[And901]

Hi everybody,

i'm new to OpenFOAM and i'm trying to solve the incompressible linearized Navier-Stokes equations.
Called U_zero the equilibrium solution, i tried to modify the icoFoam.C code as follow:

fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi_zero, U)
+ fvm::div(phi,U_zero)
- fvm::laplacian(nu, U)
);

solve(UEqn == -fvc::grad(p));

where phi_zero is defined as

surfaceScalarField phi_zero
(
IOobject
(
"phi_zero",
runTime.timeName(),
mesh,
IOobject::READ_IF_PRESENT,
IOobject::AUTO_WRITE
),
linearInterpolate(U_zero) & mesh.Sf()
);

I also defined U_zero in createFields.H as:

Info<< "Reading field U_zero\n" << endl;
volVectorField U_zero
(
IOobject
(
"U_zero",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh,
Foam::vector(1,0,0)
);

I compiled the code without errors but when i try to run a case (cavity for example) the following error message appears:

--> FOAM FATAL ERROR:

valueInternalCoeffs cannot be called for a calculatedFvPatchField
on patch movingWall of field U_zero in file "/home/andrea/Desktop/tesi/openfoam/tutorials/incompressible/icoFoam/cavityLinearized/0/U_zero"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::valueInternalCoeffs( const tmp<scalarField>&) const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 144.

FOAM exiting

I know that i should first calculate U_zero as a stationary solution and then solve the linearized NS equation in a neighbourhood of it . In my case U_zero is just a constant vector, but i'm just trying to run the code without errors to see what happens.

Thanks for your help.

Regards, Andrea

[alexeym]

Hi,

if I got your problem right, you need to set boundary conditions for U_zero. Now you create the field with:

volVectorField U_zero
(
IOobject
(
"U_zero",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh,
Foam::vector(1,0,0)
);

but you can add

volVectorField U_zero
(
IOobject
(
"U_zero",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh,
Foam::vector(1,0,0),
U.boundaryField().types()
);

so U_zero will have the same BCs as U. In fact you can change U.boundaryField().types() to any BC you'd like U_zero to have.

[ngj]

Good morning,

You must use fvc:: on the U_zero term, as it should not be a part of your matrix, but rather the source term.

Kind regards,

Niels

[And901]

Hi Alexey,

thanks for your reply, i added the new line for BC as you said but a new error appears:

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[U[0 1 -2 0 0 0 0] ] + [U[0 0 -1 0 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /opt/openfoam211/src/finiteVolume/lnInclude/fvMatrix.C at line 1316.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2
at ??:?
#3
at ??:?
#4
at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6
at ??:?
Aborted (core dumped)

It seems that U dimensions are not correct but U file in /0 directory has dimensions:

dimensions [0 1 -1 0 0 0 0];

[And901]

Hi Niels,

sorry, maybe my question is stupid but why did you say that U_zero should be a source term? In linearized Navier-Stokes equations U_zero is always coupled with U so how can i write it as a source term?

Best Regards,

Andrea.

[alexeym]

Hi,

Originally Posted by And901

--> FOAM FATAL ERROR:
incompatible dimensions for operation
[U[0 1 -2 0 0 0 0] ] + [U[0 0 -1 0 0 0 0] ]

...

It seems that U dimensions are not correct but U file in /0 directory has dimensions:

dimensions [0 1 -1 0 0 0 0];

I think it's U_zero, not U, that gives you dimension problem; it seems U_zero is dimless (so dimensions of div(phi, U_zero) is 1/s.

Maybe dimensions of U_zero that you've put in 0 folder are overwritten by Foam::vector(1,0,0), try using dimensionedVector("U_zero", dimVelocity, vector(1, 0, 0)).

About comment by Niels, in your div(phi, U_zero) there's no U, so you have to use div method from fvc namespace. And it will be treated as a source term.

[And901]

Hi Alexey,

thanks a lot for your advices, i solved the problem.
Sorry if i ask you one more question; i would like to read U_zero from a file following these steps:

1) run cavity case with icoFoam;
2) extract U field at each time step typing "foamCalc components U";
3) Set U_zero = U (so i need to read U_zero from a file);
4)Solve linearized Navier-Stokes equations around U_zero;

I have done step 1 and 2 but i don't know how to do step 3.

I would appreciate your help.

Best regards,

Andrea

[alexeym]

Hi,

right now the only solution that I can think of is to use another variant of IObject constructor to create U_zero vector field:

http://foam.sourceforge.net/docs/cpp...52f901319147b6

IOobject 	
( 	
    const fileName& path,
    const objectRegistry& registry,
    readOption r = NO_READ,
    writeOption w = NO_WRITE,
    bool registerObject = true 
)

with this constructor you can directly specify path of the object i.e. path to the simulation results you've obtained with icoFoam.

[And901]

Thanks Alexey,

problem solved.

Best Regards,

Andrea

[kkpal]

Thanks to this thread, my icoLinearFoam is also compiled.
Now I am trying to construct the operation matrix M, for , and analysis the eigenvalues of M to see if the base flow is stable or not.

[kebsiali]

Hello
I think you either have a missing file or a miss-spell in the name of the file or inside U_zero

[kkpal]

Hi, ali,
Yes, I made a mistake and I've corrected it. I have successfully compiled and run it.
Now I would like to analyse the global stability of the flow by the eigenvectors (growth rate) of the matrix M by constructing , in which U is the velocity velocity vector. Any idea how to achieve this?