When you are modeling a porous region, the only additional inputs for the problem setup are as follows. Optional inputs are indicated as such.
Methods for determining the resistance coefficients and/or permeability are presented below. If you choose to use the power-law approximation of the porous-media momentum source term, you will enter the coefficients and in Equation 7.19-3 instead of the resistance coefficients and flow direction.
You will set all parameters for the porous medium in the Fluid panel (Figure 7.19.1), which is opened from the Boundary Conditions panel (as described in Section 7.1.4).
Defining the Porous Zone
As mentioned in Section 7.1, 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 panel. The panel will expand to show the porous media inputs (as shown in Figure 7.19.1).
Defining the Porous Velocity Formulation
The Solver panel contains a Porous Formulation region where you can instruct 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 Section 7.19.7.
Defining the Fluid Passing Through the Porous Medium
To define the fluid that passes through the porous medium, select the appropriate fluid in the Material Name drop-down list in the Fluid panel. If you want to check or modify the properties of the selected material, you can click Edit... to open the Material panel; this panel contains just the properties of the selected material, not the full contents of the standard Materials panel.
| If you are modeling species transport or multiphase flow, the
Material Name list will not appear in the
Fluid panel. For species calculations, the mixture material for all fluid/porous zones will be the material you specified in the
Species Model panel. For multiphase flows, the materials are specified when you define the phases, as described in Section
Enabling Reactions in a Porous Zone
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 panel and selecting a mechanism in the Reaction Mechanism drop-down list.
If your mechanism contains wall surface reactions, you will also need to 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, FLUENT can calculate the total surface area on which the reaction takes place in each cell by multiplying by the volume of the cell. See Section 14.1.4 for details about defining reaction mechanisms. See Section 14.2 for details about wall surface reactions.
Including the Relative Velocity Resistance Formulation
Prior to FLUENT 6.3, cases with moving reference frames used the absolute velocities in the source calculations for inertial and viscous resistance. This approach has been enhanced so that relative velocities are used for the porous source calculations (Section 7.19.2). Using the Relative Velocity Resistance Formulation option (turned on by default) allows you to better predict the source terms for cases involving moving meshes or moving reference frames (MRF). This option works well in cases with non-moving and moving porous media. Note that FLUENT will use the appropriate velocities (relative or absolute), depending on your case setup.
Defining the Viscous and Inertial Resistance Coefficients
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 in 2D or two direction vectors in 3D, and then specify the viscous and/or inertial resistance coefficients in each direction. In 2D, the second direction, which is not explicitly defined, is normal to the plane defined by the specified direction vector and the direction vector. In 3D, the third direction is normal to the plane defined by the two specified direction vectors. For a 3D problem, the second direction must be normal to the first. If you fail to specify two normal directions, the solver will ensure that they are normal by ignoring any component of the second direction that is in the first direction. You should therefore be certain that the first direction is correctly specified.
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 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 separate UDF 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.
| Note that the viscous and inertial resistance coefficients are generally based on the superficial velocity of the fluid in the porous media.
The procedure for defining resistance coefficients is as follows:
For some problems in which the principal axes of the porous medium are not aligned with the coordinate axes of the domain, you may not know a priori the direction vectors of the porous medium. In such cases, the plane tool in 3D (or the line tool in 2D) can help you to determine these direction vectors.
For some problems in which the axis of the conical filter element is not aligned with the coordinate axes of the domain, you may not know a priori the direction vector of the cone axis and coordinates of a point on the cone axis. In such cases, the plane tool can help you to determine the cone axis vector and point coordinates. One method is as follows:
An alternate method is as follows:
Under Inertial Resistance, specify the inertial resistance coefficient in each direction. (You will need to scroll down with the scroll bar to view these inputs.)
For porous media cases containing highly anisotropic inertial resistances, enable Alternative Formulation under Inertial Resistance. The Alternative Formulation option provides better stability to the calculation when your porous medium is anisotropic. The pressure loss through the medium depends on the magnitude of the velocity vector of the ith component in the medium. Using the formulation of Equation 7.19-6 yields the expression below:
Whether or not you use the Alternative Formulation option depends on how well you can fit your experimentally determined pressure drop data to the FLUENT model. For example, if the flow through the medium is aligned with the grid in your FLUENT model, then it will not make a difference whether or not you use the formulation.
For more infomation about simulations involving highly anisotropic porous media, see Section 7.19.8.
| Note that the alternative formulation is compatible only with the pressure-based solver.
If you are using the Conical specification method, 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.
In 3D there are three possible categories of coefficients, and in 2D there are two:
Methods for deriving viscous and inertial loss coefficients are described in the sections that follow.
Deriving Porous Media Inputs Based on Superficial Velocity, Using a Known Pressure Loss
When you use the porous media model, you must keep in mind that the porous cells in 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 FLUENT model.
Consider a perforated plate which 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
is therefore 0.5, based on the actual fluid velocity in the plate, i.e., the velocity through the 25% open area. To compute an appropriate value for , note that in the 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:
or, noting that for the same flow rate, ,
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 (10 m). The inertial loss factor would then be
Note that, for anisotropic media, this information must be computed for each of the 2 (or 3) coordinate directions.
Using the Ergun Equation to Derive Porous Media Inputs for a Packed Bed
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 [ 98], a semi-empirical correlation applicable over a wide range of Reynolds numbers and for many types of packing:
When modeling laminar flow through a packed bed, the second term in the above equation may be dropped, resulting in the Blake-Kozeny equation [ 98]:
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 Equations 7.19-4 and 7.19-6 with 7.19-15, the permeability and inertial loss coefficient in each component direction may be identified as
Using an Empirical Equation to Derive Porous Media Inputs for Turbulent Flow Through a Perforated Plate
As a third example we will take the equation of Van Winkle et al. [ 279, 339] 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
|=||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 7.19-19, making use of the relationship
and dividing by the plate thickness, , we obtain
where is the superficial velocity (not the velocity in the holes). Comparing with Equation 7.19-6 it is seen that, for the direction normal to the plate, the constant can be calculated from
Using Tabulated Data to Derive Porous Media Inputs for Laminar Flow Through a Fibrous Mat
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 7.19-16) we might choose to employ tabulated experimental data. Such data is available for many types of fiber [ 158].
| volume fraction of
| dimensionless permeability
of glass wool
where and is the fiber diameter. , for use in Equation 7.19-4, is easily computed for a given fiber diameter and volume fraction.
Deriving the Porous Coefficients Based on Experimental Pressure and Velocity Data
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:
|Velocity (m/s)||Pressure Drop (Pa)|
then an curve can be plotted to create a trendline through these points yielding the following equation
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
Hence, comparing Equation 7.19-23 to Equation 7.19-2, yields the following curve coefficients:
with kg/m , and a porous media thickness, , assumed to be 1m in this example, the inertial resistance factor, .
with , the viscous inertial resistance factor, .
| Note that this same technique can be applied to the porous jump boundary condition. Similar to the case of the porous media, you have to take into account the thickness of the medium
. Your experimental data can be plotted in an
curve, yielding an equation that is equivalent to Equation
7.22-1. From there, you can determine the permeability
and the pressure jump coefficient
Using the Power-Law Model
If you choose to use the power-law approximation of the porous-media momentum source term (Equation 7.19-3), the only inputs required are the coefficients and . Under Power Law Model in the Fluid panel, 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 panel, and set the Porosity under Fluid Porosity.
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 FLUENT. Note that the porosity defined in the UDF must utilize the DEFINE_PROFILE macro. For more information on creating and using user-defined function, see the separate UDF Manual.
The porosity, , is the volume fraction of fluid within the porous region (i.e., the open volume fraction of the medium). The porosity is used in the prediction of heat transfer in the medium, as described in Section 7.19.3, and in the time-derivative term in the scalar transport equations for unsteady flow, as described in Section 7.19.5. 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.
Defining the Porous Material
If you choose to model heat transfer in the porous medium, you must specify the material contained in the porous medium.
To define the material contained in the porous medium, scroll down below the resistance inputs in the Fluid panel, and select the appropriate solid in the Solid Material Name drop-down list under Fluid Porosity. If you want to check or modify the properties of the selected material, you can click Edit... to open the Material panel; this panel contains just the properties of the selected material, not the full contents of the standard Materials panel. In the Material panel, you can define the non-isotropic thermal conductivity of the porous material 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 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 function, see the separate UDF Manual.
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 non-zero Energy source. The solver will compute the heat generated by the porous region by multiplying this value by the total volume of the cells comprising the porous zone. You may also define sources of mass, momentum, turbulence, species, or other scalar quantities, as described in Section 7.28.
Defining Fixed Values
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 Section 7.27 for details.
Suppressing the Turbulent Viscosity in the Porous Region
As discussed in Section 7.19.4, turbulence will be computed in the porous region just as in the bulk fluid flow. If you are using one of the turbulence models (with the exception of the Large Eddy Simulation (LES) Model), and you want the turbulence generation to be zero in the porous zone, turn on the Laminar Zone option in the Fluid panel. Refer to Section 7.17.1 for more information about suppressing turbulence generation.
Specifying the Rotation Axis and Defining Zone Motion
Inputs for the rotation axis and zone motion are the same as for a standard fluid zone. See Section 7.17.1 for details.