Explicit
2-D Structural Solid
PLANE162 Element Description
PLANE162 is used for modeling 2-D solid structures in ANSYS LS-DYNA. The element can be used either as a planer or as an axisymmetric element. The element is defined by four nodes having six degrees of freedom at each node: translations, velocities, and accelerations in the nodal x and y directions. A three-node triangle option is also available, but not recommended.
The element is used in explicit dynamic analyses only. When using this element, the model must only contain PLANE162 elements - you cannot mix 2-D and 3-D explicit elements in the same model. Furthermore, all PLANE162 elements in the model must be the same type (plane stress, plane strain, or axisymmetric). Refer to the LS-DYNA Theoretical Manual for more information.
PLANE162 Input Data
The geometry, node locations, and coordinate system for this element are shown in Figure 162.1: PLANE162 Geometry. Use KEYOPT(3) to specify whether the element is a plane stress, plane strain, or axisymmetric element. For the axisymmetric option (KEYOPT(3) = 1), you may also use KEYOPT(2) to specify either area or volume weighted axisymmetric elements.
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.
Use the EDLOAD command to apply nodal loads and other types of loads described below. For detailed information on how to apply loads in an explicit dynamic analysis, see Loading in the ANSYS LS-DYNA User's Guide. Note that when the axisymmetric option (KEYOPT(3) = 1) is selected and KEYOPT(2) = 0 (area weighted option), nodal loads should be input per unit length of circumference. Likewise, when KEYOPT(3) = 1 and KEYOPT(2) = 1 (volume weighted option), nodal loads should be input per radian. Other aspects of axisymmetric elements are covered in Harmonic Axisymmetric Elements. Pressures are always on a 360° basis, irrespective of the KEYOPT(2) setting.
Pressures can be input as surface loads on the element faces (edges) as shown by the circled numbers in Figure 162.1: PLANE162 Geometry. Positive normal pressures act into the element.
Other loads that can be applied using the EDLOAD command include base accelerations and angular velocities in the x and y directions, and displacements and forces 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.
The material models available to use with this element will depend on the KEYOPT(3) setting. KEYOPT(3) controls whether the element is a plane stress, plane strain, or axisymmetric element. For all three of these options (KEYOPT(3) = 0, 1, or 2), you can choose the following materials:
Isotropic Elastic
Orthotropic Elastic
Elastic Fluid
Viscoelastic
Bilinear Isotropic
Temperature Dependent Bilinear Isotropic
Bilinear Kinematic
Plastic Kinematic
Power Law Plasticity
Rate Sensitive Power Law Plasticity
Strain Rate Dependent Plasticity
Piecewise Linear Plasticity
Composite Damage
Johnson-Cook Plasticity
Bamman
For the plane stress option (KEYOPT(3) = 0), you can also choose the following materials:
3-Parameter Barlat Plasticity
Barlat Anisotropic Plasticity
Transversely Anisotropic Elastic Plastic
Transversely Anisotropic FLD
For the axisymmetric and plane strain options (KEYOPT(3) = 1 or 2), you can also choose the following materials:
Blatz-Ko Rubber
Mooney-Rivlin Rubber
Elastic-Plastic Hydrodynamic
Closed Cell Foam
Low Density Foam
Crushable Foam
Honeycomb
Null
Zerilli-Armstrong
Steinberg
PLANE162 Input Summary
- Nodes
I, J, K, L
- Degrees of Freedom
UX, UY, VX, VY, AX, AY
Note: For explicit dynamic analyses, V(X, Y) refers to nodal velocity, and A(X, Y) refers to nodal acceleration. Although V(X, Y) and A(X, Y) 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, PRXY or NUXY, ALPX (or CTEX or THSX), DENS, GXY, ALPD, BETD, DMPR EDMP command: RIGID, HGLS, ORTHO, FLUID - Surface Loads
- Pressures --
face 1 (J-I), face 2 (K-J), face 3 (L-K), face 4 (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(2)
Weighting option (used for axisymmetric elements, KEYOPT(3) = 1):
- 0 --
Area weighted axisymmetric element
- 1 --
Volume weighted axisymmetric element
- KEYOPT(3)
Element behavior:
- 0 --
Plane stress
- 1 --
Axisymmetric
- 2 --
Plane strain (Z strain = 0.0)
- KEYOPT(5)
Element continuum treatment:
- 0 --
Lagrangian (default)
- 1 --
ALE (Arbitrary Lagrangian-Eulerian)
PLANE162 Output Data
The solution output associated with the element is in two forms:
Nodal displacements included in the overall nodal solution
Additional element output as shown in Table 162.1: PLANE162 Element Output Definitions
Several items are illustrated in Figure 162.2: PLANE162 Stress Output. The element stresses are output in terms of the global Cartesian coordinate system by default. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.
You can rotate stress results for PLANE162 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 162.1: PLANE162 Element Output Definitions
| Name | Definition |
|---|---|
| S(X, Y, XY) | Stresses |
| S(1, 2, 3) | Principal stresses |
| SINT | Stress intensity |
| SEQV | Equivalent stress |
| EPTO(X, Y, XY) | Total strains |
| EPTO(1, 2, 3) | Total principal strains |
| EPTO(INT) | Total strain intensity |
| EPTO(EQV) | Total equivalent strain |
| EPEL(X, Y, XY) | 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. Some components of stress and strain (for example, yz and zx components) are always zero. 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).
Table 162.2: PLANE162 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 162.2: PLANE162 Item and Sequence Numbers:
- Name
output quantity
- Item
predetermined Item label for ETABLE command
- E
sequence number for single-valued or constant element data
PLANE162 Assumptions and Restrictions
The area of the element must be nonzero.
The element must lie in the global X-Y plane as shown in Figure 162.1: PLANE162 Geometry, and the Y-axis must be the axis of symmetry for axisymmetric analyses.
An axisymmetric structure should be modeled in the +X quadrants.
A triangular element may be formed by defining duplicate K and L node numbers (see Degenerated Shape Elements).