PLANE183

2-D 8-Node or 6-Node Structural Solid

Compatible Products: DesSpc | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

## PLANE183 Element Description

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 eight nodes or six nodes. It can be used as a plane element (plane stress, plane strain and generalized plane strain) or as an axisymmetric element (with or without torsion). In most cases, the element has two degrees of freedom at each node: translations in the nodal x and y directions. For the axisymmetric with torsion option, however, the element has three degrees of freedom at each node: translations in the nodal x and y directions and rotation in the nodal y direction.

The 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 state is supported. Various printout options are also available. See PLANE183 for more details about this element.

Figure 183.1:  PLANE183 Geometry ## PLANE183 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 183.1: PLANE183 Geometry.

Although a degenerated triangular-shaped element may be formed by defining the same node number for nodes K, L and O when KEYOPT(1) = 1, it is better to use KEYOPT(1) = 1 for triangular shaped elements. 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 described in Coordinate Systems.

Element loads are described in Nodal Loading. 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. The input torque (if any) for an axisymmetric analysis with torsion is on a full 360° basis.

KEYOPT(3) = 5 enables generalized plane strain. (Surface output is suppressed.) For more information about the generalized plane strain option, see Generalized Plane Strain.

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 .

For extra surface output, KEYOPT(17) = 4 activates surface solution for faces with nonzero pressure. For more information, see Surface Solution.

You can apply an initial stress state to this element via the INISTATE command. For more information, see Initial State in the Mechanical APDL Advanced Analysis Guide.

As described in Coordinate Systems, you can use ESYS to orient the material properties and stress/strain output. Use ESYS to select output that follows the material coordinate system or the global coordinate system.

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 Harmonic Axisymmetric Elements.

### PLANE183 Input Summary

Nodes

I, J, K, L, M, N, O, P when KEYOPT(1) = 0

I, J, K, L, M, N when KEYOPT(1) = 1)

Degrees of Freedom

UX, UY (KEYOPT(3) ≠ 6)

UX, UY and ROTY (KEYOPT(3) = 6)

Real Constants
 None, if KEYOPT (3) = 0, 1, or 2 THK - Thickness if KEYOPT (3) = 3
Material Properties
 TB command: See Element Support for Material Models for this element. MP command: 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, ALPD, BETD, DMPR
Pressures --

face 1 (J-I), face 2 (K-J), face 3 (L-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

Temperatures --

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

Body force densities --

The element values in the global X and Y directions.

Special Features
 Birth and death Coriolis effect Element technology autoselect Fracture parameter calculation Initial state Large deflection Large strain Linear perturbation Material force evaluation Nonlinear adaptivity Nonlinear stabilization Rezoning Stress stiffening
KEYOPT(1)

Element shape:

0 --

1 --

6-node triangle

KEYOPT(3)

Element behavior:

0 --

Plane stress

1 --

Axisymmetric

2 --

Plane strain (Z strain = 0.0)

3 --

Plane stress with thickness (TK) real constant input

5 --

Generalized plane strain (surface output suppressed)

6 --

Axisymmetric with torsion

KEYOPT(6)

Element formulation:

0 --

Use pure displacement formulation (default)

1 --

Use mixed u-P formulation (not valid with plane stress)

KEYOPT(17)

Extra surface output:

0 --

Basic element solution (default)

4 --

Surface solution for faces with nonzero pressure

## PLANE183 Output Data

The solution output associated with the element is in two forms:

Several items are illustrated in Figure 183.2: PLANE183 Stress Output.

The element stress directions are parallel to the element coordinate system. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 183.2:  PLANE183 Stress Output The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that 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 “-” indicates that the item is not available.

Table 183.1:  PLANE183 Element Output Definitions

NameDefinitionOR
ELElement number-Y
NODESNodes - I, J, K, L (for KEYOPT(1) = 0 and I, J, K (for KEYOPT(1) = 1)-Y
MATMaterial number-Y
THICKThickness-Y
VOLU:Volume-Y
XC, YCLocation where results are reportedY4
PRESPressures 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)

(T(L) only when KEYOPT(1) = 0)

-Y
S:X, Y, Z, XY Stresses (SZ = 0.0 for plane stress elements)YY
S:1, 2, 3Principal stresses-Y
S: INTStress intensity-Y
S:EQVEquivalent stress-Y
EPEL:X, Y, Z, XY Elastic strainsYY
EPEL:EQVEquivalent elastic strain -Y
EPTH:X, Y, Z, XY Thermal strains33
EPTH:EQVEquivalent thermal strain -3
EPPL:X, Y, Z, XY Plastic strains11
EPPL:EQVEquivalent plastic strain -1
EPCR:X, Y, Z, XY Creep strains22
EPCR:EQVEquivalent creep strains 22
EPTO:X, Y, Z, XY Total mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)Y-
NL:SEPLPlastic yield stress11
NL:EPEQAccumulated equivalent plastic strain11
NL:CREQAccumulated equivalent creep strain11
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding)11
NL:PLWKPlastic work/volume11
NL:HPRESHydrostatic pressure11
SEND:ELASTIC, PLASTIC, CREEP, ENTOStrain energy densities-1
LOCI:X, Y, ZIntegration point locations-5
SVAR:1, 2, ... , NState variables-6
YSIDX:TENS,SHEAYield surface activity status for Mohr-Coloumb, soil, concrete, and joint rock material models: 1 for yielded and 0 for not yielded. -Y
FPIDX: TF01,SF01, TF02,SF02, TF03,SF03, TF04,SF04Failure plane surface activity status for concrete and joint rock material models: 1 for yielded and 0 for not yielded. Tension and shear failure status are available for all four sets of failure planes.-Y

1. Nonlinear solution, output only if the element has a nonlinear material, or if large-deflection effects are enabled (NLGEOM,ON) for SEND.

2. Output only if element has a creep load.

3. Output only if element has a thermal load.

4. Available only at centroid as a *GET item.

5. Available only if OUTRES,LOCI is used.

6. Available only if the `UserMat` subroutine and TB,STATE command are used.

7. 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.

8. For the shape memory alloy material model, transformation strains are reported as plasticity strain EPPL.

9. YZ and XZ when used with the axisymmetric with torsion option.

### Axisymmetric Solution Without Torsion

In a global coordinate system, the X, Y, Z, and XY stress and strain outputs correspond to the radial, axial, hoop, and in-plane shear stresses and strains, respectively.

### Axisymmetric Solution With Torsion

Stress/strain outputs have six components with the same meanings as the 3-D solid element outputs. The results are on the 2-D plane even when the applied torque or rotation causes the plane to be twisted after large deformation. The plane is both the modeling plane and the result plane, so it represents both the initial configuration and the deformed configuration. (Think of it as the plane cut by the global Cartesian XOY plane through the deformed 3-D body, or as the Eulerian plane in finite deformation.)

To better understand the solution results, you can plot them in 3-D space (/ESHAPE,1) when PowerGraphics is enabled (/GRAPHICS,POWER). The results are plotted in either the global coordinate system (RSYS,0) or the solution coordinate system (RSYS,SOLU). Support is not available for increasing the number of planar facets per element edge (/EFACET).

When the output is on the 2-D plane, you can think of the solution in terms of the axisymmetric option without torsion by imagining the global Cartesian X and Y as radial and axial directions, and global Cartesian Z as the reverse of the hoop direction.

### PLANE183 Item and Sequence Numbers

Table 183.2: PLANE183 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 183.2: PLANE183 Item and Sequence Numbers:

Name

output quantity as defined in Table 183.1: PLANE183 Element Output Definitions

Item

predetermined Item label for ETABLE

E

sequence number for single-valued or constant element data

I,J,...,P

sequence number for data at nodes I, J, ..., P

Table 183.2:  PLANE183 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJKLMNOP
P1SMISC-21------
P2SMISC--43-----
P3SMISC---65----
P4SMISC-7--8----
THICKNMISC1--------

1. P4 is only for KEYOPT(1) = 0

See Surface Solution for the item and sequence numbers for surface output (KEYOPT(17) = 4) for the ETABLE command

## PLANE183 Assumptions and Restrictions

• 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) 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 Degenerated Shape 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 the sparse solver (default).

• Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). Prestress effects can be activated by the PSTRES command.

• The axisymmetric with torsion option (KEYOPT(3) = 6) can be used only with surface element SURF153 with KEYOPT(3) = 1. When used with contact elements, the friction in the global Cartesian Z (hoop direction) is not taken into account. Rezoning and nonlinear adaptivity are not supported.

## PLANE183 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro

• Birth and death is not available.

• Fracture parameter calculation is not available.

• Initial state is not available.

• Linear perturbation is not available.

• Material force evaluation is not available.

• Rezoning is not available.