[Nazanin]

I send for you

[Sasy]

Originally Posted by adambarfi

mhmm, I think there are problems with p BCs.
the userGuide says:

I think such same BCs for p and p_rgh is wrong, let the solver calculate the pressure based upon potential function. try "calculated" type for p BCs.

Also, I can't understand these conditions you used for p_rgh:

        type            buoyantPressure;
        gradient        uniform 0;
        value           uniform 0;

try this one:

        type            buoyantPressure;
        rho             rhok;
        value           uniform 0;

see the buoyantBoussinesqPimpleFoam and buoyantBoussinesqSimpleFoam solvers. they have tips that may help you.

Hi
I try this BCs,but the problem is still.
first I try this boundary condition:
type buoyantPressure;
value uniform 0;
and This
type zeroGradient;
but no answer...
NOTE:my case is 1D and I think should use this BCs
Regards,

[lramutti]

Hey guys, I am ran into something similar for a conjugate heat transfer problem. In my case it says:

--> FOAM FATAL ERROR:

gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch leftWall of field h in file "/home/meisu/OpenFOAM/meisu-2.2.1/run/Research/ConjugateHeatTransfer/RayleighBenard/caseFourDomeFourWalls/0/leftWall/h"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 199.

The question I have is what h file is OpenFOAM referring to? I only don't have any h scripts.

Thanks!

[lramutti]

Hey guys,

I solved the problem. I did not spell correctly the name of my boundary condition. It should have been labeled as leftWall instead of leftwall. Silly mistakes can consume a lot of time .

[zhouzhipeng77]

Hi Mostafa ,
I have some questions with the following code in createFields.H . ANd I look forward to your help .
1. regarding this code "p_rgh + rhok*gh" , rhok is calculated from temperature T , so it is different in different position , why can we use this formula for uniform rho ?

volScalarField p
(
IOobject
(
"p",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
p_rgh + rhok*gh
);

2. about the setRefCell function , what is its function with p and a_rgh , or can you explain the process of this function ?

label pRefCell = 0;
scalar pRefValue = 0.0;
setRefCell
(
p,
p_rgh,
mesh.solutionDict().subDict("PIMPLE"),
pRefCell,
pRefValue
);

3. with the following code , how dose it process ?

if (p_rgh.needReference())
{
p += dimensionedScalar
(
"p",
p.dimensions(),
pRefValue - getRefCellValue(p, pRefCell)
);
}

Thanks
Zhipeng

[adambarfi]

Hi Zhipeng and welcome

1-
remember the momentum equation and the Boussinesq approximation for naural convection:




for the case of constant density and gravity, the term can be written as grad(), where r is the position vector. then is the hydrostatic pressure, and it's convenient- and for numerical solution more efficient- to define as the head and use it in place of the pressure.
In variable density flows, one can split the term into two parts: .

for more information you can refer to Ferziger's textbook (computational methods for fluid dynamics).

2-3
The solver needs to know what and where the reference pressure is. according to the explanation in 1 and below quote, I think you can get the answer of your questions.

in OpenFOAM pRef is used only if your boundary conditions are set in such a way not to prescribe any reference for the pressure.

So, for example, if you open a duct open to the athmosphere at the outlet, and you have the velocity specified at the inlet, you should specify p equal to zero at the outlet (in incompressible flows, if you specify 1 it doesn't make any difference, you simply translate the values of the pressure in your whole domain of the same difference).

If you have a simulation where p has only Neumann (zeroGradient) conditions, the pRef value will be used, setting p = pRefVal in the cell of index pRefCell.

The values of pRefCell and pRefValue are always specified in the PISO/SIMPLE/PIMPLE subdictionary in fvSolution.

to find out how the pEqn.H works you can see the below link:
http://foam.sourceforge.net/docs/cpp/a02937.html

Bests,
Mostafa

[zhouzhipeng77]

Hi , Mostafa ,
Thank you for your help , and I have understand the question , but I can understand the following code in pEqn.H , though I have read the link you telll me .

{
volScalarField rAU("rAU", 1.0/UEqn.A());
surfaceScalarField rAUf("(1|A(U))", fvc::interpolate(rAU));

U = rAU*UEqn.H();

phi = (fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rAU, U, phi);

surfaceScalarField buoyancyPhi(rAUf*ghf*fvc::snGrad(rhok)*mesh.magSf( ));
phi -= buoyancyPhi;

while (pimple.correctNonOrthogonal())
{
fvScalarMatrix p_rghEqn
(
fvm::laplacian(rAUf, p_rgh) == fvc::div(phi)
);

p_rghEqn.setReference(pRefCell, getRefCellValue(p_rgh, pRefCell));

p_rghEqn.solve(mesh.solver(p_rgh.select(pimple.fin alInnerIter())));

if (pimple.finalNonOrthogonalIter())
{
// Calculate the conservative fluxes
phi -= p_rghEqn.flux();

// Explicitly relax pressure for momentum corrector
p_rgh.relax();

// Correct the momentum source with the pressure gradient flux
// calculated from the relaxed pressure
U -= rAU*fvc::reconstruct((buoyancyPhi + p_rghEqn.flux())/rAUf);
U.correctBoundaryConditions();
}
}

Can anybody help me to explain this , or introduce me some papers I should read ?
Thanks
Zhipeng

[adambarfi]

the explanation of this algorithm here for me is not very easy!! so I attach you a note about the SIMPLE algorithm for pressure-velocity coupling and 4 links about the PISO and SIMPLE algorithm and the implementation of them with OF:

https://www.dropbox.com/s/lplecnozku...MPLEslides.pdf

The_SIMPLE_algorithm_in_OpenFOAM

The_PISO_algorithm_in_OpenFOAM

BuoyantBoussinesqPisoFoam

SIMPLE_algorithm

hope they can help you

[Lisandro Maders]

Hello,

I have the same error posted before:

--> FOAM FATAL ERROR: 

    gradientInternalCoeffs cannot be called for a calculatedFvPatchField
    on patch OUTLET of field h in file "/home/lisandro/OpenFOAM/lisandro-2.3.0/run/tutorials/combustion/reactingFoam/ras/counterFlowFlame2D/0/h"
    You are probably trying to solve for a field with a default boundary condition.

    From function calculatedFvPatchField<Type>::gradientInternalCoeffs() const
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 199.

FOAM exiting

The thing is, I don't have this file in my 0 folder, I have the T file instead as well as species files. I am running the counterFlowFlame2D tutorial but I changed the mesh..

Why is it looking for the h file?



Best,

Lisandro

[Lisandro Maders]

Just as a matter of fact, I solved the issue above by changing the BC type of N2 (inert specie) in the Outlet patch. It was calculated and I put zeroGradient and I got no errors anymore.

Lisandro