[sazabi2001]

Hi:

I'm quite new to OpenFOAM so I still having problem with the porous media setting.

1: I notice that there're some 'porous' solvers like rhoPorousSimpleFoam and set the porosityPorperties in the /constant folder, and some other solvers like rhoSimpleFoam can set the porous media in the fvOption. Are they the same? or rhoPorousSimpleFoam will do better in solving the same problem?

2: I have not idea how to set / use the porosity value in the solver. I read the PorousZone.h and PorousZone.c, it seems in (or before) OF 2.2 the porosity value is not in use. and from OF 2.4 on I can't find the PorousZone.h and PorousZone.c anymore, instead there is porousModel folder included porousModel.h and porousModel .c, also the some other think like DarcyForchheimer.h and DarcyForchheimer.c. I don't seem anything related to porosity value setting. Can anybody tell me where to find the definition of porosity in the solver files? Or how can I set the porosity in the solver and see the velocity changes accordingly?

3: I heard that the porosity is recognized by the time derivative term of some solvers (something like fvm::ddt(U) ?), but I still can't find or proof this. Also if the porosity only use in the time derivative term but not the convection term, that sounds strange too.

[deepbandivadekar]

Originally Posted by sazabi2001

2: I have not idea how to set / use the porosity value in the solver. I read the PorousZone.h and PorousZone.c, it seems in (or before) OF 2.2 the porosity value is not in use. and from OF 2.4 on I can't find the PorousZone.h and PorousZone.c anymore, instead there is porousModel folder included porousModel.h and porousModel .c, also the some other think like DarcyForchheimer.h and DarcyForchheimer.c. I don't seem anything related to porosity value setting. Can anybody tell me where to find the definition of porosity in the solver files? Or how can I set the porosity in the solver and see the velocity changes accordingly?

Did you find any answer to this question? It's boggling.. I don't seem to find where exactly we can supply the porosity value.

[jaydeep]

Originally Posted by deepbandivadekar

Did you find any answer to this question? It's boggling.. I don't seem to find where exactly we can supply the porosity value.

Refer to this:
https://github.com/OpenFOAM/OpenFOAM...tant/fvOptions

[deepbandivadekar]

Ok. So this is what I found out (which is rather not very complicated but somehow I was stuck for quiet some time) which perhaps will help someone.

When it comes to porosity value,

• solvers based on Darcy Forchheimer equation do not explicitely need it because the equation does not involve porosity (phi) but D and F vectors which in turn depend on porosity of the material. e.g specified in porosityProperties file
• There are no solvers based on original Darcy law. precisely because Darcy-Forchheimer and its successor versions evolve into Darcy itself for low velocity flows.
• In ANSYS Fluent, when we declare a region as porous, we have a chance to supply D, F as well as porosity. I suppose Fluent chooses out of this what it needs based on user's choice of solvers. (This difference with OpenFoam solvers confused me for a bit)

I'd like to know if there's any ambiguity in this.


Thanks

[deepbandivadekar]

Originally Posted by jaydeep

Refer to this:
https://github.com/OpenFOAM/OpenFOAM...tant/fvOptions

Not sure how missed this reply. But, Jaydeep, am inquiring about applying the porosity value to the zone and not Darcy coefficient (D) or Forchheimer coefficient (F). Do you know about that?

[jaydeep]

Hi,

Yes you can do that. Here's how I have done in the past:

Add toposet:

actions
(
    {
        name    face1;
        type    cellSet;
        action  new;
        source  surfaceToCell;
        sourceInfo
        {
        file            "constant/triSurface/face.stl";
        outsidePoints   ((0.7 1.5 0));         // definition of outside
        includeCut      true;              // cells cut by surface
        includeInside   false;             // cells not on outside of surf
        includeOutside  false;             // cells on outside of surf
        useSurfaceOrientation false;  // use closed surface inside/outside
                                      // test (ignores includeCut,
                                      // outsidePoints)
        nearDistance    -1;//-1             // cells with centre near surf
                                            // (set to -1 if not used)
        //- If > 0 : include cells with distance from cellCentre to surface
        //  less than nearDist.
        curvature       0.9;                // cells within nearDistance
        }
    }
    {
        name    porousSet;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set face1;
        }
    }
);

It creates
1. cellSet face1 from stl file face.stl -- you can use faceZone or any other cellSet with different sources, such as, boxToCell etc.

2. It assigns a new cellZone porousSet to face1 cellSet.

3. Add this cellZone in selection in fvOptions

porosity
{
    type            explicitPorositySource;
    active          true;
    selectionMode   cellZone;
    cellZone        porousSet;

    explicitPorositySourceCoeffs
    {
        selectionMode   cellZone;
        cellZone        porousSet;
        type            DarcyForchheimer;

        DarcyForchheimerCoeffs
        {
            d   d [0 -2 0 0 0 0 0] (5e7 5e7 5e7);
            f   f [0 -1 0 0 0 0 0] (0 0 0);
        }

    }
}

Hope this helps

[sazabi2001]

Originally Posted by deepbandivadekar

Did you find any answer to this question? It's boggling.. I don't seem to find where exactly we can supply the porosity value.

Thanks for the reply, I actually looked into this and have the answer .. sort of.

The solvers in openfoam, at least 3.x and 4.x, will not use any porosity value related to what I want. it only uses Darcy-Forchheimer method which is the pressure-loss rather than a actual porous medium. So, in other words I have to create my own solver with the capability to read the porosity value.

I want to have a solver that able to do heat transfer in porous medium, and I think I'm getting there.

[sazabi2001]

Originally Posted by deepbandivadekar

Ok. So this is what I found out (which is rather not very complicated but somehow I was stuck for quiet some time) which perhaps will help someone.

When it comes to porosity value,

• solvers based on Darcy Forchheimer equation do not explicitely need it because the equation does not involve porosity (phi) but D and F vectors which in turn depend on porosity of the material. e.g specified in porosityProperties file
• There are no solvers based on original Darcy law. precisely because Darcy-Forchheimer and its successor versions evolve into Darcy itself for low velocity flows.
• In ANSYS Fluent, when we declare a region as porous, we have a chance to supply D, F as well as porosity. I suppose Fluent chooses out of this what it needs based on user's choice of solvers. (This difference with OpenFoam solvers confused me for a bit)

I'd like to know if there's any ambiguity in this.


Thanks

Yes, I have the same conclusion too.. Anyway, openfoam dose not seem to do a great deal with the porous thing.

[svramana]

Originally Posted by sazabi2001

Yes, I have the same conclusion too.. Anyway, openfoam dose not seem to do a great deal with the porous thing.

Hi,
I am also trying to make custom solver for porous media.Have you got any success in this direction?. Let me know if you can share your source code .

Thanks in advance,

Regards,
S.V.Ramana

[svramana]

Does any one have any idea , how to calculate fixed coefficients inline with Darcy-forchheimer "D&F" coefficients?

Reards,

S.V.Ramana

[deepbandivadekar]

Originally Posted by svramana

Does any one have any idea , how to calculate fixed coefficients inline with Darcy-forchheimer "D&F" coefficients?

Reards,

S.V.Ramana

Been wondering that myself. Yet to find any source. Do respond here if you find anything.

[regard]

hi all
i have same problem...do you solve your problem?
how can i add porous media to the solver?

Tanks in advance

[ancolli]

Has anyone solved it?

in particular:

a) Why there is a porousSimpleFoam solver if the porous region can be implemented with fvOptions using any solver?

b) How I should modify codeAddSup in order to allow D and F variable coefficients? in particular, i do not fully understand the coordinateSystem set with regards to the source term: https://openfoamwiki.net/index.php/DarcyForchheimer

thanks in advance