37.7.1. Fluid Dialog Box

The Fluid dialog box sets the conditions for a fluid cell zone. It is opened from the Cell Zone Conditions Task Page. See Inputs for Fluid Zones and User Inputs for Porous Media for details about the items below.

Controls

Zone Name

sets the name of the zone.

Material Name

sets the fluid material. The drop-down list contains the names of all materials that have been loaded into the solver. Materials are defined with the Materials Task Page.


Important:  If you are modeling species transport or multiphase flow, the Material Name list will not appear in the Fluid dialog box. For species calculations, the mixture material for all fluid zones will be the material you specified in the Species Model Dialog Box. For multiphase flows, the materials are specified when you define the phases, as described in Defining the Phases for the VOF Model.


Frame Motion

enables the moving reference frame model for the cell zone. See Specifying the Rotation Axis and Defining Zone Motion for details.

Mesh Motion

enables the sliding mesh model for the cell zone. See Setting Up the Sliding Mesh Problem for details.

Porous Zone

indicates that the zone is a porous medium. Additional items will appear in the dialog box when this option is enabled. See User Inputs for Porous Media for details.

3D Fan Zone

allows you to simulate the effect of an axial fan by applying a distributed momentum source in a toroid-shaped fluid volume. This model can calculate not only the axial velocity, but the swirl and radial velocities as well. When you enable this option, the 3D Fan Zone tab becomes available, so that you can specify the geometry and properties of the fan. The cell zone should have a toroid shape that is sized to match the blade-swept volume of the fan you are simulating (that is, has an inner and outer radius that matches the radius of the fan’s hub and blade tips, respectively, as well as a length that matches the thickness of the toroid region swept by the blades in the axial direction). Furthermore, the fluid cell zone should be “interior”, that is, have at least two boundary zones of type interior that border another fluid cell zone and act as the fan inlet and outlet (the other boundaries can be of type interior as well). See 3D Fan Zones for details.

Laminar Zone

disables the calculation of turbulence production in the fluid zone (appears only for turbulent flow calculations using the Spalart-Allmaras model or one of the -  or -  models). See Specifying a Laminar Zone for details.

LES Zone

allows you to model a smaller embedded LES zone within a larger URANS computational domain for turbulent flow calculations. When you turn on this option, the Embedded LES tab will be enabled to allow you to specify properties for the embedded LES zone. See Setting Up the Embedded Large Eddy Simulation (ELES) Model for details.

Source Terms

enables the specification of volumetric sources of mass, momentum, energy, and so on. When you turn on this option, the Source Terms tab will be enabled to allow you to specify the values for the desired sources. See Defining Mass, Momentum, Energy, and Other Sources for details.

Fixed Values

enables the fixing of the value of one or more variables in the fluid zone, rather than computing them during the calculation. See Fixing the Values of Variables for details.


Important:  You can fix values for velocity components, temperature, and species mass fractions only if you are using the pressure-based solver.


Participates In Radiation

specifies whether or not the fluid zone participates in radiation. This option appears when you are using the DO model for radiation.

Warning:  In general, disabling Participates in Radiation for fluid zones is not recommended, as it can produce erroneous results. There are rare cases when it is acceptable: for example, if the domain contains multiple fluid zones, disabling this option for zones where radiation is negligible may save computational time without affecting the results.

Reaction

enables/disables reactions in the porous zone.

Electrolyte

indicates that the zone is an electrolyte zone. By default, all fluid zones are assumed to be electrolyte zones. This option appears when the Electrochemical Reaction model is enabled.

Reference Frame

lists the parameters that define motion for a moving reference frame.

Rotation-Axis Origin

specifies the origin for the axis of rotation of solid zone. See Specifying the Rotation Axis for details. This item will appear only for 3D and 2D non-axisymmetric models.

Rotation-Axis Direction

specifies the direction vector for the solid zone’s axis of rotation. See Specifying the Rotation Axis for details. This item will appear only for 3D models.

Rotational Velocity

contains an input field for the rotational Speed of the zone.

Translational Velocity

contains inputs for the X, Y, and Z velocities of the zone.

Relative Specification

indicates whether the velocities are absolute velocities (absolute) or velocities relative to the motion of each cell zone (Relative to Cell Zone). This selection is necessary only if your problem involves moving reference frames or sliding meshes. If there is no zone motion, both options are equivalent.

UDF

allows you to hook the DEFINE_ZONE_MOTION user-defined function.

Copy to Mesh Motion

allows you to switch between the MRF and moving mesh models. The variables used for the origin, axis, and velocity components, as well as for the DEFINE_ZONE_MOTION user-defined function, will be copied from one model to the other.

Mesh Motion

lists the parameters that define motion for a moving reference frame.

Rotation-Axis Origin

specifies the origin for the axis of rotation of solid zone. See Specifying the Rotation Axis for details. This item will appear only for 3D and 2D non-axisymmetric models.

Rotation-Axis Direction

specifies the direction vector for the solid zone’s axis of rotation. See Specifying the Rotation Axis for details. This item will appear only for 3D models.

Rotational Velocity

contains an input field for the rotational Speed of the zone.

Translational Velocity

contains inputs for the X, Y, and Z velocities of the zone.

Relative Specification

indicates whether the velocities are absolute velocities (absolute) or velocities relative to the motion of each cell zone (Relative to Cell Zone). This selection is necessary only if your problem involves moving reference frames or sliding meshes. If there is no zone motion, both options are equivalent.

UDF

allows you to hook the DEFINE_ZONE_MOTION user-defined function.

Copy to Frame Motion

allows you to switch between the MRF and moving mesh models. The variables used for the origin, axis, and velocity components, as well as for the DEFINE_ZONE_MOTION user-defined function, will be copied from one model to the other.

Porous Zone

lists the parameters associated with the porous zone.

Conical

enables the specification of a conical (or cylindrical) porous medium. This item will appear only when the Porous Zone option is enabled for a 3D case.

Cone Half Angle

specifies the angle between the cone’s axis and its surface (see Figure 6.13: Cone Half Angle). Set this to 0 to define the porous region using a cylindrical coordinate system. This item will appear only when the Porous Zone and Conical options are enabled.

Snap to Zone

aligns the plane (or line, in 2D) tool with the zone selected in the drop-down list. The tool is centered at the centroid of the zone, with the tool’s axis normal to the zone. If this axis is not the desired cone axis, reposition the tool (as described in Using the Plane Tool). When you are satisfied with the axis, click the Update From Plane Tool (or Update From Line Tool) button to update the Cone Axis Vector fields.

This item will appear only when the Porous Zone and Conical options are enabled.

Update From Plane Tool

(Update From Line Tool in 2D) updates the Direction-1 Vector and (in 3D) the Direction-2 Vector from the plane tool orientation. If the Conical option is enabled, this button will update the Cone Axis Vector and the Point on Cone Axis. See Defining the Viscous and Inertial Resistance Coefficients for details. This item will appear only when the Porous Zone option is enabled.

Direction-1 Vector, Direction-2 Vector

indicate the directions for which the resistance coefficients are defined. See Defining the Viscous and Inertial Resistance Coefficients for details. These items will appear only when the Porous Zone option is enabled, but the Conical option is not. (In 2D, only Direction-1 Vector will appear.)

Cone Axis Vector

specifies the X,Y,Z vector for the cone’s axis.

This item will appear only when the Porous Zone and Conical options are enabled.

Point on Cone Axis

specifies a point on the cone’s axis. This point will be used by ANSYS Fluent to transform the resistances to the Cartesian coordinate system.

This item will appear only when the Porous Zone and Conical options are enabled.

Relative Velocity Resistance Formulation

allows ANSYS Fluent to either apply the relative reference frame or the absolute reference frame. This allows for the correct prediction of the source terms.

Viscous Resistance, Inertial Resistance

contain inputs for the viscous resistance coefficient and the inertial resistance coefficient in each direction. See Defining the Viscous and Inertial Resistance Coefficients for details. These items will appear only when the Porous Zone option is enabled.

Alternative Formulation

provides better stability to the calculation when your porous medium is anisotropic.

If you have enabled the Conical option, Direction-1 is the cone axis direction, Direction-2 is the normal to the cone surface (radial () direction for a cylinder), and Direction-3 is the circumferential () direction.

Power Law Model

contains inputs for the C0 and C1 coefficients in the power law model for porous media. See Using the Power-Law Model for details.

Fluid Porosity

contains an additional input for the porous medium. See User Inputs for Porous Media for details.

Porosity

sets the volume fraction of fluid within the porous region.

Heat Transfer Settings

contains heat transfer settings for the porous medium. See Specifying the Heat Transfer Settings for details.

Thermal Model

specifies whether or not thermal equilibrium is assumed between the medium and the fluid flow.

Equilibrium

specifies that the medium and the fluid flow are in thermal equilibrium in the porous medium.

Non-Equilibrium

specifies that the medium and the fluid flow are not in thermal equilibrium in the porous medium, so that a dual cell approach is enabled.

Solid Material Name

specifies the solid material in the porous region. This drop-down menu is only available when Equilibrium is selected from the Thermal Model list.

Solid Zone

displays the name of the solid cell zone that is coupled with the porous fluid zone through heat transfer. This field is only displayed when Non-Equilibrium is selected from the Thermal Model list.

Interfacial Area Density

specifies (as described in Non-Equilibrium Thermal Model Equations) for the porous region. This text-entry box is only available when Non-Equilibrium is selected from the Thermal Model list.

Heat Transfer Coefficient

specifies (as described in Non-Equilibrium Thermal Model Equations) for the porous region. This text-entry box is only available when Non-Equilibrium is selected from the Thermal Model list.

Anisotropic Species Diffusion

allows you to model anisotropic species diffusion in porous media. When this option is selected, you can specify the Matrix Components for the anisotropic diffusion matrix in the porous zone. This option is available only with the species transport models.

3D Fan Zone

provides the settings that define a 3D fan zone. See 3D Fan Zones for details.

Geometry

allows you to define the location and size of the fan.

Inlet Fan Zone

allows you to select a boundary zone of type interior that will act as the surface on which the fan will be located.

Hub Radius

defines the radius of the fan hub, that is, the inner radius of the blade-swept volume on which the fan’s distributed momentum sources are applied.

Tip Radius

defines the radius of the blade tips of the fan, that is, the outer radius of the blade-swept volume on which the fan’s distributed momentum sources are applied.

Thickness

defines the thickness of the toroid region swept by the blades in the axial direction.

Inflection Point

is a ratio that defines the fraction of the fan blade length (starting at the hub) over which the tangential velocity of the fan discharge is increasing with increasing radius and peaks, before tapering off (see Figure 6.17: The Inflection Point Ratio of a Pitched Blade Turbine).

Fan Origin

defines the X, Y, and Z coordinates of a point on the Inlet Fan Zone that is the origin for the fan.

Properties

allows you to define how the fan behaves.

Rotational Direction

allows you to define the fan’s rotational direction, using the right-hand rule with respect to the fan direction vector (that is, a vector from the Fan Origin that points into the 3D fan zone perpendicular to the Inlet Fan Zone).

Operating Angular Velocity

defines the angular velocity of the fan during the simulation.

Limit Flow Rate Through Fan

specifies that the flow rate through the fan adheres to minimum and maximum values, as defined in the Flow Rate group box.

Flow Rate

allows you to define the Maximum and Minimum flow rates through the fan. This group box is available when the Limit Flow Rate Through Fan option is enabled.

Tangential Source Term

enables a momentum source in the tangential direction, based on impeller theory.

Radial Source Term

enables a momentum source in the radial direction, based on impeller theory.

Axial Source Term

enables a momentum source in the axial direction, based on the settings in the Axial Source Term Settings group box.

Axial Source Term Settings

allows you to define the momentum source in the axial direction. This group box is only available when the Axial Source Term option is enabled.

Method

specifies whether a constant pressure or a fan curve (that is, a curve created from data points that plot pressure rise vs. volumetric flow rate) defines the axial momentum source.

Pressure Jump

defines the pressure jump that is applied across the 3D fan. This setting is only available when constant pressure is selected for the Method.

Read Fan Curve...

allows you to read a tab-delimited ASCII file that defines the relationship between pressure and flow rate for each 3D fan cell zone (see 3D Fan Curve File Format for details). This button is only available when fan curve is selected for the Method.

Curve Fitting Method

specifies whether Fluent should apply a polynomial or piecewise-linear fitting method to construct a curve from the data points in the fan curve file. This drop-down list is only available when fan curve is selected for the Method.

Order of Polynomial

defines the order of the polynomial curve fitting method. This setting is only available when polynomial is selected for the Curve Fitting Method.

Initial Flow Rate

specifies your best estimate of the initial flow rate through the fan. This setting is only available when fan curve is selected for the Method.

Test Angular Velocity

specifies the angular velocity of the fan used in the experiment that generated the fan curve data. This setting is only available when fan curve is selected for the Method.

Test Temperature

specifies the temperature of the fluid flowing through the fan during the experiment that generated the fan curve data. This setting is only available when fan curve is selected for the Method.

Reaction

lists the parameters for reactions in the porous zone.

Reaction Mechanism

allows you to specify a defined group, or mechanism, of available reactions. See Defining Zone-Based Reaction Mechanisms for details about defining reaction mechanisms.

Surface-to-Volume Ratio

specifies the surface area of the pore walls per unit volume (), and can be thought of as a measure of catalyst loading. With this value, ANSYS Fluent can calculate the total surface area on which the reaction takes place in each cell by multiplying by the volume of the cell.

Source Terms

defines a source of heat, mass, momentum, turbulence, species, or other scalar quantity within the fluid zone.

Fixed Values

allows you to specify which variables in the fluid zone are fixed (as a constant value or as defined by a profile or user-defined function), rather than computed during the calculation. See Fixing the Values of Variables for details.

Local Coordinate System for Fixed Velocities

enables the specification of fixed cylindrical velocity components instead of Cartesian components. The local coordinate system is defined by the Rotation-Axis Origin and Rotation-Axis Direction.

This item is available only in 3D, and only when the Fixed Values option is on.

Multiphase

allows you to set parameters that are specific to the multiphase models.

Compressive Scheme Slope Limiter

ranges from 0 to 2. For example, a Compressive Scheme Slope Limiter of 0 corresponds to first order upwind behavior, a value of 1 corresponds to second order upwind, and a value of 2 applies the compressive scheme. The Multiphase tab is available only if Zonal Discretization is enabled in the Multiphase Model Dialog Box.

Numeric Beach Treatment

is available when Open Channel Flow and/or Open Channel Wave BC is enabled in the Multiphase Model dialog box (see Numerical Beach Treatment for Open Channels for more detail).

Numerical Beach

when enabled expands the dialog box where you can specify the numerical beach parameters.

Beach Group ID

represents the cell zones sharing the damping length containing the same input parameters.

Damping Type

allows you to choose between One Dimensional and Two Dimensional damping.

One Dimensional

is the damping treatment in the flow direction.

Two Dimensional

is the damping treatment in the flow and gravity direction.

Compute From Inlet Boundary

is set to none by default. If there are available open channel boundaries (velocity-inlet, pressure-inlet, and mass-flow-inlet), boundary names are added to the drop-down list. If you select a boundary from the list, the Level Inputs, Damping Length Inputs in Flow Direction, and Damping Resistance values will be updated in the interface. You have the option to overwrite the updated inputs with values that are more applicable to your simulation.

Level Inputs

is only available for the Two Dimensional damping type.

Free Surface Level

is the same definition as for open channel flow, see Modeling Open Channel Flows.

Bottom Level

is the same definition as for open channel flow, see Modeling Open Channel Flows, and is valid only for shallow waves. The bottom level is used for calculating the liquid height.

Flow Direction

is the X, Y, and Z (for 3D) components.

Damping Length Inputs in Flow Direction

are required to calculate the start and end points of the damping length in the flow direction.

Damping Length Specification

is only available if Open Channel Wave BC is enabled in the Multiphase Model dialog box. There are two options you can choose from End Point and Wave Lengths or End and Start Points.

End Point

is the end point of the damping zone.

Start Point

is the starting point in the flow direction.

Wave Length

is updated automatically if the boundary is selected from the Compute From Inlet Boundary drop-down list.

Number Of Wave Lengths

is set to 2 by default for the calculation of the damping length.

Relative Velocity Resistance Formulation

calculates the source term using relative velocities in the numerical beach zone when using moving/deforming meshes or moving reference frames.

Linear Damping Resistance

is the resistance per unit time.

Quadratic Damping Resistance

is the resistance per unit length.


Release 18.2 - © ANSYS, Inc. All rights reserved.