[Karman123]

Hello everybody,
I am trying to set Dirichlet boundary conditions for the pressure which are unknown before runtime for the icoFoam solver at the outflow (and I am failing).
These Dirichlet values come from another calculation which depends on the solutions of icoFoam, so there is no way to do this with tableFile or csvFile.

My idea to achieve this is to create a modified version of the icoFoam Solver (called my_icoFoam).
In this new solver I edited my_icoFoam.C :
1. I created a new fvPatch for the outlet:

label outlet_patch_label = mesh.boundaryMesh().findPatchID("outlet");
const fvPatch& outlet_patch = mesh.boundary()[outlet_patch_label];

2. During runtime I tried to change the p-values at the adjacent cells:

forAll(outlet_patch, face_i){
    label curCellp = outlet_patch.faceCells()[face_i];
    p[curCellp] = value;
}

This has no effect at all.
I think the problem is that I declared the outflow boundary in the file case/0/p to:

boundaryField
{
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
}

I know that this must be possible somehow because chtMultiRegionSimpleFoam does the same thing to couple two regions with the partitioned approach.
Any tips on what I am doing wrong or how chtMultiRegionSimpleFoam solves this probem are highly appreciated.

[Karman123]

Nobody with any ideas?

Im really in a dead end here, any ideas would be helpful.

[ssss]

Maybe using groovyBC or swak4foam?

It will let you impose conditional conditions to your boundaryConditions, and you will be able to access runTime variables from it

Maybe I can help you with it which is your condition for changing the BC?

[wyldckat]

Greetings to all! And welcome to the forum Karman123!

Originally Posted by Karman123

Nobody with any ideas?

Uhm... here's an idea: A person should not simply take a pain pill for a headache that was caused by a hammer hitting one's head.

OK, joking aside, the problem here is that you might not be diagnosing properly the problem you have at hand.
Because from your description, it seems to me that you should first run icoFoam for a few iterations with a "zeroGradient" or "inletOutlet" or "outlerInlet" at the outlet; and then change the boundary type in the last iteration to "fixedValue" and continue the simulation from there. No solver coding required.

Then there is also the "mappedField" boundary type, which seems to do what you're looking for.

Better yet, have a look at the code documentation: http://www.openfoam.org/docs/cpp/ - look at the bottom of the page there, where you can find the "Boundary Conditions" link. From there you can see the various outlet boundary conditions that OpenFOAM has got and possibly one of them already does what you want to do.

Best regards,
Bruno

[Karman123]

Thank you very much for your replies.
Just to give some context, I am not using OpenFOAM professionally, but as a student (for the first time) on a project, which might explain the existance of a simple solution to my problem .

The project is to couple a 1D solver I already wrote in C++ to a 3D inflow region (which I try to compute with icoFoam).
So the pressure at the outlet boundary of the icoFoam-region is calculated by my own FV Code.

Originally Posted by ssss

Maybe using groovyBC or swak4foam?

It will let you impose conditional conditions to your boundaryConditions, and you will be able to access runTime variables from it

Maybe I can help you with it which is your condition for changing the BC?

If I understood groovyBC and swak4Foam correctly, these BCs can access internal field variables.
This part
https://openfoamwiki.net/index.php/C..._other_patches
seems to be interesting to me.
If I create a new patch in my modified icoFoam solver which contains the solutions from my 1D solver I could access that new patch from the BC-file.. correct?

Originally Posted by wyldckat

Greetings to all! And welcome to the forum Karman123!

Uhm... here's an idea: A person should not simply take a pain pill for a headache that was caused by a hammer hitting one's head.

OK, joking aside, the problem here is that you might not be diagnosing properly the problem you have at hand.
Because from your description, it seems to me that you should first run icoFoam for a few iterations with a "zeroGradient" or "inletOutlet" or "outlerInlet" at the outlet; and then change the boundary type in the last iteration to "fixedValue" and continue the simulation from there. No solver coding required.

Then there is also the "mappedField" boundary type, which seems to do what you're looking for.

Better yet, have a look at the code documentation: http://www.openfoam.org/docs/cpp/ - look at the bottom of the page there, where you can find the "Boundary Conditions" link. From there you can see the various outlet boundary conditions that OpenFOAM has got and possibly one of them already does what you want to do.

Best regards,
Bruno

Since my outlet BC should change with every time step your first suggestion would not work for my problem.

I cant find any explanations on "mappedField", only the code.
I will look into that a little more.

Thanks again and other suggestions are still welcome.

[ssss]

You could just create a volVectorField with your 1D field, and access to it from groovyBC, no need of creating a new patch.

[wyldckat]

Originally Posted by Karman123

The project is to couple a 1D solver I already wrote in C++ to a 3D inflow region (which I try to compute with icoFoam).
So the pressure at the outlet boundary of the icoFoam-region is calculated by my own FV Code.

Quick answer: Have a look at the tutorial folder "heatTransfer/buoyantSimpleFoam/externalCoupledCavity", since it somewhat looks like that it's what you're looking for. That tutorial essentially has a boundary condition coming from an outside application, where data is transferred via file.

[Karman123]

for anybody with a similar problem:

i used the solution "ssss" suggested. (I assumed coupling via file is slow)

1. install swak4foam
2. create a new solver (copy icoFoam and rename)
3. create a new volume scalar field in your createFields.H

    Info<< "Creating field for pressure coupling\n" << endl;
     volScalarField p_coupling
    (
        IOobject
        (
            "p_coupling",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("p_coupling", dimensionSet(0,2,-2,0,0,0,0), Foam::scalar(0))
    );

4. compute your boundary value in the main function (for example icoFoam.C) and set the coupling field to its value

        double value=compute_value(...);
        dimensionedScalar value_dim
        (
            "value_dim",
            dimensionSet(0,2,-2,0,0,0,0),
            scalar(value)
        ); 
        p_coupling=value_dim;

5. create a groovyBC for your pressure in 0/p with the variable name as value expression

    outlet
    {
        type groovyBC;
        valueExpression "p_coupling";
    }

6. PROFIT

thanks again ssss without you I might still be stuck