2.1. Solid and Shell Elements

2.1.1. SOLID164

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

2.1.2. SHELL163

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.

2.1.2.1. General Shell Formulations

  • 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.

2.1.2.2. Membrane Element Formulation

  • 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

2.1.2.3. Triangular Shell Formulations

  • 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.

Figure 2.1:  Integration Points

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 points0.5774
Outermost Point3 points0.7746
 4 points0.8611
 5 points0.9062
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.


2.1.3. PLANE162

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

2.1.4. SOLID168

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.


Release 18.2 - © ANSYS, Inc. All rights reserved.