Axisymmetric-Harmonic 4-Node Structural Solid
|Although this legacy element is available for use in your analysis, ANSYS, Inc. recommends using a current-technology element such as SOLID272 (KEYOPT(6) = 0), unless you are performing a linear analysis and require a sinusoidal load variation in the circumferential direction.|
PLANE25 is used for 2-D modeling of axisymmetric structures with nonaxisymmetric loading. Examples of such loading are bending, shear, or torsion. The element is defined by four nodes having three degrees of freedom per node: translations in the nodal x, y, and z direction. For unrotated nodal coordinates, these directions correspond to the radial, axial, and tangential directions, respectively.
See Harmonic Axisymmetric Elements with Nonaxisymmetric Loads for a description of various loading cases. See PLANE25 in the Mechanical APDL Theory Reference for more details about this element. See PLANE83 for a multi-node version of this element.
The geometry, node locations, and the coordinate system for this element are shown in Figure 25.1: PLANE25 Geometry. The element input data includes four nodes, the number of harmonic waves (MODE on the MODE command), the symmetry condition (ISYM on the MODE command) and the orthotropic material properties. The MODE and ISYM parameters are discussed in detail in Harmonic Axisymmetric Elements with Nonaxisymmetric Loads.
The material may be orthotropic, with directions corresponding to the element coordinate directions. The element coordinate system orientation is as described in Coordinate Systems. Harmonically varying nodal forces, if any, should be input on a full 360° basis.
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 25.1: PLANE25 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). For any other input pattern, unspecified temperatures default to TUNIF.
KEYOPT(2) is used to include or suppress the extra displacement shapes.
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).
I, J, K, L
UX, UY, UZ
|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, BETD, ALPD, DMPR|
face 1 (J-I), face 2 (K-J), face 3 (L-K), face 4 (I-L)
T(I), T(J), T(K), T(L)
Number of harmonic waves around the circumference (MODE)
Symmetry condition (MODE)
|Birth and death|
Element coordinate system:
Element coordinate system is parallel to the global coordinate system
Element coordinate system is based on the element I-J side.
Extra displacement shapes:
Include extra displacement shapes
Suppress extra displacement shapes
If MODE is greater than zero, use temperatures for:
Use temperatures only for thermal bending (evaluate material properties at TREF)
Use temperatures only for material property evaluation (thermal strains are not computed)
Extra stress output:
Basic element solution
Repeat basic solution for all integration points
Nodal Stress Solution
Combined stress output:
No combined stress solution
Combined stress solution at centroid and nodes
Include extra surface output (surface solution valid only for isotropic materials):
Basic element solution
Surface solution for face I-J also
Surface solution for both faces I-J and K-L also
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 25.1: PLANE25 Element Output Definitions.
Several items are illustrated in Figure 25.2: PLANE25 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.). The element stress directions are parallel to the element coordinate system. 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 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. Solution Output gives a general description of 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 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 25.1: PLANE25 Element Output Definitions
|NODES||Nodes - I, J, K, L||Y||Y|
|ISYM||Loading key: 1 = symmetric, -1 = antisymmetric||Y||-|
|MODE||Number of waves in loading||Y||-|
|PRES||Pressure P1 at nodes J,I; P2 at K,J; P3 at L,K; P4 at I,L||Y||Y|
|TEMP||Temperatures T(I), T(J), T(K), T(L)||Y||Y|
|PK ANG||Angle where component stresses have peak values: 0 and 90/MODE degrees. Blank if MODE = 0.||Y||Y|
|XC, YC||Location where results are reported||Y||3|
|S:X, Y, Z||Direct stresses (radial, axial, hoop) at PK ANG locations||Y||Y|
|S:XY, YZ, XZ||Shear stresses (radial-axial, axial-hoop, radial-hoop) at PK ANG locations||Y||Y|
|S:1, 2, 3||Principal stresses at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.||1||1|
|S:INT||Stress intensity at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.||1||1|
|S:EQV||Equivalent stress at both PK ANG locations as well as where extreme occurs (EXTR); if MODE = 0, only one location is given.||1||1|
|EPEL:X, Y, Z, XY||Elastic strain||Y||Y|
|EPEL:EQV||Equivalent elastic strain ||-||Y|
|EPTH:X, Y, Z, XY||Average thermal strains||1||1|
|EPTH:EQV||Equivalent thermal strain ||-||1|
|TEMP||Surface average temperature||2||2|
|EPEL(PAR, PER, Z, SH)||Surface strains (parallel, perpendicular, hoop, shear) at PK ANG locations and where extreme occurs (EXTR)||2||2|
|S(PAR, PER, Z, SH)||Surface stresses (parallel, perpendicular, hoop, shear) at PK ANG locations and where extreme occurs (EXTR)||2||2|
Table 25.2: PLANE25 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) of the Basic Analysis Guide and The Item and Sequence Number Table for more information. The following notation is used in Table 25.2: PLANE25 Item and Sequence Numbers:
Table 25.2: PLANE25 Item and Sequence Numbers
|Output Quantity Name||ETABLE and ESOL Command Input|
|THETA = 0|
|THETA = 90/MODE|
Note: 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.
The area of the element must be positive.
The element must be defined in the global X-Y plane as shown in Figure 25.1: PLANE25 Geometry and the global X-axis must be the radial direction. Negative X coordinates should not be used.
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.
A triangular element may be formed by defining duplicate K and L node numbers (see Degenerated Shape Elements). The extra shapes are automatically deleted for triangular elements so that a constant strain element results.
Surface stress printout is valid only if the conditions described in Element Solution are met.
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.
This element does not support spectrum analysis.
Modeling hint: If shear effects are important in a shell-like structure, you should use at least two elements through the thickness.