[Mahmoud_aboukhedr]

Hello All friends,

As you know with new updates for OF versions not everything work smoothly.

I'm working constantly with interfoam and lots of updates in micro flow applications. Anyway All my updates in the code and test case set-up was done in 2.2x ...

Recently I updated all my codes and test cases to 2.3x, but I kept the old BC files for the test cases as following

p_rgh

   inlet_liquid
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    inlet_gas
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }

    wall_1
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

U

inlet_liquid
    {
        type            fixedValue;
        value           uniform (0.106 0 0);
    }

    inlet_gas
    {
        type            fixedValue;
        value           uniform (0 0 -0.344);
    }

    outlet
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

    wall_1
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

For OF22x The BC works fine and everything is good,
But for OF23x it gives me error

updateCoeffs(const scalarField& snGradp) MUST be called before updateCoeffs() or evaluate() to set the boundary gradient.

From function fixedFluxPressureFvPatchScalarField::updateCoeffs( )
in file fields/fvPatchFields/derived/fixedFluxPressure/fixedFluxPressureFvPatchScalarField.C at line 151.

So did anyone had the same problem with the new versions,
maybe its a very easy problem, that I need to change something with the schemes

Any help from the expatriates will be great

Mahmoud

[vatavuk]

Hi Mahmoud,
Recently I adapted the spillway tutorial (https://www.hpc.ntnu.no/display/hpc/OpenFOAM+-+Spillway+Tutorial), to version 2.3. I noticed that in 2.3 the boundary condition for p_rgh at inlet, outled and walls was replaced by zeroGradient as is done in the weirOveflow tutorial.
Another problem that I noticed is that it is very difficult to get convergence using the fixed value condition for U, at the water inlet, I had to replace it with the variableHeightFlowRateInletVelocity. I suppose something similar may happen in your case.
Best Regards,
Paulo

[Mahmoud_aboukhedr]

Dear Paulo,

Thanks for the update,
I think the fixedFluxPressure tretment method had ben changed from 2.2x to 2.3x .. am still not sure how to fix it to be honest .

[wyldckat]

Greetings to all!

pimpleFoam has the following change in 2.3.x: https://github.com/OpenFOAM/OpenFOAM...46e787db50c95a

The code for "interFoam/pEqn.H" also has the following:

    // Update the fixedFluxPressure BCs to ensure flux consistency
    setSnGrad<fixedFluxPressureFvPatchScalarField>
    (
        p_rgh.boundaryField(),
        (
            phiHbyA.boundaryField()
          - fvOptions.relative(mesh.Sf().boundaryField() & U.boundaryField())
        )/(mesh.magSf().boundaryField()*rAUf.boundaryField())
    );

The reason is in this commit on the OpenFOAM-history repository: https://github.com/OpenCFD/OpenFOAM-...78c39cb40e82c6
And I quote:

fixedFluxPressure BC: the snGrad is now pushed into the BC from pEqn.H rather than being evaluated in the BC

This explains the issue. As for the solution:

1. I suggest you study the OpenFOAM tutorials and this commit in particular for details.
2. Or if you cannot figure out the solution, I need an example case to study .

Best regards,
Bruno

[vijaychauhan]

Originally Posted by wyldckat

Greetings to all!

pimpleFoam has the following change in 2.3.x: https://github.com/OpenFOAM/OpenFOAM...46e787db50c95a

The code for "interFoam/pEqn.H" also has the following:

    // Update the fixedFluxPressure BCs to ensure flux consistency
    setSnGrad<fixedFluxPressureFvPatchScalarField>
    (
        p_rgh.boundaryField(),
        (
            phiHbyA.boundaryField()
          - fvOptions.relative(mesh.Sf().boundaryField() & U.boundaryField())
        )/(mesh.magSf().boundaryField()*rAUf.boundaryField())
    );

The reason is in this commit on the OpenFOAM-history repository: https://github.com/OpenCFD/OpenFOAM-...78c39cb40e82c6
And I quote:
This explains the issue. As for the solution:

1. I suggest you study the OpenFOAM tutorials and this commit in particular for details.
2. Or if you cannot figure out the solution, I need an example case to study .

Best regards,
Bruno

Dear All,
I hope I can help a bit. I found a similar problem running lagrangian sprayFoam solver which I have modified little bit. What I observed was that, as mentioned by Bruno, setSnGrad<fixedFluxPressureFvPatchScalarField> is missing in some solver pEqn.H. I simply copied it from other solver pEqn.H where it exists and carefully changes variable names according to your solver. It runs well for me. Then wmake. Also dont forget to #include "fixedFluxPressureFvPatchScalarField.H" in solver file. Hope it works.