[Researcher23]

Dear Forum,

I would like to get (and use) the information about the distance to the next wall within fvOptions. I've seen that there is something called wallDist in the OpenFoam code:

https://github.com/OpenFOAM/OpenFOAM...ist/wallDist.H

My code within fvOptions was the following:

volScalarField WallDistant
(
IOobject
(
"WallDistant",
mesh_.time().timeName(),
mesh_,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh_,
dimensionedScalar("WallDistant", dimensionSet(0,1,0,0,0,0,0), 0)
);

WallDistant = wallDist(mesh).y();

But my attempt was not successful. I got the following error message:

/manni/data/stw/OpenFoamRuns/TH2_42/constant/fvOptions.massSource.scalarCodedSourceCoeffs: In member function ‘virtual void Foam::fv::sourceMassFvOptionscalarSource::addSup(F oam::fvMatrix<double>&, Foam::label)’:
/manni/data/stw/OpenFoamRuns/TH2_42/constant/fvOptions.massSource.scalarCodedSourceCoeffs:100:3 0: error: invalid use of non-static member function
/manni/data/stw/OpenFoamRuns/TH2_42/constant/fvOptions.massSource.scalarCodedSourceCoeffs: In member function ‘virtual void Foam::fv::sourceMassFvOptionscalarSource::addSup(c onst volScalarField&, Foam::fvMatrix<double>&, Foam::label)’:
/manni/data/stw/OpenFoamRuns/TH2_42/constant/fvOptions.massSource.scalarCodedSourceCoeffs:100:3 0: error: invalid use of non-static member function
make: *** [Make/linux64GccDPInt32Opt/codedFvOptionTemplate.o] Error 1


--> FOAM FATAL IO ERROR:
Failed wmake "dynamicCode/sourceMass/platforms/linux64GccDPInt32Opt/lib/libsourceMass_3da197f3cc357d741f1a55ea5ea42bbaf0e3 83a5.so"

Could someone please give me a hint how to get the wall distance information within my fvOptions code?

Thanks,
R.

[luther1990]

try

WallDistant = wallDist(mesh_).y();

[Researcher23]

Dear Luther,

thanks for your answer! It works now with your solution. But first I have to include

#include "wallDist.H"

in my code.

Regards,
R.

[Scram_1]

Hi,
I see that you want the nearest distance from the wall for each cell in the mesh.
Is it possible to get the distance from a particular cell in the mesh to the wall using wallDist() without computing this distance for other cells? I have the cellID for the cell. But wallDist(mesh_(celli)).y() gives an error. Is there a way to get this distance for a particular cell?

Thanks!

Best,
Scram_1

[Andrea1984]

Hi Researcher23,

could you share a complete example with your solution? Where exactly did you include "wallDist.H" in your code?

Many thanks,
Andrea

[Researcher23]

I used it in fvOptions as a scalarCodedSource.

The code in fvOptions was:

#include "wallDist.H"

volScalarField WallDistance
(
IOobject
(
"WallDistance",
mesh_.time().timeName(),
mesh_,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh_,
dimensionedScalar("WallDistance", dimensionSet(0,1,0,0,0,0,0), 0)
);

WallDistance = wallDist(mesh_).y();

I have to add in fvSchemes:

wallDist
{
method meshWave;
}

[Andrea1984]

Thanks for the quick reply.

This is what I have been trying to do but I have just realised I was mispelling the name of the header file

[DJF]

I want to use wallDist to create a velocity profile on a non-planar surface. I copied this solution to my fvOptions file and get the following errors:
1) Cannot open include file ".../wallDist.H" while reading dictionary ".../fvOptions"

2) if I comment #include wallDist.H I get:
"ill defined primitiveEntry starting at keyword 'volScalarField' on line 19 and ending at line 35"
[0]
[0] file: .../fvOptions at line 35.
[0]
[0] From void Foam:rimitiveEntry::readEntry(const Foam::dictionary&, Foam::Istream&)
[0] in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 236.

Any suggestions?

[s1291]

If you are using OpenFOAM ESI version (e.g. v2106) no need to compile any code or use the fvOptions framework. You simply run:

checkMesh -writeAllFields

Among the output fields, you will find wallDistance volScalarField under 0 directory.

[DJF]

Thanks for the quick reply. I have now in 0/wallDistance and want to use it for the inlet boundary in U as an expression:

expression
#{
vector(Uref/log(zRef/z0)*log(wallDistance/z0), 0, 0)
#};

but Object wallDistance does not exist

Any Ideas how to use the new volScalarField?

[louisgag]

In case someone is still looking for a simple solution, here's an example function object to put in the functions{...} section of your controlDict:

wallDist1
{
    type                coded;
    libs                (utilityFunctionObjects);
    name                wallDistance;
    executeControl      timeStep;
    executeInterval     4;
    writeControl        none;

    codeInclude
    #{
        #include        "wallDist.H"
    #};

    codeExecute
    #{
    auto* wallDistancePtr =
                mesh().getObjectPtr<volScalarField>("wallDistance");
    if (!wallDistancePtr)
    {
        Info<< "Create wallDistance field" << nl;
              wallDistancePtr = new volScalarField
        (
        IOobject
        (
        "wallDistance",
        mesh().time().timeName(),
        mesh(),
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
        ),
        mesh(),
        dimensionedScalar("wallDistance", dimensionSet(0,1,0,0,0,0,0), 0)
        );
    }
    regIOobject::store(wallDistancePtr);
    auto& wallDistance = *wallDistancePtr;
    Info<< "Computing wallDistance field\n" << endl;
    wallDistance = wallDist::New(mesh()).y();
    #};
}

[armitatz]

Originally Posted by louisgag

In case someone is still looking for a simple solution, here's an example function object to put in the functions{...} section of your controlDict:

wallDist1
{
    type                coded;
    libs                (utilityFunctionObjects);
    name                wallDistance;
    executeControl      timeStep;
    executeInterval     4;
    writeControl        none;

    codeInclude
    #{
        #include        "wallDist.H"
    #};

    codeExecute
    #{
    auto* wallDistancePtr =
                mesh().getObjectPtr<volScalarField>("wallDistance");
    if (!wallDistancePtr)
    {
        Info<< "Create wallDistance field" << nl;
              wallDistancePtr = new volScalarField
        (
        IOobject
        (
        "wallDistance",
        mesh().time().timeName(),
        mesh(),
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
        ),
        mesh(),
        dimensionedScalar("wallDistance", dimensionSet(0,1,0,0,0,0,0), 0)
        );
    }
    regIOobject::store(wallDistancePtr);
    auto& wallDistance = *wallDistancePtr;
    Info<< "Computing wallDistance field\n" << endl;
    wallDistance = wallDist::New(mesh()).y();
    #};
}

Excellent code... But
#1 There seems to be a quirk (or a bug). In cyclic BC it seems to give up.
bug.jpg
In this case left and right are cyclicAMI bc's. In the left the distance seems to be 0. It should not be 0 and even better it should wrap around. Probably it is because of the computation of the walldistance method...
#2 Can this code be implemented in a solver directly? I tried to implement it to openFoam2112 and laplacianFoam but I get errors. Obviously a copy/paste would not work. Can you point to a way to implement it?
Andrew

[louisgag]

Hi,
whether it works or not depends on which function you used to compute the wall distance, (fvSchemes), I used meshWave
you may be able to implement that in a solver, but you may have to access the pointer from the turbulence model which in turn gives you the distance.. i don't recommend trying this unless you know c++ and OpenFOAM or have a lot of time to try around

[armitatz]

I used meshwave in fvSchemes


C++ well ok but not that much...


Well my guess was that meshWave can calculate distances regardless of turbulence etc. That it is a piece of code that can be used independently. Therefore it could be used for creating a distance field for any other use.


bug2.jpg
In this case left and right are patches (not cyclicAMI). The distance is calculated correctly and is not 0 at the left border. There seems to be a bug here in the presence of cyclic borders.

[louisgag]

the patches are walls?

[armitatz]

The internal boundaries are set as walls. The distance does not work with common patches. It needs walls because it is used in turbulence and turbulence needs walls to work.

Meshwave does not make the cut. I switched to Poisson and since it uses a solver the cyclic boundaries are respected. So problem solved! (https://www.openfoam.com/documentati...e-poisson.html)


bug4.jpg


I would like to ask two more things.
#1. How can I make the field at the beginning of the simulation before any other iteration? right now I use these settings in controlDict

    startFrom       startTime;
startTime       0;
stopAt          endTime;
endTime         30;
deltaT          1;
writeControl    adjustableRunTime;
writeInterval   1;
....


executeControl      timeStep;
     executeInterval     1000;
    writeControl        timeStep;
    timeStart           0;

and it shows in the second iteration.
#2 After the #1 how can I use it inside the solver? My plan is to use this field to calculate a coefficient based on distance.
Any help would be greatly appreciated

[armitatz]

ok. Finally I made it


Based on the above code from louisgag I added it as a field in a solver (laplacianFoam)
first a new field was added: TDist in createFields.H. This will be a new field and it will be used as a variable coefficient taking the place of the old fixed coefficient DT. It will be calculated as a value*distance instead of a fixed value before the change. The distance will be the distance from the walls and the value will be defined in transportProperties with the name DDT. It will have the same units of the old coefficient DT in the code so its units are [0 2 -1 0 ...]

volScalarField TDist
(
    IOobject
    (
        "TDist",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    mesh,
    dimensionedScalar(dimensionSet(0,2,-1,0,0,0,0), 0)
);

Then I changed DT to DDT (I recycled the entry)

volScalarField DDT
 (
    IOobject
    (
        "DDT",
        runTime.timeName(),
        mesh,
        IOobject::READ_IF_PRESENT,
        IOobject::AUTO_WRITE
    ),
    mesh,
    dimensionedScalar(dimensionSet(0,1,-1,0,0,0,0), Zero)
);

I changed the dimensions because I want to multiply it with the distance from the walls which has dimensions [m]. So the original DT [0 2 -1 ... ] has to become [0 1 -1 ...] since it will be multiplied with distance of units [0 1 0 ...]

After that I changed the rest of DT to DDT in createfields.H

Then in laplacianFoam.C the #include section becomes

#include "wallDist.H" // added line
 #include "fvCFD.H"
#include "fvOptions.H"
 #include "simpleControl.H"

and then

       TDist = DDT*wallDist::New(mesh).y();

        while (simple.correctNonOrthogonal())
        {
            fvScalarMatrix TEqn
            (
                fvm::ddt(T) - fvm::laplacian(TDist, T)
             ==
                fvOptions(T)
            );

            fvOptions.constrain(TEqn);
            TEqn.solve();
            fvOptions.correct(T);
        }

          #include "write.H"

Finally in write.H the DT changes to DDT and also transportProperties becomes

DDT              DDT [ 0 1 -1 0 0 0 0 ] 10;

After compilation and running:
bug5.jpg
Simple as that!