[maysmech]

Hello
I need varying BC for interstitialInletVelocity which can be found in DPMFoam/Goldschemidt. Using table for fixed value:

    
bottom
{
    type uniformFixedValue;
    uniformValue table
    (
        (0 (0 0 1))
        (0.001 (0 0 2))
        (0.002 (0 0 3))
        (0.003 (0 0 4))
    );
    }

the run starts without error. But for interstitialInletVelocity"
The default is:

    bottom
    {
        type            interstitialInletVelocity;
        inletVelocity   uniform (0 0 1);
        value           uniform (0 0 1);
        phi             phi.air;
        alpha           alpha.air;
    }

trying to time varying it by:

    bottomSB
    {
        type            interstitialInletVelocity;
        inletVelocity   uniformFixedValue;
    uniformValue table
(
        (0 (0 0 1))
        (0.001 (0 0 2))
        (0.002 (0 0 3))
        (0.003 (0 0 4))
);

        value           table
(
        (0 (0 0 1))
        (0.001 (0 0 2))
        (0.002 (0 0 3))
        (0.003 (0 0 4))
); 
        phi             phi.air;
        alpha           alpha.air;
    }

gives this error:

--> FOAM FATAL IO ERROR: 
expected keyword 'uniform' or 'nonuniform', found table

file: /home/user/OpenFOAM/user-2.3.0/run/tutorials/lagrangian/DPMFoam/test/0/U.air.boundaryField.bottom from line 52 to line 70.

    From function Field<Type>::Field(const word& keyword, const dictionary&, const label)
    in file /home/user/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/Field.C at line 304.

FOAM exiting

Change of second "table" to "nonuniform" also gives error:

--> FOAM FATAL IO ERROR: 
wrong token type - expected Scalar, found on line 64 the punctuation token '('

file: /home/user/OpenFOAM/user-2.3.0/run/tutorials/lagrangian/DPMFoam/test/0/U.air.boundaryField.bottom.value at line 64.

    From function operator>>(Istream&, Scalar&)
    in file lnInclude/Scalar.C at line 93.

FOAM exiting

I checked other changes by "Banana" trick debugging but it doesn't work. This boundary condition is suitable for two phase flows because It consider the inlet porosity so we will sure about fixed value of inlet flow rate. It is not possible to use simple fixed value BC and should use interstitialInletVelocity instead. If anyone know about time varying this BC please share here.
Best,

[wyldckat]

Greetings to all!

@Maysam: Unfortunately I don't have enough time to give the whole solution, but I think I can still give information on why that didn't work and what can be done to fix the problem.

1. "uniformFixedValue" is a special boundary condition, derived from "fixedValue". This is the reason why it's possible to use it to define values based on tables and polynomials and so on: http://www.openfoam.org/version2.1.0...conditions.php - and as explained on that page, this feature is possible thanks to another new feature they added in OpenFOAM 2.1.0, namely the "DataEntry" class.
2. "interstitialInletVelocity" is similar to "fixedValue". Which is why it's not able to handle the time-based tables.
3. The solution is to create a new boundary condition derived from "interstitialInletVelocity", almost the same way that "uniformFixedValue" is derived from "fixedValue". Online you can find the source code folders for these 3 BCs (in OpenFOAM 2.3.x):
   • https://github.com/OpenFOAM/OpenFOAM...sic/fixedValue
   • https://github.com/OpenFOAM/OpenFOAM...formFixedValue
   • https://github.com/OpenFOAM/OpenFOAM...lInletVelocity
4. Instructions on how to create a new BC... there are several online... just Google:
   

   openfoam create new boundary condition

   and you'll find several links.

Best regards,
Bruno

[maysmech]

Thanks Bruno, Do you know what is the difference between "inletVelocity" and "value" in this BC?
fixedValue and uniformFixedValue value need one velocity but this on needs two.

[wyldckat]

Hi Maysam,

Originally Posted by maysmech

Do you know what is the difference between "inletVelocity" and "value" in this BC?

If you learn a bit about C++ and reading OpenFOAM source code, you could easily see the following details:

1. If you look at the file "src/finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity/interstitialInletVelocityFvPatchVectorField.C": https://github.com/OpenFOAM/OpenFOAM...hVectorField.C
2. Then look at this part of the code in that file:
   

   void Foam::interstitialInletVelocityFvPatchVectorField::updateCoeffs()
   {
       if (updated())
       {
           return;
       }
   
       const fvPatchField<scalar>& alphap =
           patch().lookupPatchField<volScalarField, scalar>(alphaName_);
   
       operator==(inletVelocity_/alphap);
       fixedValueFvPatchVectorField::updateCoeffs();
   }

3. You'll see that the "value" field isn't directly used during the simulation. In fact, the value in "value" should be the result of "inletVelocity_/alphap"... therefore, "value" acts as the current representation of the velocity field for the current time instance or iteration.
4. "inletVelocity" is the actual desired velocity for this inlet

Best regards,
Bruno

[maysmech]

Hi Bruno,
I know the difference between u and U, the actual and superficial velocity with relation of U=alpha*u.
This is the main advantage of "interstitialInletVelocity" to "fixedValue" and "uniformFixedaValue". My question was about why there are two entries in 0/U.air

bottom
{
type interstitialInletVelocity;
inletVelocity uniform (0 0 1.875);
value uniform (0 0 1.875);
phi phi.air;
alpha alpha.air;
}

However I found the answer. The second entry is a dummy value for 0 value reading in paraView. So I should try to use table for first entry "inletVelocity uniform (0 0 1.875);" and modify the source code. I have started to create the new boundary condition based on your comment but have faced to some problems because of C++ knowledge. I will bring the modifications to share with others to write the time varying interstitialInletVelocity BC.

[maysmech]

We want use available boundary conditions of fixedValue (BC1), uniformFixedValue (BC2) and interstitialInletVelocity (BC3) to write own myInterstitialInletVelocity (BC4).
BC4 will have advantages of BC3 (which accounts alpha to have constant mass flow rate in multiphase flows) and BC2 (which accepts table to apply time varying air velocity).

The first step is compiling BC in user directory.

1- Copying BC3 from source to user directory and renaming it to my0InterstitialInletVelocity.

$FOAM_SRC/finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity
to
$WM_PROJECT_USER_DIR/src/finiteVolume/fields/fvPatchFields/derived/my0interstitialInletVelocity

2- Modifying .H and .C files with new name.
3- Writing an appropriate Make/files and options and then compiling it in:

$WM_PROJECT_USER_DIR/src/finiteVolume/

4- Adding this dictionary to controlDict:

libs ("libmyFiniteVolume.so");

In these links the src folder and a test case are available. After extracting it in user directory it needs compile by wmake.
The link of GoldschemidtBC contains my0InterstitialInletVelocity BC in 0/U.air and dictionary in it is controlDict.
The src link contains BC1 to BC4. but is compiled for "my0InterstitialInletVelocity".
The BC4 doesn't work which will be discussed later.

https://www.dropbox.com/s/b54r786b167bmxw/src.tar.gz?dl=0
https://www.dropbox.com/s/8fpj3os65a8hnp9/GoldschmidtBC.tar.gz?dl=0

The next step is doing modification in myInterstitialInletVelocity (BC4) to possible accepting table.

The difference of BC2 to BC1 are:
1- BC2 has a new parameter definition:

const Field<Type>& fld

which I think it is for the new variable:

uniformValue_()

I define uniformInletVelocity_ in BC4 too
2- BC1 uses mapper (which I don't know what does it do):

fixedValueFvPatchField<Type>::fixedValueFvPatchField
(
    const fixedValueFvPatchField<Type>& ptf,
    const fvPatch& p,
    const DimensionedField<Type, volMesh>& iF,
    const fvPatchFieldMapper& mapper
)
:
    fvPatchField<Type>(ptf, p, iF, mapper)
{
    if (&iF && mapper.hasUnmapped())
    {
        WarningIn
        (
            "fixedValueFvPatchField<Type>::fixedValueFvPatchField\n"
            "(\n"
            "    const fixedValueFvPatchField<Type>&,\n"
            "    const fvPatch&,\n"
            "    const DimensionedField<Type, volMesh>&,\n"
            "    const fvPatchFieldMapper&\n"
            ")\n"
        )   << "On field " << iF.name() << " patch " << p.name()
            << " patchField " << this->type()
            << " : mapper does not map all values." << nl
            << "    To avoid this warning fully specify the mapping in derived"
            << " patch fields." << endl;
    }
}

but BC2 uses bypass mapper with the new variable of uniformValue_ :

template<class Type>
uniformFixedValueFvPatchField<Type>::uniformFixedValueFvPatchField
(
    const uniformFixedValueFvPatchField<Type>& ptf,
    const fvPatch& p,
    const DimensionedField<Type, volMesh>& iF,
    const fvPatchFieldMapper& mapper
)
:
    fixedValueFvPatchField<Type>(p, iF),  // bypass mapper
    uniformValue_(ptf.uniformValue_().clone().ptr())
{
    // Evaluate since value not mapped
    const scalar t = this->db().time().timeOutputValue();
    fvPatchField<Type>::operator==(uniformValue_->value(t));
}

I think it uses bypass mapper of BC1 and doesn't rewrite it here. However what we are seeking is seen here (time).

3- we see time again in next class. In this one, it is looking for value or table:

template<class Type>
uniformFixedValueFvPatchField<Type>::uniformFixedValueFvPatchField
(
    const fvPatch& p,
    const DimensionedField<Type, volMesh>& iF,
    const dictionary& dict
)
:
    fixedValueFvPatchField<Type>(p, iF),
    uniformValue_(DataEntry<Type>::New("uniformValue", dict))
{
    if (dict.found("value"))
    {
        fvPatchField<Type>::operator==(Field<Type>("value", dict, p.size()));
    }
    else
    {
        const scalar t = this->db().time().timeOutputValue();
        fvPatchField<Type>::operator==(uniformValue_->value(t));
    }
}

4- The last difference is "clone" which is added to BC2 and again I don't know what it is.

However, I tried many different tries and errors by adding classes to BC4 but not possible to compile it successfully.

Two possibles for errors are:
1- mistakes in defining parameters
2- two "operator== ..." in updateCoeff of BC4:

void Foam::myInterstitialInletVelocityFvPatchVectorField::updateCoeffs()
{

Info << "Banana1" <<endl;
    if (updated())
    {
        return;
    }
    const scalar t = this->db().time().timeOutputValue();             //
    fvPatchField<vector>::operator==(uniformInletVelocity_->value(t));  //

   // fixedValueFvPatchField<Type>::updateCoeffs();                     //

    const fvPatchField<scalar>& alphap =
        patch().lookupPatchField<volScalarField, scalar>(alphaName_);

    operator==(uniformInletVelocity_/alphap);
    fixedValueFvPatchVectorField::updateCoeffs();
}

It needs to check two things for update: alpha and uniformInletVelocity. Again I tried different configurations (separated, together, ...) but it doesn't compile at all

Sorry for this long post and thanks in advance for any suggestion.

[mechem]

Originally Posted by maysmech

We want use available boundary conditions of fixedValue (BC1), uniformFixedValue (BC2) and interstitialInletVelocity (BC3) to write own myInterstitialInletVelocity (BC4).
BC4 will have advantages of BC3 (which accounts alpha to have constant mass flow rate in multiphase flows) and BC2 (which accepts table to apply time varying air velocity).

Hi maysmech,
This is what exactly I need for finding minimum fluidization velocity.
I need a gradually increase in fluidization velocity.
I used table with fixed value but the results was mistake because of inlet porosity is not considered in fixedValue.
Did you find any solution? Please share it if you have found.
Best regards.