The element is a generalization of the axisymmetric version of FLUID79, the two dimensional fluid element, in that the loading need not be axisymmetric. Various loading cases are described in Section 2.9. The fluid element is particularly well suited for calculating hydrostatic pressures and fluid/solid interactions. Acceleration effects, such as in sloshing problems, as well as temperature effects, may be included. See Section 14.81 of the ANSYS Theory Reference for more details about this element. Another fluid element (FLUID66) is available to model fluids flowing in pipes and channels.
NoteThe reduced method is the only acceptable method for modal analyses using the ANSYS fluid elements.
Figure 4.811 FLUID81 AxisymmetricHarmonic Contained Fluid Element
The use of KEYOPT(2) for gravity springs is discussed in Section 4.80.1. Vertical acceleration (ACELY on the ACEL command) is needed for the gravity springs regardless of the value of MODE, even for a modal analysis. 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 4.811. 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.
A summary of the element input is given in Table 4.811. A general description of element input is given in Section 2.1.
Table 4.811 FLUID81 Input Summary
Element Name

FLUID81

Nodes

I, J, K, L

Degrees of Freedom

UX, UY, UZ

Real Constants

None

Material Properties

EX, ALPX, DENS, VISC, 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 for ISYM on MODE command 1  Symmetric loading 1  Antisymmetric loading

Special Features

Plasticity, Creep, Swelling, Stress stiffening, Large deflection,
Large strain, Birth and death, Adaptive descent.

KEYOPT(2)

0  Place gravity springs on all sides of all elements 1  Place gravity springs only on face of elements located on Y = 0.0 plane (element must not have positive Y coordinates)

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°. Printout for combined loading cases may be obtained from the POST1 routine. 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.
A general description of solution output is given in Section 2.2. See the ANSYS Basic Analysis Procedures Guide for ways to view results.
The following notation is used in 4.812:
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 4.812 FLUID81 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  1 
MODE

Number of waves in loading

Y  Y 
VOLU:

Volume

Y  Y 
CENT: X, Y

Global location XC, YC

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)

Y  Y 
TAVG

Average temperature

Y   
PAVG

Average pressure

Y  Y 
Table 4.813 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 4.813:
Name

Item

E

I

J

K

L

PRES

SMISC

1         
P1

SMISC

  3  2     
P2

SMISC

    5  4   
P3

SMISC

      7  6 
P4

SMISC

  8      9 
The element temperature is taken to be the average of the nodal temperatures. Temperature dependent material properties, if any, are evaluated at the reference temperature [TREF].
Elements should be rectangular since results are known to be of lower quality for nonrectangular shapes. The nonlinear transient dynamic analysis should be used instead of the linear transient dynamic analysis for this element. A lumped mass matrix may be obtained for this element with the LUMPM command. See Section 4.80.3 for more assumptions and restrictions.