2-D 4-Node Structural Solid

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

PLANE182 Element Description

PLANE182 is used to model 2-D solid structures. It can be used as either a plane element (plane stress, plane strain or generalized plane strain) or an axisymmetric element with or without torsion. In most cases, the element is defined by four nodes with two degrees of freedom at each node: translations in the nodal x and y directions. For the axisymmetric option with torsion, it is still defined by four nodes, but with 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, stress stiffening, large deflection, and large strain capabilities. It has a mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.

See PLANE182 for more details about this element.

Figure 182.1:  PLANE182 Geometry

PLANE182 Geometry

PLANE182 Input Data

The geometry and node locations for this element are shown in Figure 182.1: PLANE182 Geometry. The element input data includes four nodes, a thickness (for the plane stress option only), and the orthotropic material properties. The default element coordinate system is along global directions. You can define an element coordinate system (ESYS), which forms the basis for orthotropic material directions.

Element loads are described in Nodal Loading. Pressures can be input as surface loads on the element faces as shown by the circled numbers on Figure 182.1: PLANE182 Geometry. Positive pressures act into the element. Temperatures can 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). For any other input pattern, unspecified temperatures default to TUNIF.

Input the nodal forces (if any) 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 more information about 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 strain/stress output. Use RSYS 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.

"PLANE182 Input Summary" contains a summary of the element input. For a general description of element input, see Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

PLANE182 Input Summary


I, J, K, L

Degrees of Freedom

UX, UY (KEYOPT(3) ≠ 6)

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

Real Constants
THK - Thickness (used only if KEYOPT(3) = 3)
HGSTF - Hourglass stiffness scaling factor (used only if KEYOPT(1) = 1); default is 1.0 (if you input 0.0, the default value is used)
Material Properties
TB command: See Element Support for Material Models for this element.
Surface Loads
Pressures -- 

face 1 (J-I), face 2 (K-J), face 3 (L-K), face 4 (I-L)

Body Loads
Temperatures -- 

T(I), T(J), T(K), T(L)

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
Stress stiffening

Element technology:

0 -- 

Full integration with method

1 -- 

Uniform reduced integration with hourglass control

2 -- 

Enhanced strain formulation

3 -- 

Simplified enhanced strain formulation


Element behavior:

0 -- 

Plane stress

1 -- 


2 -- 

Plane strain (Z strain = 0.0)

3 -- 

Plane stress with thickness input

5 -- 

Generalized plane strain (surface output suppressed)

6 -- 

Axisymmetric with torsion (KEYOPT(1) = 0 only)


Element formulation:

0 -- 

Use pure displacement formulation (default)

1 -- 

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


Extra surface output:

0 -- 

Basic element solution (default)

4 -- 

Surface solution for faces with nonzero pressure

PLANE182 Element Technology

PLANE182 uses the full-integration B ¯ method (also known as the selective reduced integration method), enhanced strain formulation, simplified enhanced strain formulation, or uniform reduced integration. For the axisymmetric with torsion option (KEYOPT(3) = 6), only the full-integration method (KEYOPT(1) = 0) is available.

When enhanced strain formulation (KEYOPT(1) = 2) is selected, the element introduces four internal (user-inaccessible) degrees of freedom to handle shear locking, and one internal degree of freedom to handle volumetric locking.

For more information, see Element Technologies.

PLANE182 Output Data

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

Several items are illustrated in Figure 182.2: PLANE182 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 182.2:  PLANE182 Stress Output

PLANE182 Stress Output

Stress directions are shown for Global.

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 182.1:  PLANE182 Element Output Definitions

Name Definition O R
ELElement number-Y
NODES Nodes - I, J, K, L-Y
MATMaterial number-Y
XC, YCLocation where results are reportedY 3
PRESPressures P1 at nodes J,I; P2 at K,J; P3 at L,K; P4 at I,L-Y
TEMPTemperatures T(I), T(J), T(K), T(L)-Y
S:X, Y, Z, XY [8]Stresses (SZ = 0.0 for plane stress elements)YY
S:1, 2, 3Principal stresses-Y
S:INTStress intensity-Y
S:EQVEquivalent stressYY
EPEL:X, Y, Z, XY [8]Elastic strainsYY
EPEL:EQVEquivalent elastic strain [6]YY
EPTH:X, Y, Z, XY [8]Thermal strains 2 2
EPTH:EQVEquivalent thermal strain [6] 2 2
EPPL:X, Y, Z, XY [8]Plastic strains[7] 1 1
EPPL:EQVEquivalent plastic strain [6] 1 1
EPCR:X, Y, Z, XY [8]Creep strains 1 1
EPCR:EQVEquivalent creep strains [6] 1 1
EPTO:X, Y, Z, XY [8]Total mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)Y-
NL:SEPLPlastic yield stress 1 1
NL:EPEQAccumulated equivalent plastic strain 1 1
NL:CREQAccumulated equivalent plastic strain 1 1
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding) 1 1
NL:PLWKPlastic work/volume 1 1
NL:HPRESHydrostatic pressure 1 1
SEND:ELASTIC, PLASTIC, CREEP, ENTOStrain energy densities- 1
LOCI:X, Y, ZIntegration point locations- 4
SVAR:1, 2, ... , NState variables- 5
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 thermal load.

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

  4. Available only if OUTRES,LOCI is used.

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

  6. 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.

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

  8. 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).

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.

PLANE182 Item and Sequence Numbers

Table 182.2: PLANE182 Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Creating an Element Table and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 182.2: PLANE182 Item and Sequence Numbers:


output quantity as defined in the Table 182.1: PLANE182 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, K, L

Table 182.2:  PLANE182 Item and Sequence Numbers

Output Quantity Name ETABLE and ESOL Command Input

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

PLANE182 Assumptions and Restrictions

  • The area of the element must be nonzero.

  • The element must lie in a global X-Y plane as shown in Figure 182.1: PLANE182 Geometry and the Y-axis must be the axis of symmetry for axisymmetric analyses. An axisymmetric structure should be modeled in the +X quadrants.

  • You can form a triangular element by defining duplicate K and L node numbers. (See Degenerated Shape Elements.) For triangular elements where the or enhanced strain formulations are specified, degenerated shape functions and a conventional integration scheme are used.

  • If you use the mixed formulation (KEYOPT(6) = 1), you must use the sparse solver.

  • For modal cyclic symmetry analyses, ANSYS, Inc. recommends using enhanced strain formulation.

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

  • For the axisymmetric with torsion option (KEYOPT(3) = 6), only the full-integration method (KEYOPT(1) = 0) is available; however, it can be used with mixed u-P formulation (KEYOPT(6) =1). The option 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.

PLANE182 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.

ANSYS Mechanical Premium 

  • Birth and death is not available.

  • Fracture parameter calculation is not available.

  • Material force evaluation is not available.

  • Rezoning is not available.

Release 18.2 - © ANSYS, Inc. All rights reserved.