4.25 PLANE25 4-Node Axisymmetric-Harmonic Structural Solid

4.25 PLANE25 4-Node Axisymmetric-Harmonic Structural Solid (UP19980821 ) PLANE25 is used for two-dimensional 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.

The element is a generalization of the axisymmetric version of PLANE42, the 2-D 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 multi-node version of this element (PLANE83) is described in Section 4.83.

Figure 4.25-1 PLANE25 4-Node Axisymmetric-Harmonic Structural Solid



4.25.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.25-1. The element input data includes four nodes, the number of harmonic waves (MODE), the symmetry condition (ISYM) and the orthotropic material properties. If MODE=0, the element behaves similar to the axisymmetric case of PLANE42. The MODE and ISYM parameters are discussed in detail in Section 2.9.

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 4.25-1. 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 4.25-1. Section 2.1 gives a general description of element input.

Table 4.25-1 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 (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 )

Mode Number

Input mode number on MODE command

Loading Condition

Input this value for ISYM on MODE command
1 - Symmetric loading
-1 - Anti-symmetric 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 I-J 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 I-J also
2 - Surface solution for both faces I-J and K-L also


4.25.2 Output Data

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

Several items are illustrated in Figure 4.25-2.

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 =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 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. Section 2.2 gives a general description of solution output. See the ANSYS Basic Analysis Procedures Guide for ways to view results.

Figure 4.25-2 PLANE25 Stress Output



The following notation is used in Table 4.25-2:

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 4.25-2 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 = anti-symmetric

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

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

Table 4.25-3 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 4.25-3:

Table 4.25-3 PLANE25 Item and Sequence Numbers for the ETABLE and ESOL Commands

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
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.

See Section 2.2.2.5 of this manual for the item and sequence numbers for surface output for the ETABLE command.

4.25.3 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 4.25-1 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 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 shell-like structure, at least two elements through the thickness should be used.

4.25.4 Product Restrictions

There are no product-specific restrictions for this element.