4.83 PLANE83 8-Node Axisymmetric-Harmonic Structural Solid

4.83 PLANE83 8-Node Axisymmetric-Harmonic Structural Solid (UP19980821 ) PLANE83 is used for two-dimensional 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 two-dimensional, 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 element is also a generalization of the axisymmetric version of PLANE82, the 2-D 8-node structural solid element, in that the loading need not be axisymmetric. Various loading cases are described in Section 2.9.

The 8-node elements have compatible displacement shapes and are well suited to model curved boundaries. See Section 14.83 in the ANSYS Theory Reference for more details about this element.

Figure 4.83-1 PLANE83 8-Node Axisymmetric-Harmonic Structural Solid



4.83.1 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 4.83-1. Orthotropic material directions correspond 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. The element input data is essentially the same as for PLANE82 and is described in Section 4.82, except as follows: Z-direction material properties (EZ, ALPZ, etc.) may be input. MODE and ISYM are used to describe the harmonic loading condition (see section 2.9 for more details).

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 4.83-1. 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). 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.

The KEYOPT(3) parameter 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, the 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 4.83-1. A general description of element input is given in Section 2.1.

Table 4.83-1 PLANE83 Input Summary

Element Name

PLANE83

Nodes

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

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

Mode Number

Input mode number on MODE command

Loading Condition

Input 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(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

4.83.2 Output Data

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

Several items are illustrated in Figure 4.83-2.

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). 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 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 Section 2.2. See the ANSYS Basic Analysis Procedures Guide for ways to view results.

Figure 4.83-2 PLANE83 Stress Output



The following notation is used in Table 4.83-2:

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 4.83-2 PLANE83 Element Output Definitions

Name

Definition

O

R

EL

Element number

Y Y
NODES

Corner nodes - I, J, K, L

Y Y
MAT

Material number

Y Y
ISYM

Loading key: 1 = symmetric, -1 = anti-symmteric

Y -
MODE

Number of waves in loading

Y Y
VOLU:

Volume

Y Y
PRES

Pressures 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), T(M), T(N), T(O), T(P)

Y Y
PK ANG

Angle where 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 4.83-3 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 4.83-3:

Table 4.83-3 PLANE83 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.

4.83.3 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 4.83-1 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 Section 2.4.2 of the ANSYS 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 Section 2.2.2 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 to generate the stress state used for stress stiffened modal analyses using this element.

4.83.4 Product Restrictions

There are no product-specific restrictions for this element.