Release 11.0 Documentation for ANSYS
www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS
PLANE183
2-D 8-Node or 6-Node Structural Solid
MP ME ST PR PRN DS DSS <> <> <> <> PP VT
PLANE183 is a higher order 2-D, 8-node or 6-node element. PLANE183 has quadratic displacement behavior and is well suited to modeling irregular meshes (such as those produced by various CAD/CAM systems).
This element is defined by 8 nodes or 6-nodes having two degrees of freedom at each node: translations in the nodal x and y directions. The element may be used as a plane element (plane stress, plane strain and generalized plane strain) or as an axisymmetric element. This element has plasticity, hyperelasticity, creep, stress stiffening, large deflection, and large strain capabilities. It also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. Initial stress import is supported. Various printout options are also available. See PLANE183 in the Theory Reference for ANSYS and ANSYS Workbench for more details about this element.
The geometry, node locations, and the coordinate system for this element are shown in Figure 183.1: "PLANE183 Geometry".
For KEYOPT(1) = 0, a degenerated triangular-shaped element may be formed by defining the same node number for nodes K, L and O. In addition to the nodes, the element input data includes a thickness (TK) (for the plane stress option only) and the orthotropic material properties. Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Coordinate Systems.
Element loads are described in Node and Element Loads. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 183.1: "PLANE183 Geometry". Positive pressures act into the element. Temperatures may be input as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). If all corner node temperatures are specified, each midside node temperature defaults to the average temperature of its adjacent corner nodes. For any other input temperature pattern, unspecified temperatures default to TUNIF.
The nodal forces, if any, should be input per unit of depth for a plane analysis (except for KEYOPT(3) = 3 or KEYOPT(3) = 5) and on a full 360° basis for an axisymmetric analysis.
As described in Coordinate Systems, you can use ESYS to orient the material properties and strain/stress output. Use ESYS to choose output that follows the material coordinate system or the global coordinate system. For the case of hyperelastic materials, the output of stress and strain is always with respect to the global Cartesian coordinate system rather than following the material/element coordinate system.
KEYOPT(3) = 5 is used to enable generalized plane strain. For more information about the generalized plane strain option, see Generalized Plane Strain Option of 18x Solid Elements in the Elements Reference.
KEYOPT(6) = 1 sets the element for using mixed formulation. For details on the use of mixed formulation, see Applications of Mixed u-P Formulations in the Elements Reference.
You can apply an initial stress state to this element via the INISTATE command. For more information, see the INISTATE command, and also Initial Stress Loading in the Basic Analysis Guide. Alternately, you can set KEYOPT(10) = 1 to read initial stresses from the user subroutine USTRESS. For details on user subroutines, see the Guide to ANSYS User Programmable Features.
The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.
The next table summarizes the element input. Element Input gives a general description of element input. For axisymmetric applications see Axisymmetric Elements.
I, J, K, L, M, N, O, P when KEYOPT(1) = 0
I, J, K, L, M, N when KEYOPT(1) = 1)
UX, UY
| None, if KEYOPT (3) = 0, 1, or 2 |
| THK - Thickness if KEYOPT (3) = 3 |
| EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), |
| ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), |
| DENS, GXY, GYZ, GXZ, DAMP |
face 1 (J-I), face 2 (K-J), face 3 (I-K), face 4 (I-L) when KEYOPT(1) = 0
face 1 (J-I), face 2 (K-J), face 3 (I-K) when KEYOPT(1) = 1
T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P) when KEYOPT(1) = 0
T(I), T(J), T(K), T(L), T(M), T(N) when KEYOPT(1) = 1
| Plasticity (PLASTIC, BISO, MISO, NLISO, BKIN, MKIN, KINH, CHABOCHE, HILL) |
| Hyperelasticity (AHYPER, HYPER) |
| Viscoelasticity (PRONY, SHIFT) |
| Viscoplasticity/Creep (CREEP, RATE) |
| Elasticity (ELASTIC, ANEL) |
| Other material (USER, SDAMP, SMA, CAST, EDP, GURSON) |
| Stress stiffening |
| Large deflection |
| Large strain |
| Initial stress import |
| Nonlinear stabilization |
| Manual rezoning |
| Automatic selection of element technology |
| Birth and death |
Items in parentheses refer to data tables associated with the TB command. CAST, EDP, SMA, and UNIAXIAL are not applicable for plane stress. See the Theory Reference for ANSYS and ANSYS Workbench for details of the material models.
See Automatic Selection of Element Technologies and ETCONTROL for more information on selection of element technologies.
Element shape:
8-node quadrilateral
6-node triangle
Element behavior:
Plane stress
Axisymmetric
Plane strain (Z strain = 0.0)
Plane stress with thickness (TK) real constant input
Generalized plane strain
Element formulation:
Use pure displacement formulation (default)
Use mixed u-P formulation (not valid with plane stress)
User-defined initial stress:
No user subroutine to provide initial stresses
Read initial stress data from user subroutine USTRESS
See the Guide to ANSYS User Programmable Features for user written subroutines
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 183.1: "PLANE183 Element Output Definitions".
Several items are illustrated in Figure 183.2: "PLANE183 Stress Output".
The element stress directions are parallel to the element coordinate system. Surface stresses are defined parallel and perpendicular to the IJ face (and the KL face) and along the Z-axis for a plane analysis or in the hoop direction for an axisymmetric analysis. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.
The Element Output Definitions table uses the following notation:
A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL]. The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.
In either the O or R columns, Y indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and a - indicates that the item is not available.
Table 183.1 PLANE183 Element Output Definitions
| Name | Definition | O | R |
|---|---|---|---|
| EL | Element number | - | Y |
| NODES | Nodes - I, J, K, L (for KEYOPT(1) = 0 and I, J, K (for KEYOPT(1) = 1) | - | Y |
| MAT | Material number | - | Y |
| THICK | Thickness | - | Y |
| VOLU: | Volume | - | Y |
| XC, YC | Location where results are reported | Y | 4 |
| PRES | Pressures P1 at nodes J, I; P2 at K, J; P3 at L, K; P4 at I, L (P4 only for KEYOPT(1) = 0 | - | Y |
| TEMP | Temperatures T(I), T(J), T(K), T(L) only for KEYOPT(1) = 0 | - | Y |
| S:X, Y, Z, XY | Stresses (SZ = 0.0 for plane stress elements) | Y | Y |
| S:1, 2, 3 | Principal stresses | - | Y |
| S: INT | Stress intensity | - | Y |
| S:EQV | Equivalent stress | - | Y |
| EPEL:X, Y, Z, XY | Elastic strains | Y | Y |
| EPEL:1, 2, 3 | Principal elastic strains | Y | - |
| EPEL:EQV | Equivalent elastic strain [7] | - | Y |
| EPTH:X, Y, Z, XY | Thermal strains | 3 | 3 |
| EPTH:EQV | Equivalent thermal strain [7] | - | 3 |
| EPPL:X, Y, Z, XY | Plastic strains[8] | 1 | 1 |
| EPPL:EQV | Equivalent plastic strain [7] | - | 1 |
| EPCR:X, Y, Z, XY | Creep strains | 2 | 2 |
| EPCR:EQV | Equivalent creep strains [7] | 2 | 2 |
| EPTO:X, Y, Z, XY | Total mechanical strains (EPEL + EPPL + EPCR) | Y | - |
| EPTO:EQV | Total equivalent mechanical strains (EPEL + EPPL + EPCR) | Y | - |
| NL:EPEQ | Accumulated equivalent plastic strain | 1 | 1 |
| NL:CREQ | Accumulated equivalent creep strain | 1 | 1 |
| NL:SRAT | Plastic yielding (1 = actively yielding, 0 = not yielding) | 1 | 1 |
| NL:PLWK | Plastic work | 1 | 1 |
| NL:HPRES | Hydrostatic pressure | 1 | 1 |
| SEND:ELASTIC, PLASTIC, CREEP | Strain energy densities | - | 1 |
| LOCI:X, Y, Z | Integration point locations | - | 5 |
| SVAR:1, 2, ... , N | State variables | - | 6 |
Nonlinear solution, output only if the element has a nonlinear material.
Available only at centroid as a *GET item.
Available only if OUTRES,LOCI is used.
Available only if the USERMAT subroutine and TB,STATE are used.
The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY); for plastic and creep this value is set at 0.5.
For the shape memory alloy material model, transformation strains are reported as plasticity strain EPPL.
For axisymmetric solutions, the X, Y, XY, and Z stress and strain outputs correspond to the radial, axial, in-plane shear, and hoop stresses and strains.
Table 183.2: "PLANE183 Item and Sequence Numbers" lists output available through ETABLE using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this manual for more information. The following notation is used in Table 183.2: "PLANE183 Item and Sequence Numbers":
output quantity as defined in Table 183.1: "PLANE183 Element Output Definitions"
predetermined Item label for ETABLE
sequence number for single-valued or constant element data
sequence number for data at nodes I, J, ..., P
Table 183.2 PLANE183 Item and Sequence Numbers
| Output Quantity Name | ETABLE and ESOL Command Input | |||||||||
|---|---|---|---|---|---|---|---|---|---|---|
| Item | E | I | J | K | L | M | N | O | P | |
| P1 | SMISC | - | 2 | 1 | - | - | - | - | - | - |
| P2 | SMISC | - | - | 4 | 3 | - | - | - | - | - |
| P3 | SMISC | - | - | - | 6 | 5 | - | - | - | - |
| P4[1] | SMISC | - | 7 | - | - | 8 | - | - | - | - |
| THICK | NMISC | 1 | - | - | - | - | - | - | - | - |
See Surface Solution in this manual for the item and sequence numbers for surface output for ETABLE.
The area of the element must be positive.
The element must lie in a global X-Y plane as shown in Figure 183.1: "PLANE183 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 face with a removed midside node implies that the displacement varies linearly, rather than parabolically, along that face. See Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide for more information about the use of midside nodes.
Use at least two elements to avoid hourglass mode for KEYOPT(1) = 0.
A triangular element may be formed by defining duplicate K-L-O node numbers (see Triangle, Prism and Tetrahedral Elements). For these degenerated elements, the triangular shape function is used and the solution is the same as for the regular triangular 6-node elements, but might be slightly less efficient for KEYOPT(1) = 0. Since these degenerated elements are less efficient, the triangle shape option (KEYOPT(1) = 1) is suggested for this case.
When mixed formulation is used (KEYOPT(6) = 1), no midside nodes can be missed. If you use the mixed formulation (KEYOPT(6) = 1), you must use either the sparse solver (default) or the frontal solver.
Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). It is ignored in geometrically linear analyses (NLGEOM,OFF) when specified by SSTIF,ON. Prestress effects can be activated by the PSTRES command.
