same model, you must be careful to develop an adequate mesh transition between these two element types. This is due to the fact that SOLID168 elements conatin mid-side nodes, which are not allowed in SOLID164 elements.