CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   div(phi,U) in an incompressible solver (http://www.cfd-online.com/Forums/openfoam/89269-div-phi-u-incompressible-solver.html)

 fisch June 8, 2011 11:47

div(phi,U) in an incompressible solver

Hi Foamers,

does anybody know if div(phi,U) in an incompressible solver (like simpleFoam) is calculating the "full" divergence term of phi*U or is it directely introducing the incompressibility conditions that the calculation would be reduced to the half.

For a better understanding what i mean i will write it analytical for 2D motion (i will leave out the density):

Option a) div(U,U) = u*( du/dx+dv/dy) + u*du/dx + v*du/dy
Option b) div(U,U) = u*du/dx + v*du/dy (because the term in the brackets satisfies div(U)=0)

Which option is openFoam using?

Thanks a lot,
rupert

 santiagomarquezd June 8, 2011 13:44

Rupert, FOAM solves the "weak" form if this term. When you use FVM, integrals are volumetric at the beginning but using the Gauss Theorem you don't have to use any derivatives but only values at faces, because you have a surface integral:

int_{Omega} div(U*U) dOmega=int_{Gamma} U*U&d_Gamma=sum_f U_f*U_f&S_f=sum_f U_f*phi_f

where & is the dot product, Omega is the control volume and Gamma is its border and f indicates quantities at faces. phi is the flux U_f&S_f.

Regards.

 vatavuk June 9, 2011 07:21

Hi Rupert,
Just complementing Santiago's answer, this means that, for the x momentum equation, you have alternative a) integrated over the cell volume.
Paulo

 fisch June 9, 2011 07:46

Hi Paulo and Santiago,

So if i want to add to an equation one more term i have to integrate it over the cell volume or just multiply the cell center value with the Volume of the cell, right?

For example if i want to add a value S (like a source term) i have to integrate this value over the cell volume, too, right?

Thanks

rupert

 santiagomarquezd June 9, 2011 07:51

Rupert, the integration is part of the method and is implied using FOAM. Adding S to the equation starts a chain of events that finally integrate the source over each cell. The other option is to use the fvm::Sp().

Regards.

 fisch June 9, 2011 09:34

Hello Santiago,
does that mean that the integration is implied in the discretization schemes (like in e.g. div(phi,U)) or is it automatically implied while solving an equation???
The difference would be that i don't have to integrate my source term my own if it is done by the solve() procedure...
Can you understand what i mean??

As far as i get it out of the source code the Sp() function is anyhow multiplying with the cell Volumes; but i had no success to use it right :-/ ...

Further: what is wrong if i type: volScalarField meshVols = U.mesh().V();
There is a compiler error: error: conversion from ‘const Foam::DimensionedField<double, Foam::volMesh>’ to non-scalar type ‘Foam::volScalarField’ requested

thanks a lot,
rupert

 sabin.ceuca June 10, 2011 11:32

Quote:
 Originally Posted by fisch (Post 311273) Further: what is wrong if i type: volScalarField meshVols = U.mesh().V(); There is a compiler error: error: conversion from ‘const Foam::DimensionedField’ to non-scalar type ‘Foam::volScalarField’ requested Maybe you have some answers. thanks a lot, rupert
Hi Rupert,

tmp<volScalarField> cellVolume
(
new volScalarField
(
IOobject
(
"cellVolume",
runTime.timeName(),
mesh,
IOobject::NO_WRITE
),
mesh,
dimensionedScalar("zero",dimensionSet
(0, 3, 0, 0, 0, 0, 0), 0.0)
)
);
cellVolume().internalField() = mesh.V();

This part should store the volumes of your cells. I don't really understand why you call your volume like U.mesh().V ?

Regards,
sabin

 fisch June 14, 2011 01:42

Quote:
 Originally Posted by santiagomarquezd (Post 311249) Rupert, the integration is part of the method and is implied using FOAM. Adding S to the equation starts a chain of events that finally integrate the source over each cell. The other option is to use the fvm::Sp(). Regards.
Santiago,
do i have to use some integration over the cell volume inside an equation for the additional source term S or is it done automatically so that i have to add only the term with " + S" or do i need something else??

rupert

 Anne Lincke June 25, 2013 12:16

Good evening,
I have the same question.
I have added an explicit source term rhs in the momentum equation

HTML Code:

```tmp<fvVectorMatrix> UEqn         (             fvm::div(phi, U)             + turbulence->divDevReff(U)               +rhs )```
Is this source term automatically multiplied by the control volumes = integrated?
In my case I would like to add a face-based source term which includes the face magnitudes. Therefore I suppose that I need to divide my source term by the control volume, as I do not want it to be multiplied as the multiplication with the face magnitude symbols an integration over the face already.

Can someone please verify that the source term is automatically integrated if I insert it in the UEqn like stated above?

Kind Regards
Anne

 fumiya June 25, 2013 18:51

Hi,

You can use the cell center value not the cell integrated value when you specify
the explicit source term in the UEqn.

Hope that helps,
Fumiya

 Anne Lincke June 26, 2013 02:56

Dear Fumiya,

How can I switch between cell-centered and cell-integrated value?

Thank you,

Anne Lincke

 Anne Lincke June 27, 2013 14:06

Dear foamers,

I have written a face-based source which I would like to include in the UEqn.
I assume that this term will automatically multiplied with the cell-volume as it is explicit?
As the term corresponds to the integration over the faces it is already scaled with the face-magnitude and does not need to be scaled by the cell volume any more.

Therefore I divided the term by the cell volume, but the code does not converge :(

In the following a sketch of the code.

HTML Code:

```for( label faceI=0; faceI < mesh.nInternalFaces(); faceI++) {     label P = owner[faceI];     label N = neighbour[faceI];     rhs[P] = rhs[P] + mesh.Sf()[faceI]*Uf[faceI]*1/mesh.V()[P]; }```
Can I somehow avoid the automatic scalation with the cell center volume inside the UEqn?

Thank you very much for an answer.

Anne

 eysteinn June 28, 2013 08:40

Quote:
 Originally Posted by Anne Lincke (Post 436396) Dear foamers, I have written a face-based source which I would like to include in the UEqn. I assume that this term will automatically multiplied with the cell-volume as it is explicit? As the term corresponds to the integration over the faces it is already scaled with the face-magnitude and does not need to be scaled by the cell volume any more. Therefore I divided the term by the cell volume, but the code does not converge :( In the following a sketch of the code. Code: ```for( label faceI=0; faceI < mesh.nInternalFaces(); faceI++) {     label P = owner[faceI];     label N = neighbour[faceI];     rhs[P] = rhs[P] + mesh.Sf()[faceI]*Uf[faceI]*1/mesh.V()[P]; }``` Can I somehow avoid the automatic scalation with the cell center volume inside the UEqn? Thank you very much for an answer. Anne
Hi Anne,

Yes it is automatically multiplied with the cell volume.

I think you might be looking for the reconstruct operator to get the value in
the cell center:
Code:

```surfaceScalarField phi         = fvc::interpolate(U) & mesh.Sf();                 volVectorField UfromPhi("UfromPhi",fvc::reconstruct(phi) );```
/Eysteinn

 Anne Lincke July 1, 2013 10:40

Thank you, I think I found another reason for the non-convergence of my code.
Nevertheless this implementation helped me a lot to understand how OpenFOAM treats the source terms.

Kind Regards
Anne

 All times are GMT -4. The time now is 06:09.