HSFLD241 Element Description

HSFLD241 is used to model fluids that are fully enclosed by solids (containing vessels). The hydrostatic fluid element is well suited for calculating fluid volume and pressure for coupled problems involving fluid-solid interaction. The pressure in the fluid volume is assumed to be uniform (no pressure gradients), so sloshing effects cannot be included. Temperature effects and compressibility may be included, but fluid viscosity cannot be included.

Hydrostatic fluid elements are overlaid on the faces of 2D solid elements enclosing the fluid volume. See HSFLD241 in the Mechanical APDL Theory Reference for more details about this element. See HSFLD242 for a 3D version of this element.

Figure 241.1: HSFLD241 Geometry

HSFLD241 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 241.1: HSFLD241 Geometry. The hydrostatic fluid element is defined by three or four nodes. Nodes I, J and K on the surface (face 1) are shared with the solid element and have two degrees of freedom at each node: translation in x and y directions. Node K is not used if the underlying solid element does not have a midside node. For the case of a degenerate solid element sharing the collapsed face with the hydrostatic fluid element, the surface nodes of the hydrostatic fluid element will be coincident. Node L is a pressure node with a hydrostatic pressure degree of freedom. Hydrostatic fluid elements can be generated automatically using the ESURF command.

The pressure node (L) can be located anywhere in the fluid volume, except when the fluid volume has symmetry boundaries; in this case the pressure node must be located on the symmetry line or on the intersection point of multiple symmetry lines. The pressure node is automatically moved to the centroid of the fluid volume if there are no displacement degree-of-freedom constraints specified. To keep the pressure node on a symmetry line, you must specify symmetry boundary conditions at this node. (The displacement degrees of freedom at the pressure node do not have any displacement solution associated with them. They are only available for applying displacement degree of freedom constraints.) The pressure node is shared by all the hydrostatic fluid elements used to define the fluid volume. It is also used to apply temperature loads, fluid mass flow rate, or hydrostatic pressure degree-of-freedom constraints for the fluid.

You can define a hydrostatic fluid element without an underlying solid element in situations where the underlying solid has a discontinuity. In this case, the surface nodes (I and J) of the hydrostatic fluid element must be shared with adjacent solid elements, or the displacement degrees of freedom at the surface nodes should be constrained. For example, the gap between the cylinder and piston in a cylinder-piston assembly with fluid may be bridged with a hydrostatic fluid element by sharing one of its surface nodes (I) with a solid element on the cylinder and its other surface node (J) with a solid element on the piston (see Example Model Using Hydrostatic Fluid Elements in the Structural Analysis Guide).

You can define material properties for hydrostatic fluid elements using MP or TB commands. All hydrostatic fluid elements sharing a pressure node must use the same material property definition and must have the same real constant values (THK and PREF).

You can input element thickness and reference pressure (must be specified for compressible gas defined via TB command with Lab = FLUID and TBOPT = GAS) as real constants THK and PREF. The THK value is used to calculate element volume.

You can define the initial state of the hydrostatic fluid by defining initial pressure (input via the IC command with Lab = HDSP) at the pressure node. Specify the reference temperature by using the TREF command or the MP,REFT command. For compressible gas (defined via the TB command with Lab = FLUID and TBOPT = GAS), the initial pressure and the reference pressure (input as real constant PREF) are added internally to get the total initial pressure for the Ideal Gas Law. Internal force corresponding to initial pressure is calculated internally and applied over the first load step.

You can prescribe uniform pressure for the fluid as a hydrostatic pressure degree-of-freedom constraint at the pressure node (input on D command with Lab = HDSP). The change in hydrostatic pressure value is assumed to occur as a result of the addition or removal of fluid mass to or from the containing vessel. Applying a hydrostatic pressure degree-of-freedom constraint is equivalent to applying a surface load on the underlying solid element surface. Element loads are described in Element Loading. You can apply fluid mass flow rate as a load on the pressure node (input via F command with Lab = DVOL); a positive value indicates fluid mass flowing into the containing vessel. You can also input fluid temperature as an element body load at the pressure node (input via BF command with Lab = TEMP). The nodal temperature defaults to TUNIF.

You can model fluid flow between two fluid volumes in two containing vessels by using FLUID116 coupled thermal-fluid pipe elements to connect the pressure nodes of the two fluid volumes. A single FLUID116 element must be used to connect the two fluid volumes. You can also model fluid flow through an orifice between a fluid volume and the atmosphere by connecting one node of a FLUID116 element with the HSFLD241 pressure node; the other node of the FLUID116 element represents environmental pressure. For either of these scenarios, you must activate the PRES degree of freedom (KEYOPT(1) = 1) on the pressure node of the hydrostatic fluid elements, and you must set KEYOPT(1) = 3 on the FLUID116 element.

KEYOPT(1) defines degrees of freedom for the hydrostatic fluid element:

KEYOPT(3) defines the hydrostatic fluid element behavior:

KEYOPT(5) specifies how mass is computed for the hydrostatic fluid element:

KEYOPT(6) defines the hydrostatic fluid element compressibility:

You can define contact and target surfaces on the attached 2D solid elements to model self-contact between walls of the containing vessel after the fluid has been removed. Note that contact should not cause a single fluid region to be separated into two since the pressure-volume calculations are performed assuming a single cavity.

For more information on using hydrostatic fluid elements to model fluids enclosed by solids, see Modeling Hydrostatic Fluids in the Structural Analysis Guide.

"HSFLD241 Input Summary" contains a summary of the element input. See Element Input in this document for a general description of element input.

HSFLD241 Output Data

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

A general description of solution output is given in 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 241.2: HSFLD241 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 241.2: HSFLD241 Item and Sequence Numbers:

HSFLD241 Assumptions and Restrictions

HSFLD241 Product Restrictions

There are no product-specific restrictions for this element.