TEqn implementation in icoReactingMultiphaseInterFoam

gowthaman · September 30, 2019, 10:28

Hi Foamers,

I have a basic question on implementation of temperature equation in one of the solvers in OF v1806. I was going through the TEqn.H file of icoReactingMultiphaseInterFoam in OF and found the following implementation:

Code:

   
 fvScalarMatrix TEqn
    (
        fvm::ddt(rhoCp, T)
      + fvm::div(rhoCpPhi, T, "div(phi,T)")
      - fvm::Sp(fvc::ddt(rhoCp) + fvc::div(rhoCpPhi), T)
      - fvm::laplacian(kappaEff, T,  "laplacian(kappa,T)")
      ==
        fluid.heatTransfer(T)
      + radiation->ST(T)
      + fvOptions(rhoCp, T)
    );

Does the left-hand side of the equation mean the following?
$\rho C_{p} \frac{\partial T}{\partial t}$ + $\rho C_{p} \nabla . (\Phi T)$ - $\Delta (kT)$

If that is the case, then why are density and Cp has taken out as constant? Shouldn't the volume of fluid averaged rhoCp depend on both time and space in a multiphase system?

Please let me know if I'm missing something here as I'm quite new to heat transfer modelling.

Many thanks,
Gowthaman

CorbinMG · December 4, 2022, 20:40

Hi Gowthaman,

I think you are correct. At least for the transient term we can use the product rule to expand:

$\frac{\partial \rho CpT}{\partial t} = T \frac{\partial \rho Cp}{\partial t} + \rho Cp \frac{\partial T}{\partial t}$

Using algebra to rearrange we have the below equation. The right hand side corresponds, in so far as I can tell, to what is implemented in icoReactingMultiphaseInterFoam TEqn.H. Therefore, effectively the LHS is being calculated.

$\rho Cp \frac{\partial T}{\partial t} = \frac{\partial \rho CpT}{\partial t} - T \frac{\partial \rho Cp}{\partial t}$

Now, why code the right hand side instead of just putting $\rho Cp \frac{\partial T}{\partial t}$ directly? I have a theory: fvm::ddt(rhoCp, T) makes an fvScalarMatrix data type. OpenFOAM, in my experience, does not allow the multiplication of volScalarField by fvScalarMatrix or it will give error at compilation. That is to say, if we had rhoCp stored as volScalarField, rhoCp*fvm::ddt(T) would give volScalarField*fvScalarMatrix compilation error.

Fauster has documented this volScalarField*fvScalarMatrix compilation error, but no one has responded a way to get around it: How to multiply volScalarField and fvScalarMatrix ?

EDIT: Thank you to newGuyAtCFD for pointing out my oversight. Please regard my aforementioned theory as incorrect. volScalarField*fvScalarMatrix IS possible. But, fvScalarMatrix*volScalarField gives compilation error:

Code:

volScalarField rhoCp1 = rho1*alpha1*mixture.thermo1().Cp() + rho2*alpha2*mixture.thermo2().Cp();
fvScalarMatrix eEqn
(
rhoCp1*fvm::ddt(T)         //  compiles OK!
//fvm::ddt(T)*rhoCp1      //  gives compilation error!
==
fvOptions(rhoCp1, T)
);

newGuyAtCFD · December 5, 2022, 16:07

Quote:

Originally Posted by gowthaman

Hi Foamers,

I have a basic question on implementation of temperature equation in one of the solvers in OF v1806. I was going through the TEqn.H file of icoReactingMultiphaseInterFoam in OF and found the following implementation:

Code:

   
 fvScalarMatrix TEqn
    (
        fvm::ddt(rhoCp, T)
      + fvm::div(rhoCpPhi, T, "div(phi,T)")
      - fvm::Sp(fvc::ddt(rhoCp) + fvc::div(rhoCpPhi), T)
      - fvm::laplacian(kappaEff, T,  "laplacian(kappa,T)")
      ==
        fluid.heatTransfer(T)
      + radiation->ST(T)
      + fvOptions(rhoCp, T)
    );

Does the left-hand side of the equation mean the following?
$\rho C_{p} \frac{\partial T}{\partial t}$ + $\rho C_{p} \nabla . (\Phi T)$ - $\Delta (kT)$

If that is the case, then why are density and Cp has taken out as constant? Shouldn't the volume of fluid averaged rhoCp depend on both time and space in a multiphase system?

Please let me know if I'm missing something here as I'm quite new to heat transfer modelling.

Many thanks,
Gowthaman

To my understanding the above code should represent:

$\frac{\partial \left(\rho C_p T\right)}{\partial t} + \nabla \cdot (\rho C_p \vec{v} T) - T\left [ \frac{\partial \left(\rho C_p\right)}{\partial t} + \nabla \cdot \left(\rho C_p \vec{v} \right)\right ] - \nabla \cdot \left( k_{eff} \nabla T\right) = S_T$

Where everything is inside the parenthesis.

Please correct me if I am wrong.

Also, multiplying a volScalarField with a matrix is possible and defined on line 2816-2826 of fvMatrix.C

Code:

  template<class Type>
  Foam::tmp<Foam::fvMatrix<Type>> Foam::operator*
  (
      const volScalarField::Internal& dsf,
      const tmp<fvMatrix<Type>>& tA
  )
  {
      tmp<fvMatrix<Type>> tC(tA.ptr());
      tC.ref() *= dsf;
      return tC;
  }

überschwupper · December 6, 2022, 05:12

Quote:

Originally Posted by newGuyAtCFD

To my understanding the above code should represent:

$\frac{\partial \left(\rho C_p T\right)}{\partial t} + \nabla \cdot (\rho C_p \vec{v} T) - T\left [ \frac{\partial \left(\rho C_p\right)}{\partial t} + \nabla \cdot \left(\rho C_p \vec{v} \right)\right ] - \nabla \cdot \left( k_{eff} \nabla T\right) = S_T$

Where everything is inside the parenthesis.

Please correct me if I am wrong.

I agree with you, but corrected the T into the derivatives.
The orginial equation should look like this with the mentioned substitutions of the reformulated differentials. I mean this should be equal

$\partial_t (\rho C_p T) = \rho C_p \partial_tT + T \partial_t (\rho C_P)$
same for the divergence term. Then it follows:

$\rho C_p\partial_t T + \rho C_p (\vec{v} \cdot \nabla) T - \nabla \cdot (k_{eff} \nabla T) = S_T$

Which is nothing else than:

$\rho C_p \frac{DT}{Dt} - \nabla \cdot (k_{eff} \nabla T) = S_T$

My guess is that inserting of the reformulated differentials was done either because of discretization reasons or because of the interphase properties.

sabrahams · August 9, 2023, 10:00

Hi everyone,

I wonder if anyone can help me with a follow-up question please? In compressibleInterFoam in OF9, the TEqn is formulated as

Code:

fvm::ddt(rho, T) + fvm::div(rhoPhi, T) - fvm::Sp(contErr, T)
      - fvm::laplacian(turbulence.alphaEff(), T)
      + (
            fvc::div(fvc::absolute(phi, U), p)()() // - contErr/rho*p
          + (fvc::ddt(rho, K) + fvc::div(rhoPhi, K))()()
          - (U()&(fvModels.source(rho, U)&U)()) - contErr*K 
        )
       *(
           alpha1()/mixture.thermo1().Cv()()
         + alpha2()/mixture.thermo2().Cv()()
        )
        
     ==
           fvModels.source(rho, T)

In this case,

is used instead of

but I believe it should still be inside the derivatives since the averaged

can vary in time and space.

I believe the TEqn should be equivalent to
$\frac{\partial}{\partial t}(\rho C_v T)+\nabla\cdot(\rho C_v U T) + \frac{\partial}{\partial t}(\rho k)+\nabla\cdot(\rho U k)+\nabla \cdot (pU)-\nabla\cdot (K \nabla T)=S,$

but the formulation above seems to be equivalent to
$\frac{C_{1}C_{2}}{{\alpha_1 C_{2}+\alpha_2 C_{1}}} \left[\frac{\partial}{\partial t}(\rho T)+\nabla\cdot(\rho U T) \right]+ \frac{\partial}{\partial t}(\rho k)+\nabla\cdot(\rho U k)+\nabla \cdot (pU)-\nabla\cdot (K \nabla T)=S.$

Can anyone help me to understand how

has been taken out in this way?

Many thanks,
SAbrahams

September 30, 2019, 10:28	TEqn implementation in icoReactingMultiphaseInterFoam	#1
gowthaman New Member Gowthaman Parivendhan Join Date: Aug 2019 Location: Dublin, Ireland Posts: 3 Rep Power: 6	Hi Foamers, I have a basic question on implementation of temperature equation in one of the solvers in OF v1806. I was going through the TEqn.H file of icoReactingMultiphaseInterFoam in OF and found the following implementation: Code: fvScalarMatrix TEqn ( fvm::ddt(rhoCp, T) + fvm::div(rhoCpPhi, T, "div(phi,T)") - fvm::Sp(fvc::ddt(rhoCp) + fvc::div(rhoCpPhi), T) - fvm::laplacian(kappaEff, T, "laplacian(kappa,T)") == fluid.heatTransfer(T) + radiation->ST(T) + fvOptions(rhoCp, T) ); Does the left-hand side of the equation mean the following? $\rho C_{p} \frac{\partial T}{\partial t}$ + $\rho C_{p} \nabla . (\Phi T)$ - $\Delta (kT)$ If that is the case, then why are density and Cp has taken out as constant? Shouldn't the volume of fluid averaged rhoCp depend on both time and space in a multiphase system? Please let me know if I'm missing something here as I'm quite new to heat transfer modelling. Many thanks, Gowthaman

December 4, 2022, 20:40		#2
CorbinMG New Member Corbin G Join Date: Oct 2022 Location: Midwest, USA Posts: 11 Rep Power: 2	Hi Gowthaman, I think you are correct. At least for the transient term we can use the product rule to expand: $\frac{\partial \rho CpT}{\partial t} = T \frac{\partial \rho Cp}{\partial t} + \rho Cp \frac{\partial T}{\partial t}$ Using algebra to rearrange we have the below equation. The right hand side corresponds, in so far as I can tell, to what is implemented in icoReactingMultiphaseInterFoam TEqn.H. Therefore, effectively the LHS is being calculated. $\rho Cp \frac{\partial T}{\partial t} = \frac{\partial \rho CpT}{\partial t} - T \frac{\partial \rho Cp}{\partial t}$ Now, why code the right hand side instead of just putting $\rho Cp \frac{\partial T}{\partial t}$ directly? I have a theory: fvm::ddt(rhoCp, T) makes an fvScalarMatrix data type. OpenFOAM, in my experience, does not allow the multiplication of volScalarField by fvScalarMatrix or it will give error at compilation. That is to say, if we had rhoCp stored as volScalarField, rhoCpfvm::ddt(T) would give volScalarFieldfvScalarMatrix compilation error. Fauster has documented this volScalarFieldfvScalarMatrix compilation error, but no one has responded a way to get around it: How to multiply volScalarField and fvScalarMatrix ? EDIT: Thank you to newGuyAtCFD for pointing out my oversight. Please regard my aforementioned theory as incorrect. volScalarFieldfvScalarMatrix IS possible. But, fvScalarMatrixvolScalarField gives compilation error: Code: volScalarField rhoCp1 = rho1alpha1mixture.thermo1().Cp() + rho2alpha2mixture.thermo2().Cp(); fvScalarMatrix eEqn ( rhoCp1fvm::ddt(T) // compiles OK! //fvm::ddt(T)rhoCp1 // gives compilation error! == fvOptions(rhoCp1, T) ); Last edited by CorbinMG; December 14, 2022 at 11:34.*

August 9, 2023, 10:00		#5
sabrahams New Member S Abrahams Join Date: Mar 2022 Location: UK Posts: 14 Rep Power: 3	Hi everyone, I wonder if anyone can help me with a follow-up question please? In compressibleInterFoam in OF9, the TEqn is formulated as Code: fvm::ddt(rho, T) + fvm::div(rhoPhi, T) - fvm::Sp(contErr, T) - fvm::laplacian(turbulence.alphaEff(), T) + ( fvc::div(fvc::absolute(phi, U), p)()() // - contErr/rhop + (fvc::ddt(rho, K) + fvc::div(rhoPhi, K))()() - (U()&(fvModels.source(rho, U)&U)()) - contErrK ) ( alpha1()/mixture.thermo1().Cv()() + alpha2()/mixture.thermo2().Cv()() ) == fvModels.source(rho, T) In this case, is used instead of but I believe it should still be inside the derivatives since the averaged can vary in time and space. I believe the TEqn should be equivalent to $\frac{\partial}{\partial t}(\rho C_v T)+\nabla\cdot(\rho C_v U T) + \frac{\partial}{\partial t}(\rho k)+\nabla\cdot(\rho U k)+\nabla \cdot (pU)-\nabla\cdot (K \nabla T)=S,$ but the formulation above seems to be equivalent to $\frac{C_{1}C_{2}}{{\alpha_1 C_{2}+\alpha_2 C_{1}}} \left[\frac{\partial}{\partial t}(\rho T)+\nabla\cdot(\rho U T) \right]+ \frac{\partial}{\partial t}(\rho k)+\nabla\cdot(\rho U k)+\nabla \cdot (pU)-\nabla\cdot (K \nabla T)=S.$ Can anyone help me to understand how has been taken out in this way? Many thanks, SAbrahams Last edited by sabrahams; August 9, 2023 at 13:16. Reason: spelling*

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Radiation Models in General and the P1 implementation	Tobi	OpenFOAM Running, Solving & CFD	8	September 21, 2021 05:59
Issues in FGM combustion model implementation	Lisandro Maders	OpenFOAM Programming & Development	15	April 22, 2020 19:18
Explicit source term implementation	wvn	OpenFOAM Programming & Development	0	November 14, 2018 11:31
Implementation issues of fvSchemes / laplacianScheme, in particular gaussLaplacianSch	thomek	OpenFOAM Programming & Development	0	October 18, 2010 05:10
Please explain the implementation of species transport Eqn in reactingFoam	kallipygian	OpenFOAM Running, Solving & CFD	0	October 13, 2008 07:29