Axisymmetric-Harmonic 8-Node Structural Solid

Compatible Products: – | – | – | Enterprise | Ent PP | Ent Solver | –

PLANE83 Element Description

Although this legacy element is available for use in your analysis, ANSYS, Inc. recommends using a current-technology element such as SOLID273 (KEYOPT(6) = 0), unless you are performing a linear analysis and require a sinusoidal load variation in the circumferential direction.

PLANE83 is used for 2-D modeling of axisymmetric structures with nonaxisymmetric loading. Examples of such loading are bending, shear, or torsion. The element has three degrees of freedom per node: translations in the nodal x, y, and z directions. For unrotated nodal coordinates, these directions correspond to the radial, axial, and tangential directions, respectively.

This element is a higher order version of the 2-D, four-node element (PLANE25). It provides more accurate results for mixed (quadrilateral-triangular) automatic meshes and can tolerate irregular shapes without as much loss of accuracy. The loading need not be axisymmetric. Various loading cases are described in Harmonic Axisymmetric Elements with Nonaxisymmetric Loads.

The 8-node elements have compatible displacement shapes and are well suited to model curved boundaries. See PLANE83 in the Mechanical APDL Theory Reference for more details about this element.

Figure 83.1:  PLANE83 Geometry

PLANE83 Geometry

PLANE83 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 83.1: PLANE83 Geometry. Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Coordinate Systems. Z-direction material properties (EZ, ALPZ, etc.) may be input. MODE and ISYM are used to describe the harmonic loading condition. (See Harmonic Axisymmetric Elements with Nonaxisymmetric Loads for more details.)

Element loads are described in Nodal Loading. Harmonically varying pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 83.1: PLANE83 Geometry. Positive pressures act into the element. Harmonically varying 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.

KEYOPT(3) is used for temperature loading with MODE > 0 and temperature-dependent material properties. Material properties may only be evaluated at a constant (nonharmonically varying) temperature. If MODE = 0, the material properties are always evaluated at the average element temperature. If MODE > 0, TREF must be input as zero.

KEYOPT(4), (5), and (6) provide various element printout options. (See Element Solution.)

A summary of the element input is given in "PLANE83 Input Summary". A general description of element input is given in Element Input.

PLANE83 Input Summary


I, J, K, L, M, N, O, P

Degrees of Freedom


Real Constants


Material Properties
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), T(M), T(N), T(O), T(P)

Mode Number

Number of harmonic waves around the circumference (MODE)

Loading Condition

Symmetry condition (MODE)

Special Features
Birth and death
Stress stiffening

Element coordinate system:

0 -- 

Element coordinate system is parallel to the global coordinate system

1 -- 

Element coordinate system is based on the element I-J side


If MODE is greater than zero, use temperatures for:

0 -- 

Use temperatures only for thermal bending (evaluate material properties at TREF)

1 -- 

Use temperatures only for material property evaluation (thermal strains are not computed)


Extra stress output:

0 -- 

Basic element solution (not extra output)

1 -- 

Repeat basic solution for all integration points

2 -- 

Nodal stress solution


Combined stress output:

0 -- 

No combined stress solution

1 -- 

Combined stress solution at centroid and nodes


Extra surface output (surface solution is valid only for isotropic materials):

0 -- 

Basic element solution (no extra output)

1 -- 

Surface solution for face I-J also

2 -- 

Surface solution for both faces I-J and K-L also

PLANE83 Output Data

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

Several items are illustrated in Figure 83.2: PLANE83 Stress Output.

In the displacement printout, the UZ component is out-of-phase with the UX and UY components. For example, in the MODE = 1, ISYM = 1 loading case, UX and UY are the peak values at θ = 0° and UZ is the peak value at θ = 90°. The same occurs for the reaction forces (FX, FY, etc.). We recommend that you always use the angle field on the SET command when postprocessing the results. For more information about harmonic elements, see Harmonic Axisymmetric Elements with Nonaxisymmetric Loads.

The element stress directions are parallel to the element coordinate system. The sign convention on the surface shears is such that for a rectangular element that is lined up parallel to the axes with node J in the positive Y direction from node I, the shear stresses on surfaces I-J and K-L are analogous to the centroidal SYZ in both definition and sign. Stress components which are inherently zero for a load case are printed for clarity. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 83.2:  PLANE83 Stress Output

PLANE83 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 83.1:  PLANE83 Element Output Definitions

ELElement NumberYY
NODESCorner nodes - I, J, K, LYY
MATMaterial numberYY
ISYMLoading key: 1 = symmetric, -1 = antisymmetricY-
MODENumber of waves in loadingYY
PRESPressures P1 at nodes J,I; P2 at K,J; P3 at L,K; P4 at I,LYY
TEMPTemperatures T(I), T(J), T(K), T(L), T(M), T(N), T(O), T(P)YY
S:X, Y, ZDirect stresses (radial, axial, hoop) at PK ANG locationsYY
S:XY, YZ, XZShear stresses (radial-axial, axial-hoop, radial-hoop) at PK ANG locationsYY
S:1, 2, 3Principal stresses at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.11
S:INTStress intensity at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.11
S:EQVEquivalent stress at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.11
EPEL:X, Y, Z, XYElastic strainYY
EPEL:EQVEquivalent elastic strain [4]-Y
EPTH:X, Y, Z, XYAverage thermal strainsYY
EPTH:EQVEquivalent thermal strain [4]-Y
PK ANGAngle where stresses have peak values: 0 and 90/MODE°. Blank if MODE = 0.YY
XC, YCLocation where results are reportedY3
FACEFace label22
TEMPSurface average temperature22
EPEL(PAR, PER, Z, SH)Surface strains (parallel, perpendicular, hoop, shear) at PK ANG locations and where extreme occurs (EXTR)22
S(PAR, PER, Z, SH)Surface stresses (parallel, perpendicular, hoop, shear) at PK ANG locations and where extreme occurs (EXTR)22

  1. These items are output only if KEYOPT(5) = 1.

  2. These items are printed only if KEYOPT(6) is greater than zero.

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

  4. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY).

Table 83.2: PLANE83 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See Creating an Element Table 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 83.2: PLANE83 Item and Sequence Numbers:


output quantity as defined in the Table 83.1: PLANE83 Element Output Definitions


predetermined Item label for ETABLE command


sequence number for data at nodes I,J,K,L

Table 83.2:  PLANE83 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
EXTR Values

The NMISC items (1 thru 60) in the above table represent the combined stress solution, KEYOPT(5) = 1. If MODE = 0, their values are zero at THETA = 90/MODE and at EXTR.

See Surface Solution for the item and sequence numbers for surface output for the ETABLE command.

PLANE83 Assumptions and Restrictions

  • The area of the element must be positive.

  • The element must be defined in the global X-Y plane as shown in Figure 83.1: PLANE83 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.

  • The element assumes a linear elastic material.

  • Post-analysis superposition of results is valid only with other linear elastic solutions.

  • The element should not be used with the large deflection option.

  • The element may not be deactivated with the EKILL command.

  • The element temperature is taken to be the average of the nodal temperatures.

  • Surface stress printout is valid only if the conditions described in Element Solution are met.

Modeling hints: 

  • If shear effects are important in a shell-like structure, at least two elements through the thickness should be used.

  • You can use only axisymmetric (MODE,0) loads without significant torsional stresses to generate the stress state used for stress stiffened modal analyses using this element.

PLANE83 Product Restrictions

There are no product-specific restrictions for this element.

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