The porous media model can be used for a wide variety of single phase and multiphase problems, including flow through packed beds, filter papers, perforated plates, flow distributors, and tube banks. When you use this model, you define a cell zone in which the porous media model is applied and the pressure loss in the flow is determined via your inputs as described in Momentum Equations for Porous Media. Heat transfer through the medium can also be represented, with or without the assumption of thermal equilibrium between the medium and the fluid flow (as described in Treatment of the Energy Equation in Porous Media).
A 1D simplification of the porous media model, termed the “porous jump,” can be used to model a thin membrane with known velocity/pressure-drop characteristics. The porous jump model is applied to a face zone, not to a cell zone, and should be used (instead of the full porous media model) whenever possible because it is more robust and yields better convergence. See Porous Jump Boundary Conditions for details.
The porous media model incorporates an empirically determined flow resistance in a region of your model defined as “porous”. In essence, the porous media model adds a momentum sink in the governing momentum equations. Consequently, the following modeling assumptions and limitations should be readily recognized:
Since the volume blockage that is physically present is not represented in the model, by default ANSYS Fluent uses and reports a superficial velocity inside the porous medium, based on the volumetric flow rate, to ensure continuity of the velocity vectors across the porous medium interface. This superficial velocity formulation does not take porosity into account when calculating the convection and diffusion terms of the transport equations. You can choose to use a more accurate alternative, in which the true (physical) velocity is calculated inside the porous medium and porosity is included in the differential terms of the transport equations. See Modeling Porous Media Based on Physical Velocity for details. In a multiphase flow system, all phases share the same porosity.
The effect of the porous medium on the turbulence field is only approximated. See Treatment of Turbulence in Porous Media for details.
In general, the ANSYS Fluent porous medium model, for both single phase and multiphase, assumes the porosity is isotropic, and it can vary with space and time.
The Superficial Velocity Formulation and the Physical Velocity Formulation are available for multiphase porous media. See User Inputs for Porous Media for details.
The porous media momentum resistance and heat source terms are calculated separately on each phase. See Momentum Equations for Porous Media for details.
A unique pressure interpolation scheme is always used inside porous media zones regardless of the pressure scheme selected in the Solution Methods task page.
The interactions between a porous medium and shock waves are not considered.
When applying the porous media model in a moving reference frame, ANSYS Fluent will either apply the relative reference frame or the absolute reference frame when you enable the Relative Velocity Resistance Formulation. This allows for the correct prediction of the source terms.
Standard Initialization is the recommended initialization method for porous media simulations. The default Hybrid Initialization method does not account for the porous media properties, and depending on boundary conditions, may produce an unrealistic initial velocity field. For porous media simulations, the Hybrid Initialization method can only be used if the Maintain Constant Velocity Magnitude option is selected in the Hybrid Initialization dialog box.
The porous media models for single phase flows and multiphase flows use the Superficial Velocity Porous Formulation as the default. ANSYS Fluent calculates the superficial phase or mixture velocities based on the volumetric flow rate in a porous region. The porous media model is described in the following sections for single phase flow, however, it is important to note the following for multiphase flow:
In the Eulerian multiphase model (Eulerian Model Theory in the Theory Guide), the general porous media modeling approach, physical laws, and equations described below are applied to the corresponding phase for mass continuity, momentum, energy, and all the other scalar equations.
The Superficial Velocity Porous Formulation generally gives good representations of the bulk pressure loss through a porous region. However, since the superficial velocity values within a porous region remain the same as those outside the porous region, it cannot predict the velocity increase in porous zones and therefore limits the accuracy of the model.
Porous media are modeled by the addition of a momentum source term to the standard fluid flow equations. The source term is composed of two parts: a viscous loss term (Darcy, the first term on the right-hand side of Equation 6–1, and an inertial loss term (the second term on the right-hand side of Equation 6–1)
(6–1) |
where is the source term for the
th (
,
, or
) momentum equation,
is the magnitude
of the velocity and
and
are prescribed matrices. This momentum sink contributes
to the pressure gradient in the porous cell, creating a pressure drop
that is proportional to the fluid velocity (or velocity squared) in
the cell.
To recover the case of simple homogeneous porous media
(6–2) |
where is the permeability and
is the inertial resistance factor, simply specify
and
as diagonal matrices with
and
, respectively,
on the diagonals (and zero for the other elements).
ANSYS Fluent also allows the source term to be modeled as a power law of the velocity magnitude:
(6–3) |
where and
are user-defined empirical coefficients.
Important: In the power-law model, the pressure drop is isotropic and the
units for are SI.
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:
(6–4) |
The pressure drop that ANSYS Fluent computes in each of the three
(,
,
) coordinate directions within the porous region
is then
(6–5) |
where are the entries in
the matrix
in Equation 6–1,
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 6–1 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:
(6–6) |
or when written in terms of the pressure drop in the ,
,
directions:
(6–7) |
Again, the thickness of the medium (,
, or
) is the thickness you have defined in your model.
For viscous flows, an effective viscosity, , is introduced to account for the effect of the
porous medium on the diffusion term in the momentum equations:
(6–8) |
where is the fluid viscosity and
is the relative viscosity. In Fluent the following
sub-models are implemented to calculate the relative viscosity. The
effective viscosity is then calculated from Equation 6–8.
ANSYS Fluent solves the standard energy transport equation (Equation 5–1 in the Theory Guide) in porous media regions with modifications to the conduction flux and the transient terms only.
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:
(6–12) |
| where | |
| | |
| | |
| | |
| | |
| | |
| | |
| |
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:
(6–13) |
| where | |
| | |
| |
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
(6–14) |
and the conservation equation solved for the solid zone is
(6–15) |
| where | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| | |
| |
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 6–14 and Equation 6–15 by and
, respectively.
ANSYS Fluent will, by default, solve the standard conservation equations for turbulence quantities in the porous medium. In this default approach, turbulence in the medium is treated as though the solid medium has no effect on the turbulence generation or dissipation rates. This assumption may be reasonable if the medium’s permeability is quite large and the geometric scale of the medium does not interact with the scale of the turbulent eddies. In other instances, however, you may want to suppress the effect of turbulence in the medium.
If you are using one of the turbulence models (with the exception of the Large Eddy Simulation (LES) model), you can suppress the effect of turbulence in a porous region by enabling the Laminar Zone option in the Fluid Dialog Box. Refer to Specifying a Laminar Zone for details about using the Laminar Zone option.
For transient porous media calculations, the effect of porosity
on the time-derivative terms is accounted for in all scalar transport
equations and the continuity equation. When the effect of porosity
is taken into account, the time-derivative term becomes , where
is the scalar quantity
(
,
, and so on) and
is the porosity.
The effect of porosity is enabled automatically for transient calculations, and the porosity is set to 1 by default.
When you are modeling a porous region, the additional inputs for the problem setup are as follows. Optional inputs are indicated as such.
Define the porous zone (as described in Defining the Porous Zone).
(optional) Define the porous velocity formulation in the Cell Zone Conditions task page (as described in Defining the Porous Velocity Formulation).
Identify the fluid material flowing through the porous medium (as described in Defining the Fluid Passing Through the Porous Medium).
Enable reactions for the porous zone, if appropriate, and select the reaction mechanism (as described in Enabling Reactions in a Porous Zone).
Enable the Relative Velocity Resistance Formulation. By default, this option is already enabled and takes the moving porous media into consideration (as described in Including the Relative Velocity Resistance Formulation).
Set the viscous resistance coefficients ( in Equation 6–1, or
in Equation 6–2) and the inertial resistance coefficients (
in Equation 6–1, or
in Equation 6–2), and define the direction vectors for which they apply. Alternatively, specify the coefficients for the power-law model. (See Defining the Viscous and Inertial Resistance Coefficients for more details.)
Specify the porosity of the porous medium (as described in Defining Porosity).
(optional) Specify the settings for heat transfer (as described in Specifying the Heat Transfer Settings).
(optional) Specify a model for relative viscosity (as described in Specifying the Relative Viscosity).
(optional, Eulerian multiphase models only) Specify relative permeability (as described in Specifying the Relative Permeability.
(optional) Set the volumetric heat generation rate in the non-solid portion of the porous medium (or any other sources, such as mass or momentum). (See Defining Sources for more details.)
(optional) Set any fixed values for solution variables in the fluid region (as described in Defining Fixed Values.
Suppress the turbulent viscosity in the porous region, if appropriate. (See Suppressing the Turbulent Viscosity in the Porous Region for more details.)
Specify the rotation axis and/or zone motion, if relevant. (See Specifying the Rotation Axis and Defining Zone Motion for more details.)
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 6–3 instead of the resistance coefficients
and flow direction.
You will set all parameters for the porous medium in the Fluid Dialog Box (Figure 6.12: The Fluid Dialog Box for a Porous Zone), which is opened from the Cell Zone Conditions task page (as described in Setting Cell Zone and Boundary Conditions).
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 6.12: 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 in Workbench.
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 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.
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/porous 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.
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. 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 relative velocity resistance formulation is not supported with axisymmetric-swirl when there are non-zero swirl resistances.
Note: In ANSYS Fluent 6.3, this option was only supported for moving mesh and MRF (with the exception of power law for modeling porous sources). Currently, this option also supports dynamic mesh and takes care of proper treatment of porous sources using power law.
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 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.
Important: 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:
Define the direction vectors.
To use a Cartesian coordinate system, simply specify the Direction-1 Vector and, for 3D, the Direction-2 Vector. The unspecified direction will be determined as described above. These direction vectors correspond to the principle axes of the porous media.
Note: The units for the inertial resistance coefficients (Direction-1 Vector and Direction-2 Vector) is the inverse of length. Should you want to define different units, you can do so by opening the Units dialog box and selecting resistance from the Quantities list.
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.
“Snap” the plane tool (or the line tool) onto the boundary of the porous region. (Follow the instructions in Using the Plane Tool or Using the Line Tool for initializing the tool to a position on an existing surface.)
Rotate the axes of the tool appropriately until they are aligned with the porous medium.
Once the axes are aligned, click the or button in the Fluid dialog box. ANSYS Fluent will automatically set the Direction-1 Vector to the direction of the red arrow of the tool, and (in 3D) the Direction-2 Vector to the direction of the green arrow.
To use a conical coordinate system (for example, for an annular, conical filter element), follow the steps below. This option is available only in 3D cases.
Turn on the Conical option.
Set the Cone Half Angle (the angle between the cone’s axis and its surface, shown in Figure 6.13: Cone Half Angle). To use a cylindrical coordinate system, set the Cone Half Angle to 0.
Specify the Cone Axis Vector and Point on Cone Axis. The cone axis is specified as being in the direction of the Cone Axis Vector (unit vector), and passing through the Point on Cone Axis. The cone axis may or may not pass through the origin of the coordinate system.
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:
Select a boundary zone of the conical filter element that is normal to the cone axis vector in the drop-down list next to the button.
Click the button. ANSYS Fluent will automatically “snap” the plane tool onto the boundary. It will also set the Cone Axis Vector and the Point on Cone Axis. (Note that you will still have to set the Cone Half Angle yourself.)
An alternate method is as follows:
“Snap” the plane tool onto the boundary of the porous region. (Follow the instructions in Using the Plane Tool for initializing the tool to a position on an existing surface.)
Rotate and translate the axes of the tool appropriately until the red arrow of the tool is pointing in the direction of the cone axis vector and the origin of the tool is on the cone axis.
Once the axes and origin of the tool are aligned, click the button in the Fluid dialog box. ANSYS Fluent will automatically set the Cone Axis Vector and the Point on Cone Axis. (Note that you will still have to set the Cone Half Angle yourself.)
Under Viscous Resistance, specify
the viscous resistance coefficient in each direction.
Under Inertial Resistance, specify the inertial resistance coefficient in each direction. (You can 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 6–6 yields the expression below:
(6–16) |
Whether or not you use the Alternative Formulation option depends on how well you can fit your experimentally determined pressure drop data to the ANSYS Fluent model. For example, if the flow through the medium is aligned with the mesh in your ANSYS Fluent model, then it will not make a difference whether or not you use the formulation. In general, however, the default and the Alternative Formulation are not equivalent, and solution differences can occur when switching between the two options.
For more information about simulations involving highly anisotropic porous media, see Solution Strategies for Porous Media.
Important: 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 tangential direction
of the cone, 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:
In the isotropic case, the resistance coefficients in all directions are the same (for example, a sponge). For an isotropic case, you must explicitly set the resistance coefficients in each direction to the same value.
When (in 3D) the coefficients in two directions are the same and those in the third direction are different or (in 2D) the coefficients in the two directions are different, you must be careful to specify the coefficients properly for each direction. For example, if you had a porous region consisting of cylindrical straws with small holes in them positioned parallel to the flow direction, the flow would pass easily through the straws, but the flow in the other two directions (through the small holes) would be very little. If you had a plane of flat plates perpendicular to the flow direction, the flow would not pass through them at all; it would instead move in the other two directions.
In 3D the third possible case is one in which all three coefficients are different. For example, if the porous region consisted of a plane of irregularly-spaced objects (for example, pins), the movement of flow between the blockages would be different in each direction. You would therefore need to specify different coefficients in each direction.
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
(6–17) |
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:
The velocity through the perforated plate assumes that the plate is 100% open.
The loss coefficient must be converted into dynamic head loss per unit length of the porous region.
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:
(6–18) |
or, noting that for the same flow rate, ,
(6–19) |
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
(6–20) |
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 [28], a semi-empirical correlation applicable over a wide range of Reynolds numbers and for many types of packing:
(6–21) |
When modeling laminar flow through a packed bed, the second term in the above equation may be dropped, resulting in the Blake-Kozeny equation [28]:
(6–22) |
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 6–4 and Equation 6–6 with Equation 6–21, the permeability and inertial loss
coefficient in each component direction may be identified as
(6–23) |
and
(6–24) |
As a third example we will take the equation of Van Winkle et al. [83] [110] 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
(6–25) |
| where | |
| | |
| | |
| | |
| | |
| |
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 6–25, making use of the relationship
(6–26) |
and dividing by the plate thickness, ,
we obtain
(6–27) |
where is the superficial velocity (not
the velocity in the holes). Comparing with Equation 6–6 is seen that, for the direction normal
to the plate, the constant
can be calculated
from
(6–28) |
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 6–22) we might choose to employ tabulated experimental data. Such data is available for many types of fiber [46].
| Volume Fraction of Solid Material | Dimensionless
Permeability |
|---|---|
| 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 6–4, 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:
| Velocity (m/s) | Pressure Drop (Pa) |
|---|---|
| 20.0 | 197.8 |
| 50.0 | 948.1 |
| 80.0 | 2102.5 |
| 110.0 | 3832.9 |
then an curve can be plotted to create
a trendline through these points yielding the following equation
(6–29) |
where is the pressure drop and
is the
velocity.
Important: Although the best fit curve may yield negative coefficients, it should be avoided when using the porous media model in ANSYS Fluent.
Note that a simplified version of the momentum equation, relating the pressure drop to the source term, can be expressed as
(6–30) |
or
(6–31) |
Hence, comparing Equation 6–29 to Equation 6–2, yields the following curve coefficients:
(6–32) |
with kg/
, and a porous
media thickness,
, assumed to be 1 m in this example,
the inertial resistance factor,
.
Likewise,
(6–33) |
with , the viscous
inertial resistance factor,
.
Important: 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 6–137. From there, you can determine the permeability
and the pressure jump
coefficient
.
If you choose to use the power-law approximation of the porous-media
momentum source term (Equation 6–3),
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.
To specify that the porous medium and the fluid flow are in thermal equilibrium, scroll down below the resistance inputs in the Fluid dialog box to the Heat Transfer Settings group box and select Equilibrium from the Thermal Model list (this is the default selection). Then you must specify the material contained in the porous medium by selecting the appropriate solid in the Solid Material Name drop-down list.
If you want to check or modify the properties of the selected
material, you can click 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
porous 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 function,
see the separate Fluent Customization Manual.
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 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 6.14: 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.
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 6.14: 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 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.
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.
For two-phase flow through a porous medium, the flow rate of each phase is dictated by the portion of the total cross-sectional area that is available for the phase to flow and the permeability of the medium. Since the portion of the total cross-sectional area
is difficult to determine, the reservoir engineers use the concept of effective permeability:
(6–34) |
The effective permeability to a phase is the ability of a porous medium to transmit that phase when its saturation in the porous medium is less than 100%. The effective permeability to a phase depends on the permeability of the medium
, the phase saturation, the saturations of other phases present in the medium, the wettability preference of the medium, and its pore characteristics and size distribution.
A typical reservoir displays a range of effective permeabilities and permeability variations. To overcome this problem, the concept of the relative permeability is used:
(6–35) |
The relative permeability , therefore, is a ratio of the effective permeability
to some base permeability
. It is a dimensionless measure of the effective permeability and varies with the wetting phase saturation. There is no consensus for the choice of base permeability; however, for oil-water systems,
is
at irreducible water saturation for the oil phase, and
is
at residual oil saturation for the water phase.
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 [17] 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:
(6–36) |
| where: | |
|
| |
|
| |
|
|
In Fluent the phase saturation is the phase volume fraction. Thus
can be expressed as:
(6–37) |
where is the volume fraction residual in the
qth phase.
For the two-phase oil-water flow example, the relative permeabilities can be obtained from:
(6–38) |
This requires the specification of 6 parameters:
|
| the reference phase relative permeabilities for the two phases |
|
| the residual volume fractions for the two phases |
|
| 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
To model the relative permeability in ANSYS Fluent:
Set parameters for the mixture phase (mixture is selected for Phase in the Cell Zone Conditions task page).
In the Fluid dialog box, in the Porous Zone tab, under Relative Permeability, select Corey Model.
From the drop-down lists, select Wetting Phase and Non Wetting Phase.
Important: Although Equation 6–35 through Equation 6–38 are valid for any given phase, care must be exercised in defining the wetting and non-wetting phases.
Set conditions for the wetting phase (the wetting phase is selected from the Phase drop-down list in the Cell Zone Conditions task page). In the Fluid dialog box, in the Porous Zone tab, specify the following parameters in the Wetting Phase Relative Permeability group:
Similarly, set conditions for the non-wetting phase (the non-wetting phase is selected from the Phase drop-down list in the Cell Zone Conditions task page). In the Fluid dialog box, in the Porous Zone tab, specify the following parameters in the Non Wetting Phase Relative Permeability group:
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. 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 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.
As stated in Limitations and Assumptions of the Porous Media Model, by default ANSYS Fluent calculates the superficial velocity based on volumetric flow rate. The superficial velocity in the governing equations can be represented as
(6–39) |
where is the porosity of the media defined as
the ratio of the volume occupied by the fluid to the total volume.
The superficial velocity values within the porous region remain the same as those outside of the porous region, and porosity is not taken into account in the differential terms of the transport equations. This limits the accuracy of the porous model in cases where there should be an increase in velocity throughout the porous region, and does not yield accurate results when velocity values and gradients are important. For more accurate simulations of porous media flows, it becomes necessary to solve for the true, or physical, velocity throughout the flowfield rather than the superficial velocity, as well as to include porosity in all terms of the transport equations.
ANSYS Fluent allows the calculation of the physical velocity using the Porous Formulation, available in the Cell Zone Conditions task page. By default, the Superficial Velocity option is turned on.
Using the physical velocity formulation, and assuming a general
scalar , the governing equation in an isotropic
porous media has the following form:
(6–40) |
Assuming isotropic porosity and single phase flow, the volume-averaged mass and momentum conservation equations are as follows:
(6–41) |
(6–42) |
The last term in Equation 6–42 represents the viscous and inertial drag forces imposed by the pore walls on the fluid.
Important: Note that even when you solve for the physical velocity in Equation 6–42, the two resistance coefficients can still be derived using the superficial velocity as given in Defining the Viscous and Inertial Resistance Coefficients. ANSYS Fluent assumes that the inputs for these resistance coefficients are based upon well-established empirical correlations that are usually based on superficial velocity. Therefore, ANSYS Fluent automatically converts the inputs for the resistance coefficients into those that are compatible with the physical velocity formulation.
Important: Note that the inlet mass flow is also calculated from the superficial velocity. Therefore, for the same mass flow rate at the inlet and the same resistance coefficients, for either the physical or superficial velocity formulation you should obtain the same pressure drop across the porous media zone.
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:
(6–43) |
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 6–43 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 17–167, Equation 17–168, and Equation 17–171 in the Theory
Guide take the general forms described below.
(6–45) |
where the last term in Equation 6–45 is the momentum resistance (sink) source in a porous medium. It consists of two parts: a viscous loss term, and an inertial loss term. and
are the mass transfers from phase
to phase
and vise versa. The parameter
is the permeability, and
is the inertial resistance factor. Both
and
are functions of (
). When
, the flow is non-porous and the two loss terms disappear. Details about the user inputs related to the momentum resistance sources can be found in User Inputs for Porous Media.
(6–46) |
| where: | |
| Subscripts | |
|
| |
|
| |
|
| |
|
| |
|
| |
|
| |
|
| |
|
|
In general, you can use the standard solution procedures and
solution parameter settings when your ANSYS Fluent model includes porous
media. You may find, however, that the rate of convergence slows when
you define a porous region through which the pressure drop is relatively
large in the flow direction (for example, the permeability, , is low or the inertial
factor,
, is large).
This slow convergence can occur because the porous media pressure
drop appears as a momentum source term—yielding a loss of diagonal
dominance—in the matrix of equations solved. The best remedy
for poor convergence of a problem involving a porous medium is to
supply a good initial guess for the pressure drop across the medium.
Similarly, Standard Initialization is the recommended initialization method for porous media simulations. The default Hybrid Initialization method does not account for the porous media properties, and depending on boundary conditions, may produce an unrealistic initial velocity field. For porous media simulations, the Hybrid Initialization method should only be used with the Maintain Constant Velocity Magnitude option.
Another possible way to deal with poor convergence is to temporarily disable the porous media model (by turning off the Porous Zone option in the Fluid Dialog Box) and obtain an initial flow field without the effect of the porous region. With the porous media model turned off, ANSYS Fluent will treat the porous zone as a fluid zone and calculate the flow field accordingly. Once an initial solution is obtained, or the calculation is proceeding steadily to convergence, you can enable the porous media model and continue the calculation with the porous region included. (This method is not recommended for porous media with high resistance.)
Simulations involving highly anisotropic porous media may, at
times, pose convergence troubles. You can address these issues by
limiting the anisotropy of the porous media coefficients ( and
) to two or three orders of magnitude. Even
if the medium’s resistance in one direction is infinite, you
do not need to set the resistance in that direction to be greater
than 1000 times the resistance in the primary flow direction.
The impact of a porous region on the flow field can be determined by examining either velocity components or pressure values. Graphical plots (including XY plots and contour or vector plots) or alphanumeric reports of the following variables/functions may be of interest:
X, Y, Z Velocity (in the Velocity... category)
Static Pressure (in the Pressure... category)
These variables are contained in the specified categories of the variable selection drop-down list that appears in postprocessing dialog boxes.
Note that thermal reporting in the porous region is defined as follows:
(6–47) |
| where | |
| | |
| | |
| |
Important: For porous media involving surface reactions, you can display/report the surface reaction rates using the Arrhenius Rate of Reaction-n in the Reactions... category of the variable selection drop-down list.
Important: Special care must be taken when postprocessing a porous media simulation that utilizes the non-equilibrium thermal model. See Non-Equilibrium Thermal Model for details.