CFD Online Discussion Forums - Manual limiter of velocity doesn't work

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

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

- - Manual limiter of velocity doesn't work (https://www.cfd-online.com/Forums/openfoam-solving/114556-manual-limiter-velocity-doesnt-work.html)

Manual limiter of velocity doesn't work

Hi to everyone guys!

I'm experiencing this problem and I really don' t know what to do: I'm running with the solver adjointShapeOptimizationFoam, but now I'm trying to modify it a little, since sometimes the equations diverge.

What I want to do is to use a manual limiter, that limits the value of the velocity in each cell if it raises too much, so I've inserted these lines at the bottom of the solver:

forAll(Ua,cellI)
{
Ua[cellI].component(0)=min(Ua[cellI].component(0), 200);
Ua[cellI].component(1)=min(Ua[cellI].component(1), 200);
Ua[cellI].component(2)=min(Ua[cellI].component(2), 200);
}

forAll(Ua,cellJ)
{
Ua[cellJ].component(0)=max(Ua[cellJ].component(0), -200);
Ua[cellJ].component(1)=max(Ua[cellJ].component(1), -200);
Ua[cellJ].component(2)=max(Ua[cellJ].component(2), -200);
}

I'm expecting that these lines behave like a threshold value for each component of the velocity at each iteration, but I've run a simulation and I discovered that the values of the velocity were bigger than the range [-200:200].

Maybe the lines I've added are wrong?

Any help is really appreciated.
Thanks in advance

Simone

P.s. I'm running in parallel, but I hope this is not a problem for the code I've added.

Please guy, is there someone that can help?

You will need to limit the values on the patches also (all faces on patches)

forAll(U.boundaryField(),patchI)
{
forAll(U.boundaryField()[patchI],faceI)
{
U.boundaryField()[patchI][faceI].component(0)=some value;
}

}

Also your solver might adjust U values not only after solving momentum equation. So make sure that your are limiting after each calculation step of U

Thank you Omkar! The problem was exactly on the patches, since I had forgotten to loop on them. By adding your lines now it seems to work perfectly.

hi Simone
I think limiting velocity can also resolve my problem.
Could you send me your modified solver?
Thanks.

where should i add them exactly?

can use velocity limiters only on a patch not entire the domain?

hi Omkar
Could you send me the code with added expressions for rhoPimpleFoam?

My code consists of combination of above two codes.
Like I said, it did not work for me so I erased that code.
The codes in this forum clearly explain how to limit velocity in the domain and the patches

Hi immortality!
With respect to the adjointShapeOptimizationFoam solver, you should put the " two" limiter just above the lines

Quote:

// Explicitly relax pressure for adjoint momentum corrector
pa.relax();

// Adjoint momentum corrector
Ua -= rAUa*fvc::grad(pa);
Ua.correctBoundaryConditions();

into the predictor-corrector loop. At least, I did in this way!

If you want to "limit" only the patches you should insert only the lines that doubtsincfd suggested.

If, instead, you asked to limit only one specific patch you can use something like this:

Quote:

word patchName = "NAME_OF_THE_PATCH";
label patchID = mesh.boundary().findPatchID(patchName2);

forAll(U.boundaryField()[patchID],faceI)
{
U.boundaryField()[patchID][faceI].component(0)=some value;
}

Hope this works

Simone

thanks.where the codes should be added in rhoPimpleFoam?
rhoPimpleFoam.C is this:

Code:

#include "fvCFD.H"

#include "basicPsiThermo.H"

#include "turbulenceModel.H"

#include "bound.H"

#include "pimpleControl.H"



// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



int main(int argc, char *argv[])

{

    #include "setRootCase.H"

    #include "createTime.H"

    #include "createMesh.H"



    pimpleControl pimple(mesh);



    #include "createFields.H"

    #include "initContinuityErrs.H"



    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //



    Info<< "\nStarting time loop\n" << endl;



    while (runTime.run())

    {

        #include "readTimeControls.H"

        #include "compressibleCourantNo.H"

        #include "setDeltaT.H"



        runTime++;



        Info<< "Time = " << runTime.timeName() << nl << endl;



        #include "rhoEqn.H"



        // --- Pressure-velocity PIMPLE corrector loop

        while (pimple.loop())

        {

            #include "UEqn.H"

            #include "hEqn.H"



            // --- Pressure corrector loop

            while (pimple.correct())

            {

                #include "pEqn.H"

            }



            if (pimple.turbCorr())

            {

                turbulence->correct();

            }

        }



        runTime.write();



        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"

            << "  ClockTime = " << runTime.elapsedClockTime() << " s"

            << nl << endl;

    }



    Info<< "End\n" << endl;



    return 0;

}





// ************************************************************************* //

where UEqn.H is:

Code:

// Solve the Momentum equation



tmp<fvVectorMatrix> UEqn

(

    fvm::ddt(rho, U)

  + fvm::div(phi, U)

  + turbulence->divDevRhoReff(U)

);



UEqn().relax();



volScalarField rAU(1.0/UEqn().A());



if (pimple.momentumPredictor())

{

    solve(UEqn() == -fvc::grad(p));

    K = 0.5*magSqr(U);

}

hEqn.H:

Code:

{

    fvScalarMatrix hEqn

    (

        fvm::ddt(rho, h)

      + fvm::div(phi, h)

      - fvm::laplacian(turbulence->alphaEff(), h)

     ==

        dpdt

      - (fvc::ddt(rho, K) + fvc::div(phi, K))

    );



    hEqn.relax();

    hEqn.solve();



    thermo.correct();

}

pEqn.H:

Code:

rho = thermo.rho();

rho = max(rho, rhoMin);

rho = min(rho, rhoMax);

rho.relax();



U = rAU*UEqn().H();



if (pimple.nCorrPISO() <= 1)

{

    UEqn.clear();

}



if (pimple.transonic())

{

    surfaceScalarField phid

    (

        "phid",

        fvc::interpolate(psi)

       *(

            (fvc::interpolate(U) & mesh.Sf())

          + fvc::ddtPhiCorr(rAU, rho, U, phi)

        )

    );



    while (pimple.correctNonOrthogonal())

    {

        fvScalarMatrix pEqn

        (

            fvm::ddt(psi, p)

          + fvm::div(phid, p)

          - fvm::laplacian(rho*rAU, p)

        );



        pEqn.solve(mesh.solver(p.select(pimple.finalInnerIter())));



        if (pimple.finalNonOrthogonalIter())

        {

            phi == pEqn.flux();

        }

    }

}

else

{

    phi =

        fvc::interpolate(rho)*

        (

            (fvc::interpolate(U) & mesh.Sf())

          + fvc::ddtPhiCorr(rAU, rho, U, phi)

        );



    while (pimple.correctNonOrthogonal())

    {

        // Pressure corrector

        fvScalarMatrix pEqn

        (

            fvm::ddt(psi, p)

          + fvc::div(phi)

          - fvm::laplacian(rho*rAU, p)

        );



        pEqn.solve(mesh.solver(p.select(pimple.finalInnerIter())));



        if (pimple.finalNonOrthogonalIter())

        {

            phi += pEqn.flux();

        }

    }

}



#include "rhoEqn.H"

#include "compressibleContinuityErrs.H"



// Explicitly relax pressure for momentum corrector

p.relax();



// Recalculate density from the relaxed pressure

rho = thermo.rho();

rho = max(rho, rhoMin);

rho = min(rho, rhoMax);

rho.relax();

Info<< "rho max/min : " << max(rho).value()

    << " " << min(rho).value() << endl;



U -= rAU*fvc::grad(p);

U.correctBoundaryConditions();

K = 0.5*magSqr(U);



dpdt = fvc::ddt(p);

In my opinion after

Code:

if (pimple.turbCorr())

{

    turbulence->correct();

}

should be fine.

thank you dear Simone for your help
so I added it.is it correct?why you have wrote patchName2 in findPatchID?
I put U[cellI] instead of Ua[cellI] due to use in rhoPimpleFoam does it have any problem?
I want not to let U becomes higher than sound speed(flow should be subsonic)
will it be true that I write sqrt(1.4*287.14*T[cellI]) instead of 500 I have put now?
I want to be certain to compile the modified solver.
thanks again.

Code:

word patchName = "left";

         label patchID = mesh.boundary().findPatchID(patchName);

         forAll(U.boundaryField()[patchID],faceI)

           {

               U.boundaryField()[patchID][faceI].component(0)=min(U[cellI].component(0), 500);

           }

I used it for the patch.but velocity in cells near the inflow boundary are supersonic.
where I add the expressions to limit velocity on top of domain?
and what do you mean from cellI and cellJ in this expressions:
forAll(Ua,cellI)
{
Ua[cellI].component(0)=min(Ua[cellI].component(0), 200);
Ua[cellI].component(1)=min(Ua[cellI].component(1), 200);
Ua[cellI].component(2)=min(Ua[cellI].component(2), 200);
}

forAll(Ua,cellJ)
{
Ua[cellJ].component(0)=max(Ua[cellJ].component(0), -200);
Ua[cellJ].component(1)=max(Ua[cellJ].component(1), -200);
Ua[cellJ].component(2)=max(Ua[cellJ].component(2), -200);
}

You have to put those line before the ones to limit the boundary. cellI and cellJ are two (unuseful) different counters. You can use the same for both cycles.

thank you dear Simone again
is this correct now?:

Code:

forAll(U,cellI)

           {

            U[cellI].component(0)=min(U[cellI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30);

           }

           forAll(U,cellJ)

           {

            U[cellJ].component(1)=max(U[cellI].component(1),-150);

           }

         word patchName = "left";

         label patchID = mesh.boundary().findPatchID(patchName);

         forAll(U.boundaryField()[patchID],faceI)

           {

               U.boundaryField()[patchID][faceI].component(0)=min(U.boundaryField()[patchID][faceI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30);

               U.boundaryField()[patchID][faceI].component(1)=max(U.boundaryField()[patchID][faceI].component(1),-150);

           }

another question! could we do both loops into single one by for instance I counter?
thanks.

when compiled it this error occurred:

Code:

ehsan@Ehsan-com:~/Desktop/rhoPimpleFoamLimited$ wmakeMaking dependency list for source file rhoPimpleFoamLimited.C

SOURCE=rhoPimpleFoamLimited.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam211/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam211/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam211/src/finiteVolume/cfdTools -I/opt/openfoam211/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam211/src/OpenFOAM/lnInclude -I/opt/openfoam211/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/rhoPimpleFoamLimited.o

rhoPimpleFoamLimited.C: In function ‘int main(int, char**)’:

rhoPimpleFoamLimited.C:90:79: error: ‘Foam::T’ does not have class type

rhoPimpleFoamLimited.C:90:96: error: ‘patchID’ was not declared in this scope

rhoPimpleFoamLimited.C:90:105: error: ‘faceI’ was not declared in this scope

rhoPimpleFoamLimited.C:94:41: error: name lookup of ‘cellI’ changed for ISO ‘for’ scoping [-fpermissive]

rhoPimpleFoamLimited.C:94:41: note: (if you use ‘-fpermissive’ G++ will accept your code)

rhoPimpleFoamLimited.C:100:132: error: ‘Foam::T’ does not have class type

make: *** [Make/linux64GccDPOpt/rhoPimpleFoamLimited.o] Error 1

whats error in T?

Actually I don't know if OF will allow you such a statement:

Code:

U[cellI].component(0)=

min(U[cellI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30);

since you are looping inside the domain for the component of U you can't assign its value with respect to the value of the temperature on the boundary!

I don't know if you can use something like this:

Code:

U[cellI].component(0)=

min(U[cellI].component(0), sqrt(1.4*287.14*T.[cellI])-30);

You could try with the line above if I understand well your intention, i.e. you want to threshold the value of the velocity with respect to the local value of the Mach number.

Hope this help.

thank you.
yes Simone you understood well.
I modified it as so:

Code:

forAll(U,cellI)

           {

            U[cellI].component(0)=min(U[cellI].component(0), sqrt(1.4*287.14*T.[cellI])-30);

           }

           forAll(U,cellJ)

           {

            U[cellJ].component(1)=max(U[cellI].component(1),-150);

           }

         word patchName = "left";

         label patchID = mesh.boundary().findPatchID(patchName);

         forAll(U.boundaryField()[patchID],faceI)

           {

               U.boundaryField()[patchID][faceI].component(0)=min(U.boundaryField()[patchID][faceI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30);

               U.boundaryField()[patchID][faceI].component(1)=max(U.boundaryField()[patchID][faceI].component(1),-150);

           }

but this error is shown:

Code:

ehsan@Ehsan-com:~/Desktop/rhoPimpleFoamLimited$ wmakeMaking dependency list for source file rhoPimpleFoamLimited.C

SOURCE=rhoPimpleFoamLimited.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam211/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam211/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam211/src/finiteVolume/cfdTools -I/opt/openfoam211/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam211/src/OpenFOAM/lnInclude -I/opt/openfoam211/src/OSspecific/POSIX/lnInclude   -fPIC -c $SOURCE -o Make/linux64GccDPOpt/rhoPimpleFoamLimited.o

rhoPimpleFoamLimited.C: In function ‘int main(int, char**)’:

rhoPimpleFoamLimited.C:90:79: error: ‘Foam::T’ does not have class type

rhoPimpleFoamLimited.C:90:96: error: ‘patchID’ was not declared in this scope

rhoPimpleFoamLimited.C:90:105: error: ‘faceI’ was not declared in this scope

rhoPimpleFoamLimited.C:94:41: error: name lookup of ‘cellI’ changed for ISO ‘for’ scoping [-fpermissive]

rhoPimpleFoamLimited.C:94:41: note: (if you use ‘-fpermissive’ G++ will accept your code)

rhoPimpleFoamLimited.C:100:132: error: ‘Foam::T’ does not have class type

make: *** [Make/linux64GccDPOpt/rhoPimpleFoamLimited.o] Error 1

it's

Code:

T[cellI]

not

Code:

T.[cellI]