SOLID168 ## SOLID168 Element Description

## SOLID168 Input Data

### SOLID168 Input Summary

## SOLID168 Output Data

**Explicit
3-D 10-Node Tetrahedral Structural Solid**

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

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.

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

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

**Degrees of Freedom**UX, UY, UZ, VX, VY, VZ, AX, AY, AZ

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**None

**Material Properties****TB**command: See Element Support for Material Models for this element.**MP**command: EX, EY, EZ, NUXY, NUYZ, NUXZ,PRXY, PRXZ, PRYZ, ALPX (or CTEX *or*THSX),DENS, ALPD, BETD, DMPR **EDMP**command: RIGID, HGLS, ORTHO, FLUID**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.

**KEYOPT(1)**Element formulation:

**0, 1 --**Quadratic interpolation

**2 --**Composite (assemblages of linear tetrahedral shapes)

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**

Name | Definition |
---|---|

S:X, Y, Z, XY, YZ, XZ | Stresses |

S:1, 2, 3 | Principal stresses |

S:INT | Stress intensity |

S:EQV | Equivalent stress |

EPTO:X, Y, Z, XY, YZ, XZ | Total strains |

EPTO:1, 2, 3 | Total principal strains |

EPTO:INT | Total strain intensity |

EPTO:EQV | Total equivalent strain |

EPEL:X, Y, Z, XY, YZ, XZ | Elastic strains |

EPEL:1, 2, 3 | Principal elastic strains |

EPEL:INT | Elastic strain intensity |

EPEL:EQV | Equivalent elastic strains |

EPPL:EQV | Equivalent 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).