Hi,

I am interested in implementing the viscous heat dissipation term laplacian(mu,U) in the following energy equation:

solve
(
fvm::div(phi, T)
- fvm::laplacian(alphaEff, T)
- S*q/(rho*Cp) (<-source term)
- fvm::laplacian(mu, U) (dissipation term)
);
}

I am a beginner at openFoam so the question might be basic for some on this sight, sorry.

anyway. when trying to compile this the following error message starts like:

SOURCE_DIR=.
SOURCE=hSimpleFoam.C ; g++ -m32 -Dlinux -DDP -Wall -W -Wno-unused-parameter -Wold-style-cast -O3 -DNoRepository -ftemplate-depth-30 -I/home/erik/OpenFOAM/OpenFOAM-1.3/src/finiteVolume/lnInclude -I/home/erik/OpenFOAM/OpenFOAM-1.3/src/turbulenceModels -I/home/erik/OpenFOAM/OpenFOAM-1.3/src/transportModels -I/home/erik/OpenFOAM/OpenFOAM-1.3/src/OpenFOAM/lnInclude -IlnInclude -I. -fPIC -pthread -c $SOURCE -o Make/linuxGcc4DPOpt/hSimpleFoam.o
TT.H: In function 'int main(int, char**)':
TT.H:40: error: no match for 'operator-' in 'Foam::operator-(const Foam::tmp<foam::fvmatrix<type> >&, const Foam::tmp<foam::geometricfield<type,> >&) [with Type = double](((const Foam::tmp<foam::geometricfield<double,> >&)((const Foam::tmp<foam::geometricfield<double,> >*)(& Foam::operator/(const Foam::tmp<foam::geometricfield<type,> >&, const Foam::dimensioned<double>&) [with Type = double, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh](((const Foam::dimensioned<double>&)((const Foam::dimensioned<double>*)(& Foam::operator*(const Foam::dimensioned<double>&, const Foam

Does anyone know what I am doing wrong

/Thanks Erik

[hjasak]

Nope, not like that: what you are trying to do here is to add a laplacian with U as a working variable into the equation for temperature. Does not make sense

It is basically something like (adjust for compressible fluid etc):

volTensorField gradU = fvc::grad(U);

the term you want is something like

(mu_l*(gradU + gradU.T()) && gradU)

This lot appears as the source in the energy equation.

Enjoy,

Hrv

thank you for your answer!

Im working on a incompressible flow (modification of simpleFoam) so I guess i dont need to adjust your formula.

I have two question on the suggested source term.

what is mu_|?
what is gradU.T()?

my case is a channel with hydraulic diameter of 53mm and 11 meters long. The channel is for an air flow of 20 m/s(approx incompressible). im hoping this extra term will rise the temperature 5 more degrees so that my simulation fits experimental data.

Thanks again
/Erik

[hjasak]

mu_l is laminar viscosity. gradU.T() would be a transpose of the gradU tensor. For incompressible flows, you can just do mu_l*magSqr(gradU), that should do the trick. Don't forget to add turbulence dissipation (epsilon) to the energy blance.

Hrv

Thank you once again,
another novice question follows I am afraid.

How is epsilon to be added and do you know where I can find ducumentation of this so I can have som sort of theoretical backupp for my thesis work.

This formula was no ploblem to add to the energy equation but I wouldent expect you to be surpriced either.

/Erik

[alimea]

Originally Posted by hjasak

Nope, not like that: what you are trying to do here is to add a laplacian with U as a working variable into the equation for temperature. Does not make sense

It is basically something like (adjust for compressible fluid etc):

volTensorField gradU = fvc::grad(U);

the term you want is something like

(mu_l*(gradU + gradU.T()) && gradU)

This lot appears as the source in the energy equation.

Enjoy,

Hrv

Hi
I also want to add viscous dissipation to energy eqn. but my fluid is not Newtonian and has a special stress tensor. So the work of stress tensor field is "tau && grad(U)"

1- is it a correct relation for work of stress tensor field? or I should write:
tau && [grad(U) + transpose of (grad(U))]

2- is it correct to write:

solve
(
fvm::div(phi, T)
- fvm::laplacian(alphaEff, T)
- tau && grad(U)
);

thank you

[anthony761]

I think now, it can just be enabled in fvOption with

dissiapation1
{
    type            viscousDissipation;
    selectionMode   cellSet;
    cellSet         sourceCells1;
}

see: https://www.openfoam.com/documentati...ssipation.html