To define the material contained in the fluid zone, select the appropriate item in the Material Name drop-down list. This list will contain all fluid materials database) in the Create/Edit Materials Dialog Box. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box.

If you want to define a source of heat, mass, momentum, turbulence, species, or other scalar quantity within the fluid zone, you can do so by enabling the Source Terms option. See Defining Mass, Momentum, Energy, and Other Sources for details.

If you want to fix the value of one or more variables in the fluid zone, rather than computing them during the calculation, you can do so by enabling the Fixed Values option. See Fixing the Values of Variables for details.

When you are calculating a turbulent flow, it is possible to “turn off” turbulence modeling in a specific fluid zone. To disable turbulence modeling, turn on the Laminar Zone option in the Fluid dialog box. This is useful if you know that the flow in a certain region is laminar. For example, if you know the location of the transition point on an airfoil, you can create a laminar/turbulent transition boundary where the laminar cell zone borders the turbulent cell zone. This feature allows you to model turbulent transition on the airfoil.

By default, the Laminar Zone option will set the turbulent viscosity, , to zero and disable turbulence production in the fluid zone. Turbulent quantities will still be transported through the zone, but effects on fluid mixing and momentum will be ignored. If you want to keep the turbulent viscosity, you can do so using the text command define/ boundary-conditions/fluid. You will be asked if you want to Set Turbulent Viscosity to zero within laminar zone?. If your response is no, Ansys Fluent will set the production term in the turbulence transport equation to zero, but will retain a nonzero .

Disabling turbulence modeling in a fluid zone can be applied to all the turbulence models except the Large Eddy Simulation (LES) model.

If you are modeling species transport with reactions, you can enable a reaction mechanism in a fluid zone by turning on the Reaction option and selecting an available mechanism from the Reaction Mechanism drop-down list. See Defining Zone-Based Reaction Mechanisms for more information about defining reaction mechanisms.

If there are rotationally periodic boundaries adjacent to the fluid zone or if the zone is rotating, either the mesh or its reference frame, you must specify the rotation axis. To define the axis for a moving reference frame problem, set the Rotation-Axis Direction and Rotation-Axis Origin under the Reference Frame tab. To define the axis for a moving mesh problem, set the Rotation-Axis Direction and Rotation-Axis Origin under the Mesh Motion tab.

The cell zone axis is independent of the axis of rotation used by any adjacent wall zones or any other cell zones. For 3D problems, the axis of rotation is the vector from the Rotation-Axis Origin in the direction of the vector given by your Rotation-Axis Direction inputs for the frame of reference and the mesh motion. For 2D non-axisymmetric problems, you will specify only the Rotation-Axis Origin; the axis of rotation is the -direction vector passing through the specified point. (The direction is normal to the plane of your geometry so that rotation occurs in the plane.) For 2D axisymmetric problems, you will not define the axis: the rotation will always be about the axis, with the origin at (0,0).

To define zone motion for a moving reference frame (MRF), enable the Frame Motion option in the Fluid dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under the Reference Frame tab. For further details on such simulations, see Modeling Flows with Moving Reference Frames.

To define zone motion for a moving (sliding) mesh, enable the Mesh Motion option in the Fluid dialog box. Set the appropriate parameters in the expanded portion of the dialog box, under the Mesh Motion tab. See Setting Up the Sliding Mesh Problem for details.

For cases that do not contain zones with motion specified in a relative frame to another zone, select absolute from the Relative To Cell Zone drop-down list. Here, the velocity and rotation components are specified in an absolute reference frame, which is the default setting, as shown in Figure 7.12: Rotation Specified in the Absolute Reference Frame. If no moving zones are present in the simulation, then absolute will be the only available selection. See The Multiple Reference Frame Model for more information.

Figure 7.12: Rotation Specified in the Absolute Reference Frame

For cases where you have a moving zone specified relative to another moving zone, select the cell zone carrying the primary motion from the Relative To Cell Zone drop-down list under the Reference Frame tab or the Mesh Motion tab. Note that for such cases, Rotation-Axis Origin (Relative) will appear in the interface, signifying coordinates relative to the zone selected from the Relative To Cell Zone drop-down list.

Figure 7.13: Rotation Specified Relative to a Moving Zone illustrates that the rotational axis origin of the small rotating zone is specified relative to the cell zone carrying the primary motion (having local coordinate system ).

Figure 7.13: Rotation Specified Relative to a Moving Zone

For problems that include linear, translational motion of the fluid zone, specify the Translational Velocity by setting the X, Y, and Z components under the Mesh Motion tab. For problems that include rotational motion, specify the rotational Speed under Rotational Velocity. The rotation axis is defined as described above. Note that the speed can be specified as a constant value or a transient profile. The transient profile may be in a file format, as described in Transient Cell Zone and Boundary Conditions, or a UDF macro (DEFINE_TRANSIENT_PROFILE). Specifying the individual velocities as either a profile or a UDF allows you to specify a single component of the frame motion individually. However, you can also specify the frame motion using a user-defined function. This may prove to be quite convenient if you are modeling a more complicated motion of the moving reference frame, where the hooking of many different user-defined functions or profiles can be cumbersome.

Note that when a fluid zone undergoes normal zone motion relative to an adjacent solid zone, energy transfer at that boundary (that is, the total heat transfer rate) includes pressure work when the absolute velocity formulation is used. This pressure work is on the fluid side only, not on the solid side. For details on reporting the total heat transfer rate and/or pressure work rate, see Generating a Flux Report.

See Modeling Flows with Moving Reference Frames for details about modeling flows in moving reference frames. Details about the frame motion UDF can be found in DEFINE_ZONE_MOTION in the Fluent Customization Manual.

If you are using the DO radiation model, you can specify whether or not the fluid zone participates in radiation using the Participates in Radiation option. See Defining Boundary Conditions for Radiation for details.

To define the material contained in the solid zone, select the appropriate item in the Material Name drop-down list. This list will contain all solid materials database) in the Create/Edit Materials Dialog Box. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box.

If you want to define a source of heat within the solid zone, you can do so by enabling the Source Terms option. See Defining Mass, Momentum, Energy, and Other Sources for details.

If you want to fix the value of temperature in the solid zone, rather than computing it during the calculation, you can do so by enabling the Fixed Values option. See Fixing the Values of Variables for details.

If there are rotationally periodic boundaries adjacent to the solid zone and you are not defining zone motion (as described in Defining Zone Motion), you must specify the cell zone axis by defining the Rotation-Axis Origin and Rotation-Axis Direction in the Reference Frame tab.

The cell zone axis is independent of the axis of rotation used by any adjacent wall zones or any other cell zones. For 3D problems, the axis of rotation is the vector from the Rotation-Axis Origin in the direction of the vector given by your Rotation-Axis Direction. For 2D non-axisymmetric problems, you will specify only the Rotation-Axis Origin; the axis of rotation is the -direction vector passing through the specified point. (The direction is normal to the plane of your geometry so that rotation occurs in the plane.) For 2D axisymmetric problems, you will not define the axis: the rotation will always be about the axis, with the origin at (0,0).

When defining motion for a solid zone, you have the following options:

When defining the settings in the Reference Frame tab, Moving Mesh tab, and/or Solid Mesh tab, perform the following steps:

For frame motion and/or solid motion, the velocity must be divergence-free, which requires that the specified motion be tangential to the boundaries. If the motion has a normal component, the solver cannot achieve energy conservation. The only exception, for which normal motion is permitted, is a coupled wall or mesh interface between two solid zones having the same material and motion. The solver will print a warning to the solver transcript the first time it encounters a solid velocity having a significant normal component at any other boundary type. The following examples illustrate valid solid zone motion definitions:

Figure 7.15: Single Rotating Solid Zone

Figure 7.16: Rotating solid zone separated from another fluid or solid zone separated by a surface of revolution.

Figure 7.17: Multiple rotating solid zones having the same material and motion specifications, separated by mesh interfaces or coupled walls.

Figure 7.18: Two solids in contact where one is stationary and the other is moving with translational motion. The translational motion of the moving solid should be described in the Solid Motion tab.

Figure 7.19: Two solids in contact where one is stationary and the other is rotating. The rotational motion of the moving solid should be described in the Solid Motion tab. Both solids may also have rotation about the y-axis described in the Frame Motion tab.

The following examples illustrate invalid frame motion or solid motion definitions for solid zones:

Figure 7.20: Rotating solid with boundaries which are not tangential to the motion.

Figure 7.21: Two solids in contact with some squish. At the contact, the rotational motion has some normal component, so the solver will not achieve global energy conservation. However, the temperature field might still be acceptable for engineering purposes.

Limitations:

If you are using the DO radiation model, you can specify whether or not the solid material participates in radiation using the Participates in Radiation option. See Defining Boundary Conditions for Radiation for details.

In laminar flows through porous media, the pressure drop is typically proportional to velocity and the constant can be considered to be zero. Ignoring convective acceleration and diffusion, the porous media model then reduces to Darcy’s Law:

(7–4)

The pressure drop that Ansys Fluent computes in each of the three (, , ) coordinate directions within the porous region is then

(7–5)

where are the entries in the matrix in Equation 7–1, are the velocity components in the , , and directions, and , , and are the thicknesses of the medium in the , , and directions.

Here, the thickness of the medium (, , or ) is the actual thickness of the porous region in your model. Therefore if the thicknesses used in your model differ from the actual thicknesses, you must make the adjustments in your inputs for .

At high flow velocities, the constant in Equation 7–1 provides a correction for inertial losses in the porous medium. This constant can be viewed as a loss coefficient per unit length along the flow direction, thereby allowing the pressure drop to be specified as a function of dynamic head.

If you are modeling a perforated plate or tube bank, you can sometimes eliminate the permeability term and use the inertial loss term alone, yielding the following simplified form of the porous media equation:

(7–6)

or when written in terms of the pressure drop in the , , directions:

(7–7)

Again, the thickness of the medium (, , or ) is the thickness you have defined in your model.

For simulations in which the porous medium and fluid flow are assumed to be in thermal equilibrium, the conduction flux in the porous medium uses an effective conductivity and the transient term includes the thermal inertia of the solid region on the medium:

(7–12)

where
	= total fluid energy
	= total solid medium energy
	= fluid density
	= solid medium density
	= porosity of the medium
	= effective thermal conductivity of the medium
	= fluid enthalpy source term

The effective thermal conductivity in the porous medium, , is computed by Ansys Fluent as the volume average of the fluid conductivity and the solid conductivity:

(7–13)

where
	= fluid phase thermal conductivity (including the turbulent contribution, )
	= solid medium thermal conductivity

The fluid thermal conductivity and the solid thermal conductivity can be computed via user-defined functions.

The anisotropic effective thermal conductivity can also be specified via user-defined functions. In this case, the isotropic contributions from the fluid, , are added to the diagonal elements of the solid anisotropic thermal conductivity matrix.

For simulations in which the porous medium and fluid flow are not assumed to be in thermal equilibrium, a dual cell approach is used. In such an approach, a solid zone that is spatially coincident with the porous fluid zone is defined, and this solid zone only interacts with the fluid with regard to heat transfer. The conservation equations for energy are solved separately for the fluid and solid zones. The conservation equation solved for the fluid zone is

(7–14)

and the conservation equation solved for the solid zone is

(7–15)

where
	= total fluid energy
	= total solid medium energy
	= fluid density
	= solid medium density
	= porosity of the medium
	= fluid phase thermal conductivity (including the turbulent contribution, )
	= solid medium thermal conductivity
	= heat transfer coefficient for the fluid / solid interface
	= interfacial area density, that is, the ratio of the area of the fluid / solid interface and the volume of the porous zone
	= temperature of the fluid
	= temperature of the solid medium
	= fluid enthalpy source term
	= solid enthalpy source term

The fluid thermal conductivity and the solid thermal conductivity can be computed via user-defined functions.

The source term due to the non-equilibrium thermal model is represented in Equation 7–14 and Equation 7–15 by and , respectively.

Using the physical velocity formulation, and assuming a general scalar , the governing equation in an isotropic porous media has the following form:

(7–17)

Assuming isotropic porosity and single phase flow, the volume-averaged mass and momentum conservation equations are as follows:

(7–18)

(7–19)

The last term in Equation 7–19 represents the viscous and inertial drag forces imposed by the pore walls on the fluid.

You can simulate porous media multiphase flows using the Physical Velocity Porous Formulation to solve the true or physical velocity field throughout the entire flow field, including both porous and non-porous regions. In this approach, assuming a general scalar in the phase, , the governing equation in an isotropic porous medium takes on the following form:

(7–20)

Here is the porosity, which may vary with time and space; is the phase density; is the volume fraction; is the phase velocity vector; is the source term; and is the diffusion coefficient.

The general scalar equation Equation 7–20 applies to all other transport equations in the Eulerian multiphase model, such as the granular phase momentum and energy equations, turbulence modeling equations, and the species transport equations.

Assuming isotropic porosity and multiphase flows, the governing equations in the phase, Equation 14–193, Equation 14–194, and Equation 14–197 in the Theory Guide  take the general forms described below.

 

7.2.3.7.2.1. The Continuity Equation

(7–21)

 

7.2.3.7.2.2. The Momentum Equation

(7–22)

where is capillary pressure for the wetting phase, is phase shear stress, is the body force, and are the mass transfers from phase to phase and vice versa, is the absolute permeability, and is the relative permeability. The term in the brackets is the porous sink, having zero value in non-porous flows/regions. The last two terms includes the general interphase momentum exchange forces: is the drag force for non-porous flows/regions, is the turbulent dispersed force, and are the relative velocity vectors, and , , and are the external body, lift and virtual mass exchange forces. If the capillary pressure model is not enabled, =1.

Details about the user inputs related to the momentum resistance sources can be found in User Inputs for Porous Media.

 

7.2.3.7.2.3. The Energy Equation

(7–23)

where:
	Subscripts , , and denote phase , phase , and the solid material, respectively
	is the total enthalpy
	is the thermal conductivity
	is the heat transfer between phase and phase
	is the density
	is the heat source
	is the phase volume fraction
	is the phase velocity
	and are the total enthalpy differences between phases and and vice versa

As mentioned in Overview, a porous zone is modeled as a special type of fluid zone. To indicate that the fluid zone is a porous region, enable the Porous Zone option in the Fluid dialog box. The dialog box will expand to show the porous media inputs (as shown in Figure 7.22: The Fluid Dialog Box for a Porous Zone).

In a coupled analysis involving Fluent and System Coupling, a porous jump boundary of zero-thickness next to the porous zone can be used to transfer data between the porous zone and the System Coupling system. For more about System Coupling and the variable transferred from a porous jump boundary, see Performing System Coupling Simulations Using Fluent.

The Cell Zone Conditions task page contains a Porous Formulation region where you can instruct Ansys Fluent to use either a superficial or physical velocity in the porous medium simulation. By default, the velocity is set to Superficial Velocity. For details about using the Physical Velocity formulation, see Modeling Porous Media Based on Physical Velocity.

To define the fluid that passes through the porous medium, select the appropriate fluid in the Material Name drop-down list in the Fluid Dialog Box. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box.

If you are modeling species transport with reactions, you can enable reactions in a porous zone by turning on the Reaction option in the Fluid dialog box and selecting a mechanism in the Reaction Mechanism drop-down list.

If your mechanism contains wall surface reactions, you also must specify a value for the Surface-to-Volume Ratio. This value is 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 and the porosity. See Defining Zone-Based Reaction Mechanisms for details about defining reaction mechanisms. See Wall Surface Reactions and Chemical Vapor Deposition for details about wall surface reactions.

For cases involving moving meshes, dynamic meshes or moving reference frames (MRF), the Relative Velocity Resistance Formulation option allows you to better predict porous media sources. The porous media source terms are calculated using relative velocities in the porous zone. For more information, see Momentum Equations for Porous Media. The Relative Velocity Resistance Formulation option works well for cases with moving and stationary porous media. It is turned on by default.

Note the following limitation when using the Relative Velocity Resistance Formulation option:

The viscous and inertial resistance coefficients are both defined in the same manner. The basic approach for defining the coefficients using a Cartesian coordinate system is to define one direction vector (Direction-1 Vector) in 2D or two direction vectors (Direction-1 Vector and Direction-2 Vector) in 3D, and then specify the viscous and/or inertial resistance coefficients in each direction. The Direction-1 Vector usually represents the primary flow direction (parallel to the porous zone axis), and the other two directions represent the transverse directions.

Ansys Fluent automatically determines the second direction vector in 2D or the third direction vector in 3D, which is not explicitly defined:

If the porous zone faces are not aligned with the global Cartesian axis, you can use the plane tool in 3D or the line tool in 2D for the direction vector definitions as further described.

You can also define the viscous and/or inertial resistance coefficients in each direction using a user-defined function (UDF). The user-defined options become available in the corresponding drop-down list when the UDF has been created and loaded into Ansys Fluent. Note that the coefficients defined in the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using user-defined function, see the Fluent Customization Manual.

If you are modeling axisymmetric swirling flows, you can specify an additional direction component for the viscous and/or inertial resistance coefficients. This direction component is always tangential to the other two specified directions. This option is available for both density-based and pressure-based solvers.

In 3D, it is also possible to define the coefficients using a conical (or cylindrical) coordinate system, as described below.

The procedure for defining resistance coefficients is as follows:

Methods for deriving viscous and inertial loss coefficients are described in the sections that follow.

When you use the porous media model, you must remember that the porous cells in Ansys Fluent are 100% open, and that the values that you specify for and/or must be based on this assumption. Suppose, however, that you know how the pressure drop varies with the velocity through the actual device, which is only partially open to flow. The following exercise is designed to show you how to compute a value for which is appropriate for the Ansys Fluent model.

Consider a perforated plate that has 25% area open to flow. The pressure drop through the plate is known to be 0.5 times the dynamic head in the plate. The loss factor, , defined as

(7–25)

is therefore 0.5, based on the actual fluid velocity in the plate, that is, the velocity through the 25% open area. To compute an appropriate value for , note that in the Ansys Fluent model:

Noting item 1, the first step is to compute an adjusted loss factor, , which would be based on the velocity of a 100% open area:

(7–26)

or, noting that for the same flow rate, ,

(7–27)

The adjusted loss factor has a value of 8. Noting item 2, you must now convert this into a loss coefficient per unit thickness of the perforated plate. Assume that the plate has a thickness of 1.0 mm ( m). The inertial loss factor would then be

(7–28)

Note that, for anisotropic media, this information must be computed for each of the 2 (or 3) coordinate directions.

As a second example, consider the modeling of a packed bed. In turbulent flows, packed beds are modeled using both a permeability and an inertial loss coefficient. One technique for deriving the appropriate constants involves the use of the Ergun equation  [42], a semi-empirical correlation applicable over a wide range of Reynolds numbers and for many types of packing:

(7–29)

When modeling laminar flow through a packed bed, the second term in the above equation may be dropped, resulting in the Blake-Kozeny equation   [42]:

(7–30)

In these equations, is the viscosity, is the mean particle diameter, is the bed depth, and is the void fraction, defined as the volume of voids divided by the volume of the packed bed region. Comparing Equation 7–4 and  Equation 7–6 with  Equation 7–29, the permeability and inertial loss coefficient in each component direction may be identified as

(7–31)

and

(7–32)

As a third example we will take the equation of Van Winkle et al. [118] [150] and show how porous media inputs can be calculated for pressure loss through a perforated plate with square-edged holes.

The expression, which is claimed by the authors to apply for turbulent flow through square-edged holes on an equilateral triangular spacing, is

(7–33)

where
	= mass flow rate through the plate
	= the free area or total area of the holes
	= the area of the plate (solid and holes)
	= a coefficient that has been tabulated for various Reynolds-number ranges and for various
	= the ratio of hole diameter to plate thickness

for and for the coefficient takes a value of approximately 0.98, where the Reynolds number is based on hole diameter and velocity in the holes.

Rearranging Equation 7–33, making use of the relationship

(7–34)

and dividing by the plate thickness, , we obtain

(7–35)

where is the superficial velocity (not the velocity in the holes). Comparing with Equation 7–6 is seen that, for the direction normal to the plate, the constant can be calculated from

(7–36)

Consider the problem of laminar flow through a mat or filter pad which is made up of randomly-oriented fibers of glass wool. As an alternative to the Blake-Kozeny equation (Equation 7–30) we might choose to employ tabulated experimental data. Such data is available for many types of fiber  [71].

Volume Fraction of Solid Material	Dimensionless Permeability of Glass Wool
0.262	0.25
0.258	0.26
0.221	0.40
0.218	0.41
0.172	0.80

where and is the fiber diameter. , for use in Equation 7–4, is easily computed for a given fiber diameter and volume fraction.

Experimental data that is available in the form of pressure drop against velocity through the porous component, can be extrapolated to determine the coefficients for the porous media. To effect a pressure drop across a porous medium of thickness, , the coefficients of the porous media are determined in the manner described below.

If the experimental data is:

then an curve can be plotted to create a trendline through these points yielding the following equation

(7–37)

where is the pressure drop and is the velocity.

Note that a simplified version of the momentum equation, relating the pressure drop to the source term, can be expressed as

(7–38)

or

(7–39)

Hence, comparing Equation 7–37 to Equation 7–2, yields the following curve coefficients:

(7–40)

with kg/ , and a porous media thickness, , assumed to be 1 m in this example, the inertial resistance factor, .

Likewise,

(7–41)

with , the viscous inertial resistance factor, .

If you choose to use the power-law approximation of the porous-media momentum source term (Equation 7–3), the only inputs required are the coefficients and . Under Power Law Model in the Fluid dialog box, enter the values for C0 and C1. Note that the power-law model can be used in conjunction with the Darcy and inertia models.

C0 must be in SI units, consistent with the value of C1.

To define the porosity, scroll down below the resistance inputs in the Fluid dialog box, and set the Porosity under Fluid Porosity. Note that the value of the Porosity must be in the range of 0 – 1 ; furthermore, the lower and upper limits (that is, 0 and 1, respectively) are not allowed for the non-equilibrium thermal model.

You can also define the porosity using a user-defined function (UDF). The user-defined option becomes available in the corresponding drop-down list when the UDF has been created and loaded into Ansys Fluent. Note that the porosity defined in the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using user-defined functions, see the separate Fluent Customization Manual.

The porosity, , is the volume fraction of fluid within the porous region (that is, the open volume fraction of the medium). The porosity is used in the prediction of heat transfer in the medium, as described in Treatment of the Energy Equation in Porous Media, and in the time-derivative term in the scalar transport equations for unsteady flow, as described in Effect of Porosity on Transient Scalar Equations. It also impacts the calculation of reaction source terms and body forces in the medium. These sources will be proportional to the fluid volume in the medium. If you want to represent the medium as completely open (no effect of the solid medium), you should set the porosity equal to 1.0 (the default). When the porosity is equal to 1.0, the solid portion of the medium will have no impact on heat transfer or thermal/reaction source terms in the medium.

You can model heat transfer in the porous material, with or without the assumption of thermal equilibrium between the medium and the fluid flow. Note that heat transfer is not available for inviscid flow.

 

7.2.3.8.14.2. Non-Equilibrium Thermal Model

---

Note:  The non-equilibrium thermal model is incompatible with the density-based solver.

---

The assumption of thermal equilibrium between the solid medium and the fluid flow is not appropriate for all simulations, as the presence of different geometric length scales (for example, pore sizes) and physical properties of solid and liquid phases may result in local temperature differences between the phases. Examples of when a non-equilibrium thermal model may be suitable include the simulation of light-off for exhaust after-treatment, fuel cells, catalytic converters, and so on.

The non-equilibrium thermal model available for porous media in Ansys Fluent is based on a dual cell approach. This approach is referred to as “dual cell” because it involves a second solid cell zone that overlaps (that is, is spatially coincident with) the porous fluid zone; the two zones are solved simultaneously and are coupled only through heat transfer. Ansys Fluent can automatically create a solid zone for you that is a duplicate of the porous fluid zone; otherwise, you can create a duplicate cell zone manually using the mesh/modify-zones/copy-move-cell-zone text command before you enable the non-equilibrium thermal model, or make sure that the mesh you read contains two cell zones in the region where the porous medium will be defined. You should ensure that the duplicate zone is defined as a solid zone, and that the two zones have similar levels of mesh refinement (as one-to-one mapping will be employed between the cell centroids of the fluid zone and the solid zone).

---

Important:  When setting up both the porous fluid zone and the overlapping solid zone, note that the non-equilibrium thermal model is not supported for zones that undergo (or are adjacent to zones that undergo) changes to the geometry or mesh, such as dynamic mesh zones or zones that undergo hanging node adaption, utilize the mesh morpher/optimizer, or are involved in fluid-structure interaction (FSI) applications.

---

The instructions that follow assume you have already performed steps 1–7 in User Inputs for Porous Media. Before you enable the non-equilibrium thermal model, click OK in the Fluid dialog box, in order to save your settings in the Porous Zone tab; note that if you do not save your settings, they will be reset to the default values when you enable the non-equilibrium thermal model. Then reopen the Fluid dialog box and scroll down below the resistance inputs in the Porous Zone tab. Select Non-Equilibrium from the Thermal Model list in the Heat Transfer Settings group box (see Figure 7.24: The Heat Transfer Settings Group Box of the Fluid Dialog Box); this will enable the dual cell approach and display the associated GUI input controls. If a solid zone that is spatially coincident with the porous fluid zone does not already exist, use the Question dialog box that opens to automatically create one. The name of the newly created solid cell zone will then be displayed in the Solid Zone text box of the Fluid dialog box.

---

Important:  Note that the Non-Equilibrium option button is not available if a radiation and/or multiphase model is enabled, as such a combination is not supported.

---

Figure 7.24: The Heat Transfer Settings Group Box of the Fluid Dialog Box

Next, define and (as described in Non-Equilibrium Thermal Model Equations) for Interfacial Area Density and Heat Transfer Coefficient, respectively; you can define these settings as a Constant, a New Input Parameter..., or as a user-defined function. The user-defined option becomes available in the corresponding drop-down list when the UDF has been created and loaded into Ansys Fluent. Note that the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using user-defined functions, see the separate Fluent Customization Manual.

When you are finished setting up the porous fluid zone, you should verify that the solid zone created in the previous step has the appropriate settings. Note the name of the zone displayed in the Solid Zone text box of the Heat Transfer Settings group box (see Figure 7.24: The Heat Transfer Settings Group Box of the Fluid Dialog Box), and then double-click that zone in the Zone list of the Cell Zone Conditions task page to open the Solid dialog box. Then, verify that an appropriate selection is made for Material Name. If you want to check or modify the properties of the selected material, you can click Edit... to open the Edit Material dialog box; this dialog box contains just the properties of the selected material, not the full contents of the standard Create/Edit Materials dialog box. You can define the Thermal Conductivity of the solid material using a user-defined function (UDF), in order to define a non-isotropic thermal conductivity. The user-defined option becomes available in the corresponding drop-down list when the UDF has been created and loaded into Ansys Fluent. Note that the non-isotropic thermal conductivity defined in the UDF must utilize the DEFINE_PROPERTY macro. For more information on creating and using user-defined functions, see the separate Fluent Customization Manual.

---

Important:  For transient simulations using the Non-Equilibrium Thermal Model with low porosity (typically < 0.2), it is recommended to increase the Solid Time Step Size as described in Specifying the Solid Time Step Size. A value ~1s or the Automatic option can help with solution stability and convergence.

---

Note that when postprocessing simulations that utilize the non-equilibrium thermal model, you can display the energy source due to the temperature difference between the fluid and solid zones using the Non-Equilibrium Thermal Model Source variable in the Temperature... category. Furthermore, attention must be paid to the fact that there are overlapping cell zones (that is, a fluid and a solid zone) in the porous region. For example:

• When creating an isosurface and making selections from the From Zones selection list of the Iso-Surface dialog box, you should never select both the porous fluid zone and the overlapping solid zone at the same time. Note that if no selections are made in this list, then all the cell zones are selected.

• When making selections from the Surfaces list of the Contours dialog box, you should not select a surface that is associated with the porous fluid zone and a surface associated with the overlapping solid zone at the same time, if those surfaces are spatially coincident.

• When postprocessing the thermal conductivity property in the porous region, the value that is reported for the fluid zone is the thermal conductivity of the fluid material scaled by the porosity () and for the overlapping solid zone the value reported is the thermal conductivity of the solid zone scaled by the complement of the porosity (); where is the porosity, is the fluid phase thermal conductivity (including the turbulent contribution, ), and is the solid medium thermal conductivity.

The relative viscosity can be used to account for the effect of the porous media on the diffusion term in the momentum equation. By default, the relative viscosity is set to a constant value of 1 (that is, the effective viscosity is equal to the molecular viscosity). You can choose to model the relative viscosity using one of the models described in Relative Viscosity in Porous Media, or you can specify a user-defined function using a DEFINE_PROPERTY macro.

When you define multiple porous zones, the last value you enter for the relative viscosity will be applied to compute the effective viscosity for all porous zones in your simulation. If you want to simulate different effective viscosities in different porous zones, specify the Viscosity property of the porous material directly via user-defined function using the DEFINE_PROPERTY macro (in the Create/Edit Materials dialog box).

The relative permeability of a phase denotes its ability to transmit the phase material when its saturation (volume fraction) is less than 100%.

Reservoir engineers often resort to empirical models or measurement curves to determine the relative and, therefore, the effective permeabilities. In Fluent, the Corey power law model [27] is available to account for the relative permeability for the two-phase flow through porous media. The Corey correlations of the relative permeability can be represented as follows:

(7–42)

where:
	is the reference phase relative permeability
	is the normalized saturation in the q th phase
	is the Corey exponent for the q th phase

In Fluent the phase saturation is the phase volume fraction. Thus can be expressed as:

(7–43)

where and are the volume fraction and the volume fraction residual in the q ^th phase, respectively.

For the two-phase oil-water flow in a water-wet-system, the relative permeabilities can be obtained from:

(7–44)

where:

Subscripts and refer to the water and oil phases, respectively

and are the reference phase relative permeabilities for the wetting and non-wetting phases, respectively

and are the Corey exponents for the two phases

The Corey correlation is often used for approximation of the relative permeabilities, particularly for water flooding type scenarios. The relative permeability curves of the oil (or the non-wetting phase) is usually an S-shaped curve and of the water (or the wetting phase) is a concave upward curve.

Alternatively, if relative permeability data for one or two phases are available as tabular functions of other solution variables, you can use generic text files to input such data to define phase relative permeability as described in Reading Files in Tabular Format.

To model the relative permeability in Ansys Fluent:

On rare occasions, the saturation may still fall below residual saturation. You can fix the affected phase to its residual saturation and allow the other phase to pass through normally by issuing the following text commands:

solve/set/multiphase-numerics/porous-media/relative-permeability

enable fix option below residual saturation? [no] yes

When using the Eulerian multiphase model, you can optionally specify a sub-model for capillary pressure.

When two or more phases are present in pores, one of the phase (usually water) has a preference for the pore surfaces. This phase is referred to as the wetting phase, while the other phase is called the non-wetting phase. The boundary between the phases present in a porous medium is also curved, due to interfacial tension between the fluid, and this gives rise to a difference in the pressure across the interface:

(7–45)

where and are the non-wetting and wetting phase pressures, respectively. The difference, is the capillary pressure. It presents a significant driving force under the conditions of low flow pressure and high volume fraction.

At the pore scale, capillary pressure depends primarily on the pore geometric characteristics (sizes, distributions, etc.), interfacial tensions and wettability (contact angles). At the Macro scale the capillary pressure is generally assumed to be a function of the saturation of the wetting fluid:

(7–46)

Its value is often obtained either by measurements or correlations.

 

7.2.3.8.17.1. Brooks-Corey Model

The Brooks-Corey model [27] proposed the following relationship for capillary pressure for primary drainage, in which the porous media initially saturated with water is invaded with oil phase:

(7–47)

where is the resulting normalized (effective) saturation:

(7–48)

where and are the minimum and maximum volume fraction (saturation) values, respectively. By default and where is the residual saturation of phase The value of is limited to values greater than 0.001 in order to avoid an infinite value for capillary pressure.

In order to solve Equation 7–47, the entry pressure, , and the parameter related to the pore size are required. The default values in Fluent are and which are appropriate for air-water flow in sand [29].

 

7.2.3.8.17.2. Van-Genuchten Model

Another well established parametric model was proposed by van Genuchten [48]:

(7–49)

where is the entry pressure. is the pore size distribution and . The default values inFluent are and which are appropriate for air-water flow in sand [29].

 

7.2.3.8.17.3. Leverett J-Function

The J-function was developed by Leverett in an attempt to extend the pore-scale capillary pressure formulation by Washburn [29] to a Macro-scale capillary pressure model. Leverett proposed that the averaged pore radius can be expressed in terms of porosity and permeability:

(7–50)

Furthermore, he acknowledged that the capillary pressure should depend on porosity and permeability. By analogy to the Washburn equation, he developed a dimensionless J-function [85]:

(7–51)

(7–52)

where is the surface tension, is the wetting or contact angle, and and are fitting parameters. Various empirical J-functions can be developed to estimate capillary pressure. In the Fluent, the following formulation is used:

(7–53)

This is the same formulation as is used in the Fluent Fuel Cell Module (see Liquid Water Formation, Transport, and its Effects (Low-Temperature PEMFC Only) in the Fluent Theory Guide).

 

7.2.3.8.17.4. Skjaeveland Model

All of the above-mentioned capillary pressure models (Brooks-Corey, Van-Genuchten, Leverett J-Function) are limited to primary drainage processes. Water saturation decreases in a primary drainage process. To model a displacement process where flooding is important, such as water-drive, models that describe imbibition are required. However, most reservoirs are mixed wettabilty and for these systems a more comprehensive model that describes both drainage and imbibition processes is required. The Skjaeveland model for capillary pressure encompasses these features.

The Skjaeveland model [145] for capillary pressure treats the two fluids symmetrically for wettability. The Skjaeveland capillary pressure curve is defined by Equation 7–54.

(7–54)

Where is the capillary pressure of the phase, and are fitting parameters, and are constants, and and are the volume fractions of the two phases. and subscripts refer to wetting and non-wetting phases, respectively.

The positive part of the capillary pressure curve is defined by and . and define the negative portion of the capillary pressure curve. The effects of varying , , , and on the capillary pressure curve are shown in Figure 7.27: Skjaeveland Correlation Behavior [145].

Figure 7.27: Skjaeveland Correlation Behavior

Figure 7.27: Skjaeveland Correlation Behavior shows that there is a lot of flexibility in the capillary pressure curve. You can add further flexibility to the capillary pressure curve by estimating the residual oil saturation. Note that by varying and you can modify the cross-over point (while keeping and unchanged).

Parameter	Default Value
	9.e5
	9.e5
	0.05
	0.05

Default-Skjaevland-Model
Sw          Pc
0.2122      195399.0883
0.2245      156423.6016
0.2367      134012.8962
0.249       117936.4991
0.2612      105469.0929
0.2735      95079.83957
0.2857      86245.04955
0.298       78405.02466

 

7.2.3.8.17.7. Modeling Capillary Pressure as Diffusion

By default, the capillary pressure term is included as a source in the wetting phase momentum equation as shown in Equation 7–22. For two-phase cases, you can use an alternative approach where capillary pressure is modeled as a diffusion term in the wetting phase continuity equation. This approach provides numerical robustness and stability for certain cases.

The gradient of capillary pressure is expressed as a function of the wetting phase saturation :

(7–55)

The calculation of the gradient of capillary pressure with respect to the wetting phase volume fraction can be done analytically.

To model capillary pressure as diffusion, issue the following text command:

solve/set/multiphase-numerics/porous-media/capillary-pressure-as-diffusion?
model capillary pressure as diffusion? [no] yes

---

Note:

• When modeling the capillary pressure as diffusion, the secondary phase must be the wetting phase.

• Regardless of whether the flow is laminar or turbulent, Ansys Fluent uses only the viscous resistance in the calculation of capillary pressure gradient.

---

If you want to include effects of the heat generated by the porous medium in the energy equation, enable the Source Terms option and set a nonzero Energy source. For porous media, energy source terms on the solid and gas sides are applied exactly as entered with no adjustment for porosity. A source term of 100 W/m ³ specified for a solid zone of volume 1.0 m ³ will, therefore, deliver 100 W even if the solids make up only 60% of that volume. You may also define sources of mass, momentum, turbulence, species, or other scalar quantities, as described in Defining Mass, Momentum, Energy, and Other Sources.

If you want to fix the value of one or more variables in the fluid region of the zone, rather than computing them during the calculation, you can do so by enabling the Fixed Values option. See Fixing the Values of Variables for details.

As discussed in Treatment of Turbulence in Porous Media, turbulence will be computed in the porous region just as in the bulk fluid flow. If you are using one of the turbulence models (other than the Large Eddy Simulation model) and you want the turbulence generation to be zero in the porous zone, turn on the Laminar Zone option in the Fluid dialog box. Refer to Specifying a Laminar Zone for more information about suppressing turbulence generation.

Inputs for the rotation axis and zone motion are the same as for a standard fluid zone. See Inputs for Fluid Zones for details.

After enabling the 3D Fan Zone option in the Fluid dialog box, you can begin setting it up by defining the settings in the Geometry group box in the 3D Fan Zone tab of the fluid cell zone:

To complete the setup of a 3D fan zone, you must define the settings in the Properties group box in the 3D Fan Zone tab of the fluid cell zone:

The variables that can be fixed include velocity components (pressure-based solver only), turbulence quantities, temperature (pressure-based solver only), enthalpy, species mass fractions (pressure-based solver only), and user-defined scalars. For turbulence quantities, different values can be set depending on your choice of turbulence model. You can fix the value of the temperature in a fluid or solid zone if you are solving the energy equation. If you are using the non-premixed combustion model, you can fix the enthalpy in a fluid zone. If you have more than one species in your model, you can specify fixed values for the species mass fractions for each individual species except the last one you defined. See the Fluent Customization Manual for details about defining user-defined scalars.

If you are using the Eulerian multiphase model, you can fix the values of velocity components and (depending on which multiphase turbulence model you are using) turbulence quantities on a per-phase basis. See Eulerian Model for details about setting boundary conditions for Eulerian multiphase calculations.

To fix the velocity components, you can specify X, Y, and (in 3D) Z Velocity values, or, for axisymmetric cases, Axial, Radial, and (for axisymmetric swirl) Swirl Velocity values. The units for a fixed velocity are m/s.

For 3D cases, you can choose to specify cylindrical velocity components instead of Cartesian components. Turn on the Local Coordinate System For Fixed Velocities option, and then specify the Axial, Radial, and/or Tangential Velocity values. The local coordinate system is defined by the Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See Specifying the Rotation Axis for information about setting these parameters. (Note that it is acceptable to specify the rotation axis and direction for a non-rotating zone. This will not cause the zone to rotate; it will not rotate unless it has been explicitly defined as a moving zone.)

If you are solving the energy equation, you can fix the temperature in a zone by specifying the value of the Temperature. The units for a fixed temperature are K.

If you are using the non-premixed combustion model, you can fix the enthalpy in a zone by specifying the value of the Enthalpy. The units for a fixed enthalpy are J/kg.

If you specify a radial-type profile (see Profile Specification Types) for temperature or enthalpy, the local coordinate system upon which the radial profile is based is defined by the Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See above for details.

If you are using the species transport model, you can fix the values of the species mass fractions for individual species. Ansys Fluent allows you to fix the species mass fraction for each species (for example, h2, o2) except the last one you defined.

If you specify a radial-type profile (see Profile Specification Types) for a species mass fraction, the local coordinate system upon which the radial profile is based is defined by the Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See above for details.

To fix the values of and in the -  equations, specify the Turbulence Kinetic Energy and Turbulence Dissipation Rate values. The units for are / and those for are /.

To fix the value of the modified turbulent viscosity () for the Spalart-Allmaras model, specify the Modified Turbulent Viscosity value. The units for the modified turbulent viscosity are /s.

To fix the values of and in the -  equations, specify the Turbulence Kinetic Energy and Specific Dissipation Rate values. The units for are / and those for are 1/s.

To fix the value of , , or the Reynolds stresses in the RSM transport equations, specify the Turbulence Kinetic Energy, Turbulence Dissipation Rate, Specific Dissipation Rate, UU Reynolds Stress, VV Reynolds Stress, WW Reynolds Stress, UV Reynolds Stress, VW Reynolds Stress, and/or UW Reynolds Stress. The units for and the Reynolds stresses are /, and those for are /.

If you specify a radial-type profile (see Profile Specification Types) for , , , or , the local coordinate system upon which the radial profile is based is defined by the Rotation-Axis Origin and Rotation-Axis Direction for the fluid zone. See above for details. Note that you cannot specify radial-type profiles for the Reynolds stresses.

To fix the value of a user-defined scalar, specify the User-defined scalar-n value. (There will be one for each user-defined scalar you have defined.) The units for a user-defined scalar will be the appropriate SI units for the scalar quantity. See the Fluent Customization Manual for information on user-defined scalars.

If you have only one species in your problem, you can simply define a Mass source for that species. The units for the mass source are . In the continuity equation (Equation 1–1 in the Theory Guide), the defined mass source will appear in the term.

If you have more than one species, you can specify mass sources for each individual species. There will be a total Mass source term as well as a source term listed explicitly for each species (for example, h2, o2) except the last one you defined. If the total of all species mass sources (including the last one) is 0, then you should specify a value of 0 for the Mass source, and also specify the values of the nonzero individual species mass sources. Since you cannot specify the mass source for the last species explicitly, Ansys Fluent will compute it by subtracting the sum of all other species mass sources from the specified total Mass source.

For example, if the mass source for hydrogen in a hydrogen-air mixture is 0.01, the mass source for oxygen is 0.02, and the mass source for nitrogen (the last species) is 0.015, you will specify a value of 0.01 in the h2 field, a value of 0.02 in the o2 field, and a value of 0.045 in the Mass field. This concept also applies within each cell if you use user-defined functions for species mass sources.

The units for the species mass sources are . In the conservation equation for a chemical species (Equation 7–1 in the Theory Guide), the defined mass source will appear in the term.

To define a source of momentum, specify the X Momentum, Y Momentum, and/or Z Momentum term. The units for the momentum source are N/ . In the momentum equation (Equation 1–3 in the Theory Guide), the defined momentum source will appear in the term.

To define a source of energy, specify an Energy term. The units for the energy source are W/ . In the energy equation (Equation 5–1 in the Theory Guide), the defined energy source will appear in the term.

To define a source of the mean mixture fraction or its variance for the non-premixed combustion model, specify the Mean Mixture Fraction or Mixture Fraction Variance term. The units for the mean mixture fraction source are , and those for the mixture fraction variance source are .

The defined mean mixture fraction source will appear in the term in the transport equation for the mixture fraction (Equation 8–4 in the Theory Guide).

The defined mixture fraction variance source will appear in the term in the transport equation for the mixture fraction variance (Equation 8–5 in the Theory Guide).

If you are using the two-mixture-fraction approach, you can also specify sources of the Secondary Mean Mixture Fraction and Secondary Mixture Fraction Variance.

To define a source for the P-1 radiation model, specify the P1 term. The units for the radiation source are W/ , and the defined source will appear in the term in Equation 5–57 in the Theory Guide.

Note that, if the source term you are defining represents a transfer from internal energy to radiative energy (for example, absorption or emission), you must specify an Energy source of the same magnitude as the P1 source, but with the opposite sign, in order to ensure overall energy conservation.

To define a source of the progress variable for the premixed combustion model, specify the Progress Variable term. The units for the progress variable source are kg/ -s, and the defined source will appear in the term in Equation 8–70 in the Theory Guide.

To define a source of NO, HCN, or for the NOx model, specify the no, hcn, or nh3 term. The units for these sources are kg/ -s, and the defined sources will appear in the , , and terms of Equation 9–1, Equation 9–2, and Equation 9–3 in the Theory Guide.

For the Discrete and Inhomogeneous Discrete population balance models, you can specify Bin-i-fraction source terms (where i is the bin label). Note that bins are labeled from 0 to , where is the number of bins that you specified in the Population Balance Model tab of the Multiphase Model dialog box. The units for the fraction source are kg/m³ s.

You can specify source term(s) for each UDS transport equation you have defined in your model. See Setting Up UDS Equations in Ansys Fluent for details.