Explicit
3-D 10-Node Tetrahedral Structural Solid
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.
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
- 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)
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
| 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).