The element is a generalization of the axisymmetric version of PLANE42, the 2D structural solid element, in that the loading need not be axisymmetric. See Section for a description of various loading cases. See Section 14.25 in the ANSYS Theory Reference for more details about this element. A multinode version of this element (PLANE83) is described in Section 4.83.
Figure 4.251 PLANE25 4Node AxisymmetricHarmonic Structural Solid
The material may be orthotropic, with directions corresponding to the element coordinate directions. The element coordinate system orientation is as described in Section 2.3. Properties not input default as described in Section 2.4. Harmonically varying nodal forces, if any, should be input on a full 360° basis.
Element loads are described in Section 2.7. Harmonically varying pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 4.251. 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 greater than zero and temperature dependent material properties. Material properties may only be evaluated at a constant (nonharmonically varying) temperature. If MODE equals zero, material properties are always evaluated at the average element temperature.
KEYOPT(4), (5), and (6) provide various element printout options (see Section 2.2.2).
A summary of the element input is given in Table 4.251. Section 2.1 gives a general description of element input.
Table 4.251 PLANE25 Input Summary
Element Name

PLANE25

Nodes

I, J, K, L

Degrees of Freedom

UX, UY, UZ

Real Constants

None.

Material Properties

EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), ALPX,
ALPY, ALPZ, DENS, GXY, GYZ, GXZ, DAMP

Surface Loads

Pressures: face 1 (JI), face 2 (KJ), face 3 (LK), face 4 (IL)

Body Loads

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

Mode Number

Input mode number on MODE command

Loading Condition

Input this value for ISYM on MODE command 1  Symmetric loading 1  Antisymmetric loading

Special Features

Stress stiffening, Birth and death

KEYOPT(1)

0  Element coordinate system is parallel to the global coordinate
system 1  Element coordinate system is based on the element IJ side.

KEYOPT(2)

0  Include extra displacement shapes 1  Suppress extra displacement shapes

KEYOPT(3)

Used only for mode greater than zero 0  Use temperatures for thermal bending (evaluate material properties at TREF) 1  Use temperatures for material property evaluation (Thermal bending not permitted  ALPX, ALPY, and ALPZ must all be zero)

KEYOPT(4)

Controls solution printout: 0  Basic element solution 1  Repeat basic solution for all integration points 2  Nodal stress solution

KEYOPT(5)

Controls combined stress output: 0  No combined stress solution 1  Combined stress solution at centroid and nodes

KEYOPT(6)

Controls surface printout. Surface solution is valid only for isotropic
materials. 0  Basic element solution 1  Surface solution for face IJ also 2  Surface solution for both faces IJ and KL also

In the displacement printout, the UZ component is outofphase with the UX and UY components. For example, in the MODE=1, ISYM=1 loading case, UX and UY are the peak values at =0° and UZ is the peak value at =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 Section 2.9
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 IJ and KL 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. Section 2.2 gives a general description of solution output. See the ANSYS Basic Analysis Procedures Guide for ways to view results.
Figure 4.252 PLANE25 Stress Output
The following notation is used in Table 4.252:
A colon (:) in the Name column indicates the item can be accessed by the Component Name method [ETABLE, ESOL] (see Section 2.2.2). The O and R columns indicate the availability of the items in the file Jobname.OUT (O) or in the results file (R), a Y indicates that the item is always available, a number refers to a table footnote which describes when the item is conditionally available, and a  indicates that the item is not available.
Table 4.252 PLANE25 Element Output Definitions
Name

Definition

O

R

EL

Element number

Y  Y 
NODES

Nodes  I, J, K, L

Y  Y 
MAT

Material number

Y  Y 
ISYM

Loading key: 1 = symmetric, 1 = antisymmetric

Y   
MODE

Number of waves in loading

Y   
VOLU:

Volume

Y  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 
CENT: X, Y

Global location of element centroid XC, YC

Y  Y 
S: X, Y, Z

Direct stresses (radial, axial, hoop) at PK ANG locations

Y  Y 
S: XY, YZ, XZ

Shear stresses (radialaxial, axialhoop, radialhoop) 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 
FACE

Face label

2  Y 
TEMP

Surface average temperature

2  Y 
EPEL(PAR,
PER, Z, SH)

Surface strains (parallel, perpendicular, hoop, shear) at PK
ANG locations and where extreme occurs (EXTR)

2  Y 
S(PAR, PER,
Z, SH)

Surface stresses (parallel, perpendicular, hoop, shear) at PK
ANG locations and where extreme occurs (EXTR)

2  Y 
2. These items are printed only if KEYOPT(6) is greater than zero.
Table 4.253 lists output available through the ETABLE command using the Sequence Number method. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide and Section 2.2.2.2 of this manual for more information. The following notation is used in Table 4.253:
Name

Item

I

J

K

L

P1

SMISC

2  1     
P2

SMISC

  4  3   
P3

SMISC

    6  5 
P4

SMISC

7      8 
THETA=0


S1

NMISC

1  16  31  46 
S2

NMISC

2  17  32  47 
S3

NMISC

3  18  33  48 
SINT

NMISC

4  19  34  49 
SEQV

NMISC

5  20  35  50 
THETA=90/MODE


S1

NMISC

6  21  36  51 
S2

NMISC

7  22  37  52 
S3

NMISC

8  23  38  53 
SINT

NMISC

9  24  39  54 
SEQV

NMISC

10  25  40  55 
EXTR Values


S1

NMISC

11  26  41  56 
S2

NMISC

12  27  42  57 
S3

NMISC

13  28  43  58 
SINT

NMISC

14  29  44  59 
SEQV

NMISC

15  30  45  60 
See Section 2.2.2.5 of this manual for the item and sequence numbers for surface output for the ETABLE command.
The element assumes a linear elastic material. Postanalysis 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 Section 2.8). 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 Section 2.2.2 are met. You can use only axisymmetric (MODE,0) loads to generate the stress state used for stress stiffened modal analyses using this element.
Modeling hints: If shear effects are important in a shelllike structure, at least two elements through the thickness should be used.