[rr3245]

Hi all,

I am running foam-extend 4.0 and trying to use the FSI toolkit, however I get the following error message when running the 3 tutorials in fsiFoam:

Time = 0.1, iteration: 1
Current fsi under-relaxation factor: 0.4
Creating accumulated fluid interface displacement
Maximal accumulated displacement of interface points: 0
GAMG:  Solving for cellMotionUx, Initial residual = 0, Final residual = 0, No Iterations 1
GAMG:  Solving for cellMotionUy, Initial residual = 0, Final residual = 0, No Iterations 1
GAMG:  Solving for cellMotionUz, Initial residual = 0, Final residual = 0, No Iterations 1
Evolving fluid solver: consistentIcoFluid
Courant Number mean: 2.74517e-18 max: 0.425797 velocity magnitude: 0.0464238
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 3.27614e-07, No Iterations 4
DILUPBiCG:  Solving for Uy, Initial residual = 0.988361, Final residual = 8.95334e-07, No Iterations 4
DILUPBiCG:  Solving for Uz, Initial residual = 0.985989, Final residual = 9.63029e-07, No Iterations 4
GAMG:  Solving for p, Initial residual = 1, Final residual = 7.79802e-07, No Iterations 19
GAMG:  Solving for p, Initial residual = 2.59508e-05, Final residual = 3.63815e-07, No Iterations 2


--> FOAM FATAL ERROR: 
flux requested but p not specified in the fluxRequired sub-dictionary of fvSchemes.

    From function fvMatrix<Type>::flux()
    in file lnInclude/fvMatrix.C at line 1046.

FOAM aborting

The following thread addresses some of these issues, where it is suggested that fluxRequired should be disabled:

https://www.cfd-online.com/Forums/openfoam-solving/185685-fsifoam-4-0-can-not-run-tutorials.html

The source code has been updated since that thread, incorporating some of the 'fixes'. I have been trying to update a createFields.H file as suggested in the above thread:

"You have to integrate that line into your createFields.H and recompile your solver."

mesh.schemesDict().setFluxRequired(p.name());

However, the createFields.H appears to have been blended into icoFluid.C, consistentIcoFluid.C, and pisoFluid.C. For example, below is an excerpt from pisoFluid.C :

pisoFluid::pisoFluid(const fvMesh& mesh)
:
    fluidSolver(this->typeName, mesh),
    U_
    (
        IOobject
        (
            "U",
            runTime().timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        mesh
    ),
    p_
    (

Therefore the fix suggested above isn't valid, and I don't know what to try next. Has anybody been able to run tutorials for the fsiFoam recently?

Regards, RH.

[alia]

Hi!

you just need to add the following line to your fluid solver at the begining of evolve() function :

mesh.schemesDict().setFluxRequired(p_.name());

Cheers

[rr3245]

Originally Posted by alia

Hi!

you just need to add the following line to your fluid solver at the begining of evolve() function :

mesh.schemesDict().setFluxRequired(p_.name());

Cheers

My solver seems to break on consistentIcoFluid, so I have tried adding the line above to consistentIcoFluid.C and consistentIcoFluid.H. Both those files have an evolve() function, but I am not sure where to include the line.

Could you please identify which files need to be edited, and where?

Thanks,
RH.

[alia]

Originally Posted by rr3245

My solver seems to break on consistentIcoFluid, so I have tried adding the line above to consistentIcoFluid.C and consistentIcoFluid.H. Both those files have an evolve() function, but I am not sure where to include the line.

Could you please identify which files need to be edited, and where?

Thanks,
RH.

.H files of classes are just for declarations. you definitely should add that line in the .C file. you need to add the line inside the scope of evolve() function after the line

    const fvMesh& mesh = fluidSolver::mesh();

cheers

[rr3245]

Originally Posted by alia

.H files of classes are just for declarations. you definitely should add that line in the .C file. you need to add the line inside the scope of evolve() function after the line

    const fvMesh& mesh = fluidSolver::mesh();

cheers

That's pretty much what I've been trying, but with no luck. Here is an excerpt from fluidSolidInteraction/fluidSolvers/icoFluid/icoFluid.C:

 void icoFluid::evolve()
{
    Info << "Evolving fluid solver: " << this->type() << endl;

    const fvMesh& mesh = fluidSolver::mesh();

//EDIT START
mesh.schemesDict().setFluxRequired(p_.name());
//EDIT END

    int nCorr(readInt(fluidProperties().lookup("nCorrectors")));

    int nNonOrthCorr =
        readInt(fluidProperties().lookup("nNonOrthogonalCorrectors"));

I have downloaded the fsi package once again and made the above changes to my icoFluid.C, consistentIcoFluid.C, and pisoFluid.C files. I get an error when compilling with './Allwmake':

 
lnInclude/icoFluid.H: In member function ‘virtual void Foam::fluidSolvers::consistentIcoFluid::evolve()’:
lnInclude/icoFluid.H:66:24: error: ‘Foam::volScalarField Foam::fluidSolvers::icoFluid::p_’ is private
         volScalarField p_;
                        ^
fluidSolvers/consistentIcoFluid/consistentIcoFluid.C:149:36: error: within this context
 mesh.schemesDict().setFluxRequired(p_.name());

[alia]

in that case you need to use the access function p():

 mesh.schemesDict().setFluxRequired(p().name());

[rr3245]

Originally Posted by alia

in that case you need to use the access function p():

 mesh.schemesDict().setFluxRequired(p().name());

That seems to have worked. I will update this once I test it properly. Thanks for the guidance. RH.

[rr3245]

Thanks for your help alia. For completeness, this is what I did:

I inserted one line of code into the evolve() function for each fluidSolver (i.e. consistentIcoFluid.C, icoFluid.C, pisoFluid.C)

Insert

mesh.schemesDict().setFluxRequired(p().name());

after

const fvMesh& mesh = fluidSolver::mesh();

...into:
src/fluidSolidInteraction/fluidSolvers/consistentIcoFluid/consistentIcoFluid.C
src/fluidSolidInteraction/fluidSolvers/icoFluid/icoFluid.C
src/fluidSolidInteraction/fluidSolvers/pisoFluid/pisoFluid.C

Then I ran ./Allwmake to update and the beam tutorial ran fine. RH.