ChtMultiRegionFoam

From OpenFOAMWiki
Revision as of 14:10, 20 December 2018 by MAlletto (Talk | contribs)

ChtMultiRegionFoam

   Solver for steady or transient fluid flow and solid heat conduction, with
   conjugate heat transfer between regions, buoyancy effects, turbulence,
   reactions and radiation modelling.

1 Solution Strategy

The solver follows a segregated solution strategy. This means that the equations for each variable characterizing the system is solved sequentially and the solution of the preceding equations is inserted in the subsequent equation. The coupling between fluid and solid follows also the same strategy: First the equations for the fluid are solved using the temperature of the solid of the preceding iteration to define the boundary conditions for the temperature in the fluid. After that, the equation for the solid is solved using the temperature of the fluid of the preceding iteration to define the boundary condition for the solid temperature. This iteration procedure is executed until convergence.

The source code can be found in chtMultiRegionFoam.C


 
 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2011-2018 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.
 
    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.
 
    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.
 
    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
 
Application
    chtMultiRegionFoam
 
Description
    Solver for steady or transient fluid flow and solid heat conduction, with
    conjugate heat transfer between regions, buoyancy effects, turbulence,
    reactions and radiation modelling.
 
\*---------------------------------------------------------------------------*/
 
#include "fvCFD.H"
#include "turbulentFluidThermoModel.H"
#include "rhoReactionThermo.H"
#include "CombustionModel.H"
#include "fixedGradientFvPatchFields.H"
#include "regionProperties.H"
#include "compressibleCourantNo.H"
#include "solidRegionDiffNo.H"
#include "solidThermo.H"
#include "radiationModel.H"
#include "fvOptions.H"
#include "coordinateSystem.H"
#include "pimpleMultiRegionControl.H"
#include "pressureControl.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
int main(int argc, char *argv[])
{
    #define NO_CONTROL
    #define CREATE_MESH createMeshesPostProcess.H
    #include "postProcess.H"
 
    #include "setRootCaseLists.H"
    #include "createTime.H"
    #include "createMeshes.H"
    #include "createFields.H"
    #include "initContinuityErrs.H"
    pimpleMultiRegionControl pimples(fluidRegions, solidRegions);
    #include "createFluidPressureControls.H"
    #include "createTimeControls.H"
    #include "readSolidTimeControls.H"
    #include "compressibleMultiRegionCourantNo.H"
    #include "solidRegionDiffusionNo.H"
    #include "setInitialMultiRegionDeltaT.H"
 
    while (pimples.run(runTime))
    {
        #include "readTimeControls.H"
        #include "readSolidTimeControls.H"
 
        #include "compressibleMultiRegionCourantNo.H"
        #include "solidRegionDiffusionNo.H"
        #include "setMultiRegionDeltaT.H"
 
        runTime++;
 
        Info<< "Time = " << runTime.timeName() << nl << endl;
 
        // --- PIMPLE loop
        while (pimples.loop())
        {
            forAll(fluidRegions, i)
            {
                Info<< "\nSolving for fluid region "
                    << fluidRegions[i].name() << endl;
                #include "setRegionFluidFields.H"
                #include "solveFluid.H"
            }
 
            forAll(solidRegions, i)
            {
                Info<< "\nSolving for solid region "
                    << solidRegions[i].name() << endl;
                #include "setRegionSolidFields.H"
                #include "solveSolid.H"
            }
        }
 
        runTime.write();
 
        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }
 
    Info<< "End\n" << endl;
 
    return 0;
}
 
 
// ************************************************************************* //
 
 


2 Equations

For each region defined as fluid, the according equation for the fluid is solved and the same is done for each solid region. The regions are coupled by a thermal boundary condition. A short description of the solver can be found also in [1]

2.1 Equations Fluid

For each fluid region the compressible Navier Stokes equation are solved. The solver used to solve the fluid equations is a pressure bases solver. That means that a pressure equation (similar to the pressure equation used in an incompressible solver) is used to establish the connection between the momentum and the continuity equation. The algorithm to advance the solution in time is the following:

1. Update the density with the help of the continuity equation

2. Solve the momentum equation

3. Solve the spices transport equation

4. Solve the energy equation

5. Solve the pressure equation to ensure mass conservation

6. Correct the density by means of the new pressure field and the equation of state


The source code can be found in solveFluid.H


 
 
if (pimple.frozenFlow())
{
    #include "EEqn.H"
}
else
{
    if (!mesh.steady() && pimples.nCorrPimple() <= 1)
    {
        #include "rhoEqn.H"
    }
 
    #include "UEqn.H"
    #include "YEqn.H"
    #include "EEqn.H"
 
    // --- PISO loop
    while (pimple.correct())
    {
        #include "pEqn.H"
    }
 
    if (pimples.pimpleTurbCorr(i))
    {
        turbulence.correct();
    }
 
    if (!mesh.steady() && pimples.finalIter())
    {
        rho = thermo.rho();
    }
}
 


2.1.1 Mass conservation

The variable-density continuity equation is



\frac{\partial \rho}{\partial t} +   \frac{\partial {\rho u}_j}{\partial x_j} = 0
(1)

The source code can be found in src/finiteVolume/cfdTools/compressible/rhoEqn.H:


 
 
{
    fvScalarMatrix rhoEqn
    (
        fvm::ddt(rho)
      + fvc::div(phi)
      ==
        fvOptions(rho)
    );
 
    fvOptions.constrain(rhoEqn);
 
    rhoEqn.solve();
 
    fvOptions.correct(rho);
}
 

2.1.2 Momentum conservation



    \frac{ \partial (\rho {u}_i)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j u_i \right) = 

   - \frac{\partial p_{rgh}} {\partial{x_i}} - \frac{\partial \rho g_j x_j}{\partial x_i}  + \frac{\partial}{\partial x_j} \left( \tau_{ij} + \tau_{t_{ij}} \right)
(2)

 u represent the velocity,  g_i the gravitational acceleration,  p_{rgh} = p - \rho g_j x_j the pressure minus the hydrostatic pressure and  \tau_{ij}  and  \tau_{t_{ij}}  are the viscose and turbulent stresses.

The source code can be found in Ueqn.H:


 
 
    // Solve the Momentum equation
 
    MRF.correctBoundaryVelocity(U);
 
    tmp<fvVectorMatrix> tUEqn
    (
        fvm::ddt(rho, U) + fvm::div(phi, U)
      + MRF.DDt(rho, U)
      + turbulence.divDevRhoReff(U)
     ==
        fvOptions(rho, U)
    );
    fvVectorMatrix& UEqn = tUEqn.ref();
 
    UEqn.relax();
 
    fvOptions.constrain(UEqn);
 
    if (pimple.momentumPredictor())
    {
        solve
        (
            UEqn
         ==
            fvc::reconstruct
            (
                (
                  - ghf*fvc::snGrad(rho)
                  - fvc::snGrad(p_rgh)
                )*mesh.magSf()
            )
        );
 
        fvOptions.correct(U);
        K = 0.5*magSqr(U);
    }
 
    fvOptions.correct(U);
 
 


Note the the function fvc::reconstruct reconstructs a vector  u_i from its face fluxes  \phi_f = u_i  S_{fi} using following expression:




u_i =\left( \sum_f \frac{S_{fi}S_{fi}}{|S_{fi} |}  \right)^{-1}\left [   \sum_f \phi_f \frac{S_{fi}  }{|S_{fi} |} \right]
(x)

2.1.3 Pressure equation

A good explanation of the derivation of the pressure correction equation for incompressible flows can be found in the book [2]. In this solver however a pressure equation is solved. The purpose is to correct the velocity field and via the equation of sate also the density in order to have a velocity and density field which satisfy the continuity equation. The derivation of this pressure equation can be found in [3]. or also following the link https://feaweb.aub.edu.lb/research/cfd/pdfs/publications/Algorithms-1.pdf.

The equation reads in semi discrete form:


    \frac{ \partial \rho}{\partial t} V_P + \sum_f \psi p v_f ^*  \cdot S_f  +  \sum_f  \rho_f^* \frac{\bold{H[v^*]}}{\bold{A_P}} \cdot S_f - 
    \sum_f \frac{\nabla p_P}{\bold{A_P}} \cdot S_f - \sum_f \rho_f^*v_f^* \cdot S_f +  \sum_f  \rho_f^* \frac{\bold{H[v']}}{\bold{A_P}} \cdot S_f +
\sum_f \rho_f^'v_f^' \cdot S_f
   = 0
(x)

The density  \rho can be written as:


 \rho = \psi p
(x)


The sum is taken over the faces of the cell with the centre point P. The last term in the above equation is very small and hence neglected. The second last term is also neglected since the velocity correction  v' is not know a the moment of the solution of the equation. Hence the final form of the pressure equation reads:


    \frac{ \partial \rho}{\partial t} V_P + \sum_f \psi p v_f ^*  \cdot S_f  +  \sum_f  \rho_f^* \frac{\bold{H[v^*]}}{\bold{A_P}} \cdot S_f - 
    \sum_f \frac{\nabla p_P}{\bold{A_P}} \cdot S_f - \sum_f \rho_f^*v_f^* \cdot S_f 
   = 0
(x)

The pressure p can be written as


 p = p_{rgh} + \rho g_i x_i
(x)

The purpose is the obtain an equation for modified pressure  p_{rgh} . Inserting the expression for the pressure in the above equation one obtains:


    \frac{ \partial \rho }{\partial t} V_P + \sum_f \psi ( p_{rgh} + \rho g_i x_i ) v_f ^*  \cdot S_f  +  \sum_f  \rho_f^* \frac{\bold{H[v^*]}}{\bold{A_P}} \cdot S_f - 
    \sum_f \frac{\nabla p_{rghP}}{\bold{A_P}} \cdot S_f - \sum_f \frac{\nabla \rho_{P} g_i x_i}{\bold{A_P}} \cdot S_f  - \sum_f \rho_f^*v_f^* \cdot S_f 
   = 0
(x)
.

The above equation still contains the density  \rho of the current time step. As approximation of the density of the current time step the density of the previous time step  \rho^* could be used. By doing this and with the following expression:


  \psi p_{rgh} = \psi p -  \psi \rho g_i x_i = \rho - \psi \rho g_i x_i
(x)

the above equation for the modified pressure could be simplified:


    \frac{ \partial \rho  }{\partial t} V_P + \sum_f \psi  p_{rgh} v_f ^*  \cdot S_f   -  \sum_f \psi  p_{rgh}^* v_f ^*  \cdot S_f +  \sum_f  \rho_f^* \frac{\bold{H[v^*]}}{\bold{A_P}} \cdot S_f - 
    \sum_f \frac{\nabla p_{rghP}}{\bold{A_P}} \cdot S_f - \sum_f \frac{\nabla \rho^*_{P} g_i x_i}{\bold{A_P}} \cdot S_f  
   = 0
(x)
.

Comparing the above equation with the source code in the bottom we can identify the corrected phase velocity without considering the pressure gradient as:


 v_f ^*    =  \frac{\bold{H[v^*]}}{\bold{A_P}} -  \frac{\nabla \rho^*_{P} g_i x_i}{\bold{A_P}}
(x)
.

In order to derive the expression for the time derivative in the source code of the pressure equation, the density is divided into the density of the previous time step  \rho^* and a density correction  \rho^' , i.e.,  \rho =  \rho^* +  \rho^'  and the time derivative is taken from this expression:


\frac{\partial \rho}{\partial t} = \frac{\partial \rho^*}{\partial t} + \frac{\partial \rho^'}{\partial t} =  \frac{\partial \rho^*}{\partial t} + \psi ( \frac{\partial p_{rgh}^'}{\partial t} +  \frac{\partial \rho^'}{\partial t}g_i x_i   )
(x)
.

Neglecting the last two terms in the above equation one obtains:


\frac{\partial \rho}{\partial t} =   \frac{\partial \rho^*}{\partial t} + \psi \frac{\partial p_{rgh}^'}{\partial t}
(x)
.

The source code for the pressure equation can be found in pEqn.H:


 
 
if (!mesh.steady() && !pimple.simpleRho())
{
    rho = thermo.rho();
}
 
volScalarField rAU("rAU", 1.0/UEqn.A());
surfaceScalarField rhorAUf("rhorAUf", fvc::interpolate(rho*rAU));
volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p_rgh));
if (pimple.nCorrPISO() <= 1)
{
    tUEqn.clear();
}
 
surfaceScalarField phig(-rhorAUf*ghf*fvc::snGrad(rho)*mesh.magSf());
 
surfaceScalarField phiHbyA
(
    "phiHbyA",
    fvc::flux(rho*HbyA)
  + MRF.zeroFilter(rhorAUf*fvc::ddtCorr(rho, U, phi))
);
 
MRF.makeRelative(fvc::interpolate(rho), phiHbyA);
 
const bool closedVolume = adjustPhi(phiHbyA, U, p_rgh);
const bool adjustMass = closedVolume && !thermo.incompressible();
 
phiHbyA += phig;
 
// Update the pressure BCs to ensure flux consistency
constrainPressure(p_rgh, rho, U, phiHbyA, rhorAUf, MRF);
 
{
    fvScalarMatrix p_rghEqnComp
    (
        fvc::ddt(rho) + psi*correction(fvm::ddt(p_rgh))
    );
 
    if (pimple.transonic())
    {
        surfaceScalarField phid
        (
            "phid",
            (fvc::interpolate(psi)/fvc::interpolate(rho))*phiHbyA
        );
 
        phiHbyA -= fvc::interpolate(psi*p_rgh)*phiHbyA/fvc::interpolate(rho);
 
        p_rghEqnComp += fvm::div(phid, p_rgh);
    }
 
    // Thermodynamic density needs to be updated by psi*d(p) after the
    // pressure solution
    tmp<volScalarField> psip0(mesh.steady() ? tmp<volScalarField>() : psi*p);
 
    while (pimple.correctNonOrthogonal())
    {
        fvScalarMatrix p_rghEqnIncomp
        (
            fvc::div(phiHbyA)
          - fvm::laplacian(rhorAUf, p_rgh)
        );
 
        fvScalarMatrix p_rghEqn(p_rghEqnComp + p_rghEqnIncomp);
 
        p_rghEqn.setReference
        (
            pressureControl.refCell(),
            pressureControl.refValue()
        );
 
        p_rghEqn.solve(mesh.solver(p_rgh.select(pimple.finalInnerIter())));
 
        if (pimple.finalNonOrthogonalIter())
        {
            // Calculate the conservative fluxes
            phi = phiHbyA + p_rghEqn.flux();
 
            // Explicitly relax pressure for momentum corrector
            p_rgh.relax();
 
            // Correct the momentum source with the pressure gradient flux
            // calculated from the relaxed pressure
            U = HbyA
                + rAU*fvc::reconstruct((phig + p_rghEqnIncomp.flux())/rhorAUf);
            U.correctBoundaryConditions();
            fvOptions.correct(U);
            K = 0.5*magSqr(U);
        }
    }
 
    p = p_rgh + rho*gh;
 
    // Thermodynamic density update
    if (!mesh.steady())
    {
        thermo.correctRho(psi*p - psip0);
    }
}
 
// Update pressure time derivative if needed
if (thermo.dpdt())
{
    dpdt = fvc::ddt(p);
}
 
// Solve continuity
if (!mesh.steady())
{
    #include "rhoEqn.H"
    #include "compressibleContinuityErrs.H"
}
else
{
    #include "incompressible/continuityErrs.H"
}
 
// Pressure limiting
const bool pLimited = pressureControl.limit(p);
 
// For closed-volume compressible cases adjust the pressure level
// to obey overall mass continuity
if (adjustMass)
{
    p += (initialMass - fvc::domainIntegrate(thermo.rho()))
        /fvc::domainIntegrate(psi);
    p_rgh = p - rho*gh;
}
 
if (adjustMass || pLimited)
{
    p.correctBoundaryConditions();
}
 
// Density updates
if (adjustMass || pLimited || mesh.steady() || pimple.simpleRho())
{
    rho = thermo.rho();
}
 
if (mesh.steady() && !pimple.transonic())
{
    rho.relax();
}
 
Info<< "Min/max rho:" << min(rho).value() << ' '
    << max(rho).value() << endl;
 
 

2.1.4 Energy conservation

The energy equation can be found in: https://cfd.direct/openfoam/energy-equation/

The total energy of a fluid element can be seen as the sum of kinetic energy  k = 0.5 u_i u_i and internal energy  e . The rate of change of the kinetic energy within a fluid element is the work done on this fluid element by the viscous forces, the pressure and eternal volume forces like the gravity:



    \frac{ \partial (\rho k)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j k \right) =     - \frac{\partial p u_j} {\partial{x_i} }- \rho g_j u_j  + 
\frac{\partial}{\partial x_j}\left( \tau_{ij} u_i \right)
(3)

The rate of change of the internal energy  e of a fluid element is the heat transferred to this fluid element by diffusion and turbulence   q_i + q_{ti}  plus the heat source term  r plus the heat source by radiation  Rad  :



    \frac{ \partial (\rho e)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j e \right) =     - \frac{\partial q_i} {\partial{x_i} } +  \rho r  + Rad
(4)

The change rate of the total energy is the sum of the above two equations:



    \frac{ \partial (\rho e)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j e \right) + \frac{ \partial (\rho k)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j k \right)   =     - \frac{\partial ( q_i + q_{ti}) } {\partial{x_i} } +  \rho r  + Rad    - \frac{\partial p u_j} {\partial{x_i} }- \rho g_j u_j  + 
\frac{\partial}{\partial x_j}\left( \tau_{ij} u_i \right)
(5)

Instead of the internal energy  e there is also the option to solve the equation for the enthalpy  h =  e + p/\rho :



    \frac{ \partial (\rho h)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j h \right) + \frac{ \partial (\rho k)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j k \right)   =     - \frac{\partial  ( q_i + q_{ti})} {\partial{x_i} } +  \rho r  + Rad    + \frac{\partial p} {\partial{t} }- \rho g_j u_j  + 
\frac{\partial}{\partial x_j}\left( \tau_{ij} u_i \right)
(5)

The source code can be found in EEqn.H:


 
{
    volScalarField& he = thermo.he();
 
    fvScalarMatrix EEqn
    (
        fvm::ddt(rho, he) + fvm::div(phi, he)
      + fvc::ddt(rho, K) + fvc::div(phi, K)
      + (
            he.name() == "e"
          ? fvc::div
            (
                fvc::absolute(phi/fvc::interpolate(rho), U),
                p,
                "div(phiv,p)"
            )
          : -dpdt
        )
      - fvm::laplacian(turbulence.alphaEff(), he)
     ==
        rho*(U&g)
      + rad.Sh(thermo, he)
      + Qdot
      + fvOptions(rho, he)
    );
 
    EEqn.relax();
 
    fvOptions.constrain(EEqn);
 
    EEqn.solve();
 
    fvOptions.correct(he);
 
    thermo.correct();
    rad.correct();
 
    Info<< "Min/max T:" << min(thermo.T()).value() << ' '
        << max(thermo.T()).value() << endl;
}

2.1.5 Species conservation

In order to account for the chemical reactions occurring between different chemical species a conservation equation for each species k has to be solved:



   \frac{ \partial (\rho Y_k)}{\partial t} + \frac{\partial}{\partial x_j} \left( \rho {u}_j Y_k \right) =      \frac{\partial } {\partial{x_j} }\mu_{eff}\frac{\partial Y_k}{\partial x_j} + R_k
(6)

 R_k is the reaction rate of the species k.

The source code can be found in YEqn.H:


 
tmp<fv::convectionScheme<scalar>> mvConvection(nullptr);
 
if (Y.size())
{
    mvConvection = tmp<fv::convectionScheme<scalar>>
    (
        fv::convectionScheme<scalar>::New
        (
            mesh,
            fields,
            phi,
            mesh.divScheme("div(phi,Yi_h)")
        )
    );
}
 
{
    reaction.correct();
    Qdot = reaction.Qdot();
    volScalarField Yt
    (
        IOobject("Yt", runTime.timeName(), mesh),
        mesh,
        dimensionedScalar("Yt", dimless, 0)
    );
 
    forAll(Y, i)
    {
        if (i != inertIndex && composition.active(i))
        {
            volScalarField& Yi = Y[i];
 
            fvScalarMatrix YiEqn
            (
                fvm::ddt(rho, Yi)
              + mvConvection->fvmDiv(phi, Yi)
              - fvm::laplacian(turbulence.muEff(), Yi)
             ==
                reaction.R(Yi)
              + fvOptions(rho, Yi)
            );
 
            YiEqn.relax();
 
            fvOptions.constrain(YiEqn);
 
            YiEqn.solve(mesh.solver("Yi"));
 
            fvOptions.correct(Yi);
 
            Yi.max(0.0);
            Yt += Yi;
        }
    }
 
    if (Y.size())
    {
        Y[inertIndex] = scalar(1) - Yt;
        Y[inertIndex].max(0.0);
    }
}
 

2.2 Equations Solid

For the solid regions only the energy equation has to be solved. The energy equation states that the temporal change of enthalpy of the solid is equal to the divergence of the heat conducted through the solid:



    \frac{ \partial (\rho h)}{\partial t}    =     
\frac{\partial}{\partial x_j}\left( \alpha \frac{\partial h}{\partial x_j}  \right)
(7)
.

h is the specific enthalpy, \rho the density and \alpha  = \kappa / c_p  is the thermal diffusivity which is defined as the ratio between the thermal conductivity \kappa and the specific heat capacity c_p . Note that \kappa can be also anisotropic.

The source code can be found in solveSolid.H:


 
 
{
    while (pimple.correctNonOrthogonal())
    {
        fvScalarMatrix hEqn
        (
            fvm::ddt(betav*rho, h)
          - (
                thermo.isotropic()
              ? fvm::laplacian(betav*thermo.alpha(), h, "laplacian(alpha,h)")
              : fvm::laplacian(betav*taniAlpha(), h, "laplacian(alpha,h)")
            )
          ==
            fvOptions(rho, h)
        );
 
        hEqn.relax();
 
        fvOptions.constrain(hEqn);
 
        hEqn.solve(mesh.solver(h.select(pimples.finalIter())));
 
        fvOptions.correct(h);
    
 
thermo.correct();
 
Info<< "Min/max T:" << min(thermo.T()).value() << ' '
    << max(thermo.T()).value() << endl;
 
 

2.3 Coupling between Fluid and Solid

A good explanation of the coupling between fluid and solid can be found in https://www.cfd-online.com/Forums/openfoam-solving/143571-understanding-temperature-coupling-bcs.html.

At the interface between solid s and fluid f the temperature T for both phases that to be the same:



T_f = T_s
(8)
.

Furthermore the heat flux entering one region at one side of the interphase should be equal to the heat flux leaving the other region on the other side of the domain:




Q_f = -Q_s
(9)
.

If we neglect radiation the above expression can be written as:



\kappa_f \frac{d T_f}{ d n} = - \kappa_s \frac{d T_s}{ d n}
(10)
.

 n  represents the direction normal to the wall.  \kappa_f  and  \kappa_s  are the thermal conductivity of the fluid and solid, respectively.

The source code of the above boundary condition can be found in src/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/turbulentTemperatureCoupledBaffleMixed/turbulentTemperatureCoupledBaffleMixedFvPatchScalarField.C


 
 
 
void turbulentTemperatureCoupledBaffleMixedFvPatchScalarField::updateCoeffs()
 {
     if (updated())
     {
         return;
     }
 
     // Since we're inside initEvaluate/evaluate there might be processor
     // comms underway. Change the tag we use.
     int oldTag = UPstream::msgType();
     UPstream::msgType() = oldTag+1;
 
     // Get the coupling information from the mappedPatchBase
     const mappedPatchBase& mpp =
         refCast<const mappedPatchBase>(patch().patch());
     const polyMesh& nbrMesh = mpp.sampleMesh();
     const label samplePatchi = mpp.samplePolyPatch().index();
     const fvPatch& nbrPatch =
         refCast<const fvMesh>(nbrMesh).boundary()[samplePatchi];
 
     // Calculate the temperature by harmonic averaging
     // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
 
     const turbulentTemperatureCoupledBaffleMixedFvPatchScalarField& nbrField =
     refCast
     <
         const turbulentTemperatureCoupledBaffleMixedFvPatchScalarField
     >
     (
         nbrPatch.lookupPatchField<volScalarField, scalar>
         (
             TnbrName_
         )
     );
 
     // Swap to obtain full local values of neighbour internal field
     tmp<scalarField> nbrIntFld(new scalarField(nbrField.size(), 0.0));
     tmp<scalarField> nbrKDelta(new scalarField(nbrField.size(), 0.0));
 
     if (contactRes_ == 0.0)
     {
         nbrIntFld.ref() = nbrField.patchInternalField();
         nbrKDelta.ref() = nbrField.kappa(nbrField)*nbrPatch.deltaCoeffs();
     }
     else
     {
         nbrIntFld.ref() = nbrField;
         nbrKDelta.ref() = contactRes_;
     }
 
     mpp.distribute(nbrIntFld.ref());
     mpp.distribute(nbrKDelta.ref());
 
     tmp<scalarField> myKDelta = kappa(*this)*patch().deltaCoeffs();
 
 
     // Both sides agree on
     // - temperature : (myKDelta*fld + nbrKDelta*nbrFld)/(myKDelta+nbrKDelta)
     // - gradient    : (temperature-fld)*delta
     // We've got a degree of freedom in how to implement this in a mixed bc.
     // (what gradient, what fixedValue and mixing coefficient)
     // Two reasonable choices:
     // 1. specify above temperature on one side (preferentially the high side)
     //    and above gradient on the other. So this will switch between pure
     //    fixedvalue and pure fixedgradient
     // 2. specify gradient and temperature such that the equations are the
     //    same on both sides. This leads to the choice of
     //    - refGradient = zero gradient
     //    - refValue = neighbour value
     //    - mixFraction = nbrKDelta / (nbrKDelta + myKDelta())
 
     this->refValue() = nbrIntFld();
     this->refGrad() = 0.0;
     this->valueFraction() = nbrKDelta()/(nbrKDelta() + myKDelta());
 
     mixedFvPatchScalarField::updateCoeffs();
 
     if (debug)
     {
         scalar Q = gSum(kappa(*this)*patch().magSf()*snGrad());
 
         Info<< patch().boundaryMesh().mesh().name() << ':'
             << patch().name() << ':'
             << this->internalField().name() << " <- "
             << nbrMesh.name() << ':'
             << nbrPatch.name() << ':'
             << this->internalField().name() << " :"
             << " heat transfer rate:" << Q
             << " walltemperature "
             << " min:" << gMin(*this)
             << " max:" << gMax(*this)
             << " avg:" << gAverage(*this)
             << endl;
     }
 
     // Restore tag
     UPstream::msgType() = oldTag;
 }
 

3 Source Code

4 References

  1. EL ABBASSIA, M.; LAHAYE, D. J. P.; VUIK, C. MODELLING TURBULENT COMBUSTION COUPLED WITH CONJUGATE HEAT TRANSFER IN OPENFOAM.
  2. Moukalled, F., L. Mangani, and M. Darwish. "The finite volume method in computational fluid dynamics." An Advanced Introduction with OpenFOAM and Matlab (2016):
  3. Darwish, F. Moukalled, M. "A unified formulation of the segregated class of algorithms for fluid flow at all speeds." Numerical Heat Transfer: Part B: Fundamentals 37.1 (2000): 103-139