Explicit
3-D Structural Solid
SOLID164 Element Description
SOLID164 is used for the 3-D modeling of solid structures. The element is defined by eight nodes having the following degrees of freedom at each node: translations, velocities, and accelerations in the nodal x, y, and z directions.
This element is used in explicit dynamic analyses only. Refer to the LS-DYNA Theoretical Manual for more information.
SOLID164 Input Data
The geometry, node locations, and the coordinate system for this element are shown in Figure 164.1: SOLID164 Geometry. The element is defined by eight 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.
By default, SOLID164 uses reduced (one point) integration plus viscous hourglass control for faster element formulation. A fully integrated solid formulation (KEYOPT(1) = 2) is also available.
KEYOPT(5) defines the element continuum treatment. Two different formulations are available: Lagrangian (default) and Arbitrary Lagrangian-Eulerian (ALE). In addition to setting KEYOPT(5) = 1, you must also set appropriate parameters on the EDALE and EDGCALE commands in order for the ALE formulation to take affect. See Arbitrary Lagrangian-Eulerian Formulation in the ANSYS LS-DYNA User's Guide for more information. Some material models that are normally available for this element type are not supported when the ALE formulation is used. See the material list below for details.
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 164.1: SOLID164 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. The material models marked by an asterisk (*) are not supported by the ALE formulation (KEYOPT(5) = 1).
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
SOLID164 Input Summary
- Nodes
I, J, K, L, M, N, O, P
- 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. AlthoughV (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), GXY, GYZ, GXZ, DENS, ALPD, BETD, DMPR EDMP command: RIGID, HGLS, ORTHO, FLUID - Surface Loads
- Pressures --
face 1 (J-I-L-K), face 2 (I-J-N-M), face 3 (J-K-O-N), face 4 (K-L-P-O), face 5 (L-I-M-P), face 6 (M-N-O-P)
- 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 --
Constant stress solid element (default)
- 2 --
Fully integrated selectively-reduced solid
- KEYOPT(5)
Element continuum treatment:
- 0 --
Lagrangian (default)
- 1 --
ALE (Arbitrary Lagrangian-Eulerian)
SOLID164 Output Data
Output for SOLID164 is listed in Table 164.1: SOLID164 Element Output Definitions. If you issue PRNSOL, a single set of stress and a single set of strain values is output at all eight 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 SOLID164 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 164.1: SOLID164 Element Output Definitions
| Name | Definition |
|---|---|
| S(X, Y, Z, XY, YZ, XZ) | Stresses |
| S(1, 2, 3) | Principal stresses |
| SINT | Stress intensity |
| SEQV | 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 strain |
| EPPL(EQV) | Equivalent plastic strain |
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).
SOLID164 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 eight nodes.
A prism-shaped element may be formed by defining duplicate K and L and duplicate O and P node numbers (see Degenerated Shape Elements). A tetrahedron shape is also available. When the degenerated elements are used, be careful in choosing the element formulations. For the tetrahedron shape, SOLID168 should be considered instead.