CFD Online Discussion Forums - Lagrangian Boundary Condition: interstitialInletVelocity

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Lagrangian Boundary Condition: interstitialInletVelocity (https://www.cfd-online.com/Forums/openfoam-solving/131395-lagrangian-boundary-condition-interstitialinletvelocity.html)

Lagrangian Boundary Condition: interstitialInletVelocity

Hello Foamers,

I have a question about interstitialInletVelocity inlet BC which is used in lagrangian/MPPIC/Goldschemidt testcase.

Code:

    bottom

    {

        type            interstitialInletVelocity;

        inletVelocity   uniform (0 0 1.875);

        value           uniform (0 0 1.875);

        phi             phi.air;

        alpha           alpha.air;

    }

What is its difference with fixedvalue in application?
in its .h description it says:

HTML Code:

Description

    Inlet velocity in which the actual interstitial velocity is calculated

    by dividing the specified inletVelocity field with the local phase-fraction.

To find its difference with uniformFixedValue I compared average magnitude of inlet velocity (By using Integration over bottom patch) and found that in fixedvalue (0 0 2) the average of inlet velocity is 2, But in interstitialInletVelocity of ( 0 0 2 ) the average velocity is 4.8 m/s.
I calculated average alpha.air magnitude in this patch = 0.42 and understood that 4.8 m/s=2.0/0.42 as described in .h file.
Seeing the contour of inlet in this condition shows the magnitude of air varies between 4 to 6.51 m/s with the average of 4.89 (is attached) and I don't know why it increases the stated 2 m/s to higher magnitudes. If it considers the solid fractions in inlet patch so it should be some zero magnitude velocities on inlet but there is not seen.

Greetings Maysam,

If you take a look into the C file:

Quote:

Originally Posted by src/finiteVolume/fields/fvPatchFields/derived/interstitialInletVelocity/interstitialInletVelocityFvPatchVectorField.C

Code:

void Foam::interstitialInletVelocityFvPatchVectorField::updateCoeffs()

{

    if (updated())

    {

        return;

    }



    const fvPatchField<scalar>& alphap =

        patch().lookupPatchField<volScalarField, scalar>(alphaName_);



    operator==(inletVelocity_/alphap);

    fixedValueFvPatchVectorField::updateCoeffs();

}

It essentially defines that the fixed boundary value for U at the inlet should be defined as "inletVelocity_/alphap". Therefore, this apparently assumes that:

"inletVelocity_" is a reference velocity for a full "alphap" value, namely "1.0".
"alphap" can never be zero, otherwise it would result in a crash with a SIGFPE: http://en.wikipedia.org/wiki/SIGFPE#SIGFPE
The logic might be that the phase proportion is inversely proportional to the velocity, possibly due to a vacuum-like effect. I.e., when there is very little of this phase (smaller than 1.0), it acts as high-speed+low-pressure combination.

Best regards,
Bruno

Dear Bruno,

This boundary condition 'interstitialInletVelocity' is used in the lagrangian and multiphase solvers:

Code:

lagrangian/MPPICFoam/Goldschmidt/0/U.air:40:        type            interstitialInletVelocity;

lagrangian/DPMFoam/Goldschmidt/0/U.air:40:        type            interstitialInletVelocity;

multiphase/reactingTwoPhaseEulerFoam/laminar/fluidisedBed/0/U.air:25:        type               interstitialInletVelocity;

multiphase/reactingTwoPhaseEulerFoam/RAS/fluidisedBed/0/U.air:25:        type               interstitialInletVelocity;

multiphase/twoPhaseEulerFoam/laminar/fluidisedBed/0/U.air:25:        type               interstitialInletVelocity;

. It seems that this is always used in the inlet BC of continuous phase. So in this case, the item 'inletVelocity' corresponds to the actual velocity predicted from the mass flow rate? So the inlet velocity which is from 'inletVelocity / alpha' is always bigger than the actual one. Do we also need to use this BC for the dispersed phase inlet BC? Thank you so much.

OFFO

Quick answers:

Quote:

Originally Posted by openfoammaofnepo (Post 588912)

It seems that this is always used in the inlet BC of continuous phase.

Yes...

Quote:

Originally Posted by openfoammaofnepo (Post 588912)

So in this case, the item 'inletVelocity' corresponds to the actual velocity predicted from the mass flow rate?

yes...

Quote:

Originally Posted by openfoammaofnepo (Post 588912)

So the inlet velocity which is from 'inletVelocity / alpha' is always bigger than the actual one.

Greater or equal. If alpha is 1.0, then it's equal.

Quote:

Originally Posted by openfoammaofnepo (Post 588912)

Do we also need to use this BC for the dispersed phase inlet BC?

I'm out of context here.

If the dispersed phase is Lagrangian, then you probably cannot use this boundary condition.
If it's another fluid, you just need to configure it accordingly in the names.

The paradigm should be simple enough: if I'm not mistaken, the Lagrangian "phase" will act as a physical net that constrains the fluid passing through it.