Explicit 3-D 10-Node Tetrahedral Structural Solid

Compatible Products: – | – | – | – | – | – | DYNA

SOLID168 Element Description

SOLID168 is a higher order 3-D, 10-node explicit dynamic element. It is well suited to modeling irregular meshes such as those produced from various CAD/CAM systems. The element is defined by ten nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions.

By default, SOLID168 uses a quadratic displacement behavior with five point integration (KEYOPT(1) = 0 or 1). A composite formulation which is an assemblage of linear sub-tetrahedral shapes (KEYOPT(1) = 2) is also available. This second formulation effectively overcomes the difficulty of lumped mass calculations and volume locking inherent to the quadratic elements.

Figure 168.1:  SOLID168 Geometry

SOLID168 Geometry

SOLID168 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 168.1: SOLID168 Geometry. The element is defined by ten nodes. Orthotropic material properties may be defined. Use the EDMP command to specify an orthotropic material and the EDLCS command to define the orthotropic material directions.

Use the EDLOAD command to apply nodal loads and other load types described below. For detailed information on how to apply loads in an explicit dynamic analysis, see the ANSYS LS-DYNA User's Guide.

Pressures can be input as surface loads on the element faces as shown by the circled numbers in Figure 168.1: SOLID168 Geometry. Positive normal pressures act into the element.

Base accelerations and angular velocities in the x, y, and z directions can be applied at the nodes using the EDLOAD command. To apply these loads, you need to first select the nodes and create a component. The load is then applied to that component. You can also use the EDLOAD command to apply loads (displacements, forces, etc.) on rigid bodies.

Several types of temperature loading are also available for this element. See Temperature Loading in the ANSYS LS-DYNA User's Guide. For this element, you can choose from the materials listed below.

  • Isotropic Elastic

  • Orthotropic Elastic

  • Anisotropic Elastic

  • Bilinear Kinematic

  • Plastic Kinematic

  • Viscoelastic

  • Blatz-Ko Rubber

  • Bilinear Isotropic

  • Temperature Dependent 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 Input Summary


I, J, K, L, M, N, O, P, Q, R

Degrees of Freedom


For explicit dynamic analyses, V(X, Y, Z) refers to nodal velocity, and A(X, Y, Z) refers to nodal acceleration. Although V(X, Y, Z) and A(X, Y, Z) appear as DOFs, they are not actually physical DOFs. However, these quantities are computed as DOF solutions and stored for postprocessing.

Real Constants


Material Properties
TB command: See Element Support for Material Models for this element.
MP command: EX, EY, EZ, NUXY, NUYZ, NUXZ,
Surface Loads
Pressures -- 

face 1 (J-I-K), face 2 (I-J-L), face 3 (J-K-L), face 4 (K-I-L)

Body Loads
Temperatures -- 

See Temperature Loading in the ANSYS LS-DYNA User's Guide

Special Features

All nonlinear features allowed for an explicit dynamic analysis.


Element formulation:

0, 1  -- 

Quadratic interpolation

2  -- 

Composite (assemblages of linear tetrahedral shapes)

SOLID168 Output Data

Output for SOLID168 is listed in Table 168.1: SOLID168 Element Output Definitions. If you issue PRNSOL, a single set of stress and a single set of strain values is output at all ten nodes; that is, you will get the same sets of values at each node. If you issue PRESOL, you will get only a single set of values at the centroid.

You can rotate stress results for SOLID168 into a defined coordinate system using the RSYS command. However, RSYS cannot be used to rotate strain results for this element type.

The following items are available on the results file.

Table 168.1:  SOLID168 Element Output Definitions

S:X, Y, Z, XY, YZ, XZStresses
S:1, 2, 3Principal stresses
S:INTStress intensity
S:EQVEquivalent stress
EPTO:X, Y, Z, XY, YZ, XZTotal strains
EPTO:1, 2, 3Total principal strains
EPTO:INTTotal strain intensity
EPTO:EQVTotal equivalent strain
EPEL:X, Y, Z, XY, YZ, XZElastic strains
EPEL:1, 2, 3Principal elastic strains
EPEL:INTElastic strain intensity
EPEL:EQVEquivalent elastic strains
EPPL:EQVEquivalent plastic strains

Note:  Stress and total strain are always available. The availability of elastic strain and equivalent plastic strain depends on the material model used for the element (see Element Output Data in the ANSYS LS-DYNA User's Guide for details).

SOLID168 Assumptions and Restrictions

  • Zero volume elements are not allowed.

  • The element may not be twisted such that it has two separate volumes. This occurs most frequently when the element is not numbered properly.

  • The element must have ten nodes.

SOLID168 Product Restrictions

There are no product-specific restrictions for this element.

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