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.
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.
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.
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).
Temperature Dependent Bilinear Isotropic
Power Law Plasticity
Strain Rate Dependent Plasticity
Piecewise Linear Plasticity*
Barlat Anisotropic Plasticity
Rate Sensitive Power Law Plasticity
Elastic Viscoplastic Thermal
Closed Cell Foam*
Low Density Foam
I, J, K, L, M, N, O, P
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.
|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|
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)
All nonlinear features allowed for an explicit dynamic analysis.
Constant stress solid element (default)
Fully integrated selectively-reduced solid
Element continuum treatment:
ALE (Arbitrary Lagrangian-Eulerian)
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.
The following items are available on the results file.
Table 164.1: SOLID164 Element Output Definitions
|S(X, Y, Z, XY, YZ, XZ)||Stresses|
|S(1, 2, 3)||Principal stresses|
|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|
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.