CFD Online Discussion Forums - Improve simpleFoam convergence

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Improve simpleFoam convergence (https://www.cfd-online.com/Forums/openfoam-solving/78354-improve-simplefoam-convergence.html)

Quote:

Dear Matey
But if i inizialized my simulation with a field very precise, I must not use necessarily a very low tolerance or not?

Yes, you should do! The precise field for initialization gets "unprecise" immediately on the new mesh.

Quote:

Post my solution. The source for mapfields utility is the same for all. I change tolerance convergence.

Although your results for tau/tau_0 look stable after reaching 1e-2, it really is a very high tolerance criteria! I use at least 1e-4 for simpleFoam. The other results (U for example) will differ much more, I suppose. Well, I hope you are not running nuclear power plants or passenger air planes with your simulations ;)

No I'm not simulating a nuclear power plant! :D But also u profile is good, i think that I'll use 1e-3 tolerance convergence. I know the importance of tolerance i made structural simulation for a wing with nastran and I know the its importance

Hi
Do you know a way to interface my openfoam simulation with a matlab script that use OpenFoam results?

The best interface is interaction via files, I think...
I found this thread where you had problems starting OpenFOAM from Matlab:
http://www.cfd-online.com/Forums/ope...de-matlab.html

Do you still have problems in doing so? If so, try

Code:

unix('foamExec simpleFoam')

since this should set your environment variables properly.

Otherwise

Code:

unix('source path/to/OpenFOAMs/bashrc; simpleFoam')

could work.

For the data you need in Matlab:
Do you only need values for shear stress on the wall?
Is it enough to have coordinates for each shear stress value, or do you need the full mesh structure?
Do you use a more sophisticated transport model than newtonian flow?
Are you using OpenFOAM in parallel?

I have some code snippets here that would write a simple ";"-separated .csv file which you can parse in Matlab.

If I use your command I have this:

unix('foamExec blockMesh')
/bin/bash: foamExec: command not found

I only need values for shear stress on the wall, and it is enough to have coordinates for each shear stress value;

"Do you use a more sophisticated transport model than newtonian flow?" ->> No
Are you using OpenFOAM in parallel? ->> No (maybe later)

Thanks
Daniele

What about the other command: unix('source path/to/OpenFOAMs/bashrc; simpleFoam') ?

"path/to/OpenFOAMs" must be replaced with the full path to your OpenFOAM's installation directory, than the "bashrc" file follows, which includes the environment for OpenFOAM. Than there is a ";", followed by another command (simpleFoam) to be executed in the just set environment...

What's the name of the patch, you need the shear stress values for? Is it "bottom"?

I do:
unix('/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/etc/bashrc; blockMesh')
and

/bin/bash: /home/acconcia/OpenFOAM/OpenFOAM-1.6.x/etc/bashrc: permission denied
/bin/bash: blockMesh: command not found

Patch name is "bottom"

How long do you work with OpenFoam? Do you use it for university or work? I'm star to use is one month ago, and I like it, it's very flexible.

unix('/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/etc/bashrc; blockMesh')

Now It works, I changed matlab permission

Thanks

Hi Daniele,

here we go:

Go to the simpleFoam source directory:
"~/OpenFOAM/OpenFOAM-1.6.x/applications/solvers/incompressible/simpleFoam/"
The version number might be different for your system.

Create a new file there with name "write.H". Paste this code in there:

Code:

// write matlab file

{

    Info << "Writing wall shear stress for matlab!" << endl;



    word wallPatchName = "bottom";

    Info << "Searching for patch " << wallPatchName << endl;



    // Check, if the patch name exists:

    label patchID = mesh.boundaryMesh().findPatchID(wallPatchName);

    if (patchID < 0)

    {

        Info << "No patch found with name \"" << wallPatchName << "\"!"

             << endl;

    }

    else

    {

        /* for laminar case:

        Info<< "Reading viscosity nu\n" << endl;

        dimensionedScalar nu_

        (

            laminarTransport.lookup("nu")

        );

        */

        // calculating wall shear rate

        volVectorField wallGradU

        (

                IOobject

                (

                        "wallGradU",

                        runTime.timeName(),

                        mesh,

                        IOobject::NO_READ,

                        IOobject::AUTO_WRITE

                ),

                mesh,

                dimensionedVector

                (

                        "wallGradU",

                        U.dimensions()/dimLength,

                        vector::zero

                )

        );



        forAll(wallGradU.boundaryField(), patchi)

        {

            wallGradU.boundaryField()[patchi] =

                -U.boundaryField()[patchi].snGrad();

        }



        // calculating wall shear stress

        volVectorField tau

        (

                IOobject

                (

                        "tau",

                        runTime.timeName(),

                        mesh,

                        IOobject::NO_READ,

                        IOobject::AUTO_WRITE

                ),

                //laminar case: nu_ * wallGradU

                turbulence->nuEff() * wallGradU

                // turbulence->nu() * wallGradU

        );



        // Pointer to the patch we want to have shear stress for:

        const polyPatch& cPatch = mesh.boundaryMesh()[patchID];

        label nFaces = cPatch.size();



        pointField faceCenterCoords(nFaces, vector(0,0,0));

        pointField faceAreas(nFaces, vector(0,0,0));

        pointField wallShearStress(nFaces, vector(0,0,0));



        label runFaces = 0;



        // collecting the interesting data

        for (int i=0; i<nFaces; i++)

        {

            faceCenterCoords[runFaces] = mesh.Cf().boundaryField()[patchID][i];

            faceAreas[runFaces] = mesh.Sf().boundaryField()[patchID][i];

            wallShearStress[runFaces] = wallGradU.boundaryField()[patchID][i];

            runFaces++;

        }



        //  make a cute filename

        fileName casePath = cwd();//casePath.name();

        fileName caseName = casePath.name();

        fileName myFile = caseName+"_wallShearStress.csv";

        Info << "Data is written to file " << myFile << endl;



        // create a new file

        OFstream *myStream = NULL;

        myStream = new OFstream(myFile);



        for (int i=0; i<nFaces; i++)

        {

            *myStream << i << "; "

                    // coordinates on face centers:

                    << mesh.Cf().boundaryField()[patchID][i].component(0) << "; "

                    << mesh.Cf().boundaryField()[patchID][i].component(1) << "; "

                    << mesh.Cf().boundaryField()[patchID][i].component(2) << "; "



                    // wall shear stress as a vector:

                    << tau.boundaryField()[patchID][i].component(0) << "; "

                    << tau.boundaryField()[patchID][i].component(1) << "; "

                    << tau.boundaryField()[patchID][i].component(2) << "; "



                    // magnitude of wall shear stress:

                    << mag(tau.boundaryField()[patchID][i]) << endl;

        }



    }

}

Then open the simpleFoam.C file. Add this line to the includes at the top:

Code:

#include "OFstream.H"

Behind the runTime loop of simpleFoam paste the following two lines, so that it looks like:

Code:

        ...

        #include "convergenceCheck.H"

    }

    // writing additional data for matlab

#   include "write.H" // <--- this is the important one

    ...

In the simpleFoam directory call

Code:

wclean

wmake

Now if you are running simpleFoam an extra file with name "your_case_name_wallShearStress.csv" is written. It's format is:
number; coordX; coordY; coordZ; wallShearStressX; wallShearStressY; wallShearStressZ; magnitude(wallShearStress)

I haven't tested this code, so use it with care! Check and double check, if the wall shear stress is calculated really correctly!!!
Have a look a line 62, where the wall shear stress is calculated:

Code:

turbulence->nuEff() * wallGradU

is just a guess, since I don't have experience with turbulence. It might be nu, or nut or something totally different there...

Have fun :-)

Martin

p.s.: I'm using OpenFOAM for seven month now... but I'm still learning, of course ;-) And I'm using it for work.

Dear Martin
Thanks for your code, is a gold mining! There are many things I want to learn to. I'll change the computation of wallShearStress, I think that i'll use the openfoam code for this and I add it to write.h.

Daniele

MRF simple foam linear upwind: convergence troubles

Hi,
I'm trying to set a linearUpwind MRF simpleFoam simulation of a cooling fan. The mesh has been imported from GAMBIT (8.5 e+6 cells, not bad quality) and the simulation diverges.Here attached: log, fvSchemes,fvSolution. Could you please have a look in order to give me advices about settings?
thanks
Aldo

But if I want extract also k with code? How can i modify the code post previously?

Hi Daniele,

what about adding

Code:

<< k.boundaryField()[patchID][i] << "; "

to the "myStream" loop?
Martin

Hi Martin
It is that I do...I did a syntax error probably.
Thanks!

Daniele

Hi
Now I try to use a cluster to increase my speed, and so i'm traying tu use OpenFoam parallel utility. But when i run decomposePar i have this error:

FOAM FATAL IO ERROR:

Cannot find 'value' entry on patch bottom of field epsilon in file "/u/acconcia/OpenFOAM/acconcia-1.6/run/blayer4/0/epsilon"
which is required to set the values of the generic patch field.
(Actual type epsilonWallFunction)

Please add the 'value' entry to the write function of the user-defined boundary-condition
or link the boundary-condition into libfoamUtil.so

file: /u/acconcia/OpenFOAM/acconcia-1.6/run/blayer4/0/epsilon::boundaryField::bottom from line 49 to line 52.

From function genericFvPatchField<Type>::genericFvPatchField(con st fvPatch&, const Field<Type>&, const dictionary&)
in file genericFvPatchField/genericFvPatchField.C at line 71.

My boundary condition are the same of the case that I use not in parallel and they haven't give me problem.

The best think you can do is to follow what the error message clearly says so (especially when it does say it so clearly). On patch "bottom" you have not prescribed value of epsilon. What is the BC for epsilon on bottom? It is probably some which needs a value.

Now why you do not need it in single but need it in parallel?
My guess is that you do not use k-eps but k-omega where BC for epsilon is not needed.
The decompose utility does not know what you will use for the run so it does decompose everything and checks for you BCs which is very kind of it.
But it's only my guess.

good luck

matej

These are my BC. And I'm sure that I'm using k-eps model, this BC have never been a problem.

Thanks

OK. then you have 2 possibilities:

(1) add the value uniform number; line to your bottom BC for the decomposer to be happy
(end remove it afterwards as the value is not needed by the wall functions (you can check it in doxygen)

(2) remove the need of it from the decomposer, recompile it and if it works report it

matej

Hi
I solved my problem, paralle is happy with a value!
To calculate wall shear stress with single processor I used Martin's code of post 29, but in parallel I can't use it: is possible a similar code to have a output at simulation stop? A tau.dat like output then i'll manipulate with matlab.

Hi Daniele,

not fully tested, but it should be a point to start from:

Code:

// write matlab file

{

    Info << "Writing wall shear stress for matlab!" << endl;



    word wallPatchName = "bottom";

    Info << "Searching for patch " << wallPatchName << endl;



    // Check, if the patch name exists:

    label patchID = mesh.boundaryMesh().findPatchID(wallPatchName);

    if (patchID < 0)

    {

        Info << "No patch found with name \"" << wallPatchName << "\"!"

             << endl;

    }

    else

    {

        /* for laminar case:

        Info<< "Reading viscosity nu\n" << endl;

        dimensionedScalar nu_

        (

            laminarTransport.lookup("nu")

        );

        */

        // calculating wall shear rate

        volVectorField wallGradU

        (

                IOobject

                (

                        "wallGradU",

                        runTime.timeName(),

                        mesh,

                        IOobject::NO_READ,

                        IOobject::AUTO_WRITE

                ),

                mesh,

                dimensionedVector

                (

                        "wallGradU",

                        U.dimensions()/dimLength,

                        vector::zero

                )

        );



        forAll(wallGradU.boundaryField(), patchi)

        {

            wallGradU.boundaryField()[patchi] =

                -U.boundaryField()[patchi].snGrad();

        }



        // calculating wall shear stress

        volVectorField tau

        (

                IOobject

                (

                        "tau",

                        runTime.timeName(),

                        mesh,

                        IOobject::NO_READ,

                        IOobject::AUTO_WRITE

                ),

                //laminar case: nu_ * wallGradU

                turbulence->nuEff() * wallGradU

                // turbulence->nu() * wallGradU

        );

        

        // Pointer to the patch we want to have shear stress for:

        const polyPatch& cPatch = mesh.boundaryMesh()[patchID];

        label nFaces = cPatch.size();



        pointField faceCenterCoords(nFaces, vector(0,0,0));

        pointField faceAreas(nFaces, vector(0,0,0));

        pointField wallShearStress(nFaces, vector(0,0,0));



        label runFaces = 0;



        // collecting the interesting data

        for (int i=0; i<nFaces; i++)

        {

            faceCenterCoords[runFaces] = mesh.Cf().boundaryField()[patchID][i];

            faceAreas[runFaces] = mesh.Sf().boundaryField()[patchID][i];

            wallShearStress[runFaces] = tau.boundaryField()[patchID][i];

            runFaces++;

        }



        // for parallel

        reduce(nFaces, sumOp<label>());

        Info << "Number of global faces: " << nFaces << endl;

        



        //  make a cute filename

        fileName casePath = cwd();//casePath.name();

        fileName caseName = casePath.name();

        fileName myFile = caseName+"_wallShearStress.csv";

        Info << "Data is written to file " << myFile << endl;



        // create a new file

        OFstream *myStream = NULL;

        if (Pstream::master())

        {

            myStream = new OFstream(myFile);

        }



        // slaves send data to master, master writes data to file

        if (Pstream::parRun())

        {

            if (Pstream::myProcNo() != Pstream::masterNo())

            {

                OPstream toMaster(Pstream::blocking, Pstream::masterNo());

                toMaster << faceCenterCoords;

                toMaster << faceAreas;

                toMaster << wallShearStress;

            }

            else // master part

            {

                // first write own data

                for (int i=0; i<faceCenterCoords.size(); i++)

                {

                    *myStream << i << ";"

                        << faceCenterCoords[i].component(0) << "; "

                        << faceCenterCoords[i].component(1) << "; "

                        << faceCenterCoords[i].component(2) << "; "



                        << wallShearStress[i].component(0) << "; "

                        << wallShearStress[i].component(1) << "; "

                        << wallShearStress[i].component(2) << "; "



                        << mag(wallShearStress[i]) << endl;

                }



                label run = faceCenterCoords.size();

                

                // then receive slave data and write

                pointField bufferFaceCenterCoords;

                pointField bufferFaceAreas;

                pointField bufferWallShearStress;



                

                for (int slave=Pstream::firstSlave(); slave <= Pstream::lastSlave(); slave++)

                {

                    IPstream fromSlave(Pstream::blocking, slave);

                    fromSlave >> bufferFaceCenterCoords;

                    fromSlave >> bufferFaceAreas;

                    fromSlave >> bufferWallShearStress;

                    

                    for (int i=0; i<bufferFaceCenterCoords.size(); i++)

                    {

                        *myStream << run << ";"

                            << bufferFaceCenterCoords[i].component(0) << "; "

                            << bufferFaceCenterCoords[i].component(1) << "; "

                            << bufferFaceCenterCoords[i].component(2) << "; "



                            << bufferWallShearStress[i].component(0) << "; "

                            << bufferWallShearStress[i].component(1) << "; "

                            << bufferWallShearStress[i].component(2) << "; "



                            << mag(bufferWallShearStress[i]) << endl;

                        run++;

                    }

                }

            }

        }

        else // single processor only

        {

            for (int i=0; i<nFaces; i++)

            {

                *myStream << i << "; "

                        // coordinates on face centers:

                        << mesh.Cf().boundaryField()[patchID][i].component(0) << "; "

                        << mesh.Cf().boundaryField()[patchID][i].component(1) << "; "

                        << mesh.Cf().boundaryField()[patchID][i].component(2) << "; "



                        // wall shear stress as a vector:

                        << tau.boundaryField()[patchID][i].component(0) << "; "

                        << tau.boundaryField()[patchID][i].component(1) << "; "

                        << tau.boundaryField()[patchID][i].component(2) << "; "



                        // magnitude of wall shear stress:

                        << mag(tau.boundaryField()[patchID][i]) << endl;

            }

        }



    }

}

Martin