[coroi]

Hi everyone, i am a beginner user of opeFOAM. I have a case to work on, wich is run in the fireFOAM solver , and a question for the meaning of "$internalField ". Consider the next selection of p_rgh Dictionary:


internalField uniform 101325;

boundaryField
{
........
verticalInterior
{
type buoyantPressure;
value $internalField;
}

atmosphereHorizont
{
type totalPressure;
U U;
phi phi;
rho rho;
psi none;
gamma 1.4;
p0 $internalField;
//value $internalField;
}
defaultFaces
{
type empty;
}

}


// ************************************************** *********************** //

So let's get to the question :
Does $internalField in the both patches means that for any timeStep the p-rho*g*h wil be equal to 101325 or that when time is advancing the boundary values for p-rho*g*h is varying and equal to calculated internalfield values?

Thank you very much in advance!
Best regards,
Alexandru

[alexeym]

Hi,

in case of buoyandPressure it's just value for the first time step, then, as the BC is a child of fixedGradient, gradient p_rgh will be set to

gradient() = -rho.snGrad()*(g.value() & patch().Cf());

in case of totalPressure, it's a child of fixedValue BC, and the value will be set to:

operator==(p0p - 0.5*rho*(1.0 - pos(phip))*magSqr(Up))

where p0p is 101325.

[coroi]

Thank you very much Alexey Matveichev . Can I ask you something else ? Where should I search those kind of expressions/explanations like gradient() = .... and operator==... for other BC types ? Are they wrote in some files of /opt/openfoam211/... ?

[alexeym]

Implementations of boundary conditions are located in:

$FOAM_SRC/finiteVolume/fields/fvPatchFields

(I guess $FOAM_SRC in your case is /opt/openfoam211/src)

buoyantPressure and totalPressure are in derived folder.