[saicharan662000@gmail.com]

Hello guys,
when I ran the test cases of dam break and sloshing tank problem sloshing tank has 2 different boundary conditions for Pressure(i. e P_rgh ,P). BUT DAM BREAK has only one boundary condition for P. Can anyone tell me why this is done? I know both are made for different solvers but why two boundary conditions for P in sloshing tank?


Thanks in advance.

[orss_st]

i have the same problem

[orss_st]

i have the same problem

[LuckyTran]

p doesn't have boundary conditions, they're all type calculated.

[saicharan662000@gmail.com]

Hello luckyTran,
If p are all type calculated then why dam break problem had only p_rgh in 0 folder. And sloshing tank has p,p_rgh in zero folder ?
Thanks and regards

[LuckyTran]

Because potentialFreeSurfaceFoam needs a way to set the reference pressure consistently for both the total pressure and the hydraulic pressure. In interFoam, that job is fulfilled by rho.

[saicharan662000@gmail.com]

Hello Lucky,
Can you please explain it in more detail.

Thanks in advance

[LuckyTran]

All the details you can ever hope for are in createFields.H and pEqn.H

Info<< "Reading field p (kinematic)\n" << endl;
volScalarField p
(
    IOobject
    (
        "p",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

Info<< "Reading field U\n" << endl;
volVectorField U
(
    IOobject
    (
        "U",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

#include "createPhi.H"

singlePhaseTransportModel laminarTransport(U, phi);

autoPtr<incompressible::momentumTransportModel> turbulence
(
    incompressible::momentumTransportModel::New(U, phi, laminarTransport)
);

#include "readGravitationalAcceleration.H"

Info<< "Creating field zeta\n" << endl;
volVectorField zeta
(
    IOobject
    (
        "zeta",
        runTime.timeName(),
        mesh,
        IOobject::READ_IF_PRESENT,
        IOobject::AUTO_WRITE
    ),
    mesh,
    dimensionedVector(dimLength, Zero)
);

Info<< "Creating field p_gh\n" << endl;
volScalarField p_gh
(
    IOobject
    (
        "p_gh",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

// Force p_gh to be consistent with p
// Height is made relative to field 'refLevel'
p_gh =  p - (g & mesh.C());

pressureReference pressureReference(p_gh, pimple.dict());

mesh.setFluxRequired(p_gh.name());

#include "createMRF.H"
#include "createFvModels.H"
#include "createFvConstraints.H"

Specifically the two lines of importance are:

p_gh =  p - (g & mesh.C());


 pressureReference pressureReference(p_gh, pimple.dict());

The only other call to p is in the final line of pEqn.H where it is recalculated from elevation and hydraulic pressure.

p = p_gh + (g & mesh.C());

p never gets used in any equation and therefore does not need boundary conditions. That's why all its types are calculated in the tutorial. On the other hand, p_gh does have a solver and therefore needs boundary conditions. At the same time, p_rgh is the dynamic variable in interFoam and there needs boundary conditions.

[saicharan662000@gmail.com]

Hello Lucky,
But we have 'P' in in tutorials of compressibleInterfoam in zero folder . Why do we have it?
Thanks and Regards

[LuckyTran]

And? What's your point? p in compressibleInterFoam also does not have any boundary conditions.

[saicharan662000@gmail.com]

Why do we need to set a special reference to P in compressible interfoam tutorial cases? There is no special reference for p in test cases of interfoam in zero folder.
Thanks and regards.

[LuckyTran]

Because compressibleInterFoam is compressible and uses a non-incompressible thermophysical model. Equations of states are based off of p and T (and not p_gh/p_rgh).


Please don't ask why there is a T in compressibleInterFoam and not in interFoam. God forbid people develop solvers that do more things. Just stick to interFoam if you're that lost.

[Saicharan]

I am not that blind to ask why T is in compressible interfoam. I know compressible interfoam solver solves for energy equation. Anyway thanks for help lucky tran

[LuckyTran]

Let me make this even clearer since I don't think you actually get it yet. Even if there was no energy equation (just like there is no equation for p) you would still need to supply a T field simply because the thermophsysical model you are using asks for one (in compressibleInterFoam anyway). Energy equation means you need to provide boundary conditions for the variable, yes. But there are other reasons for providing a field

[Saicharan]

Hello lucky,
Now I get it.
Thank you for patiently explaining things for me.