[milad653279]

Dear Guys

Could anyones explain the difference between bouyantpressure and fixedFluxPressure boundary conditions? Please explain with mathematical formula.

Regards

[Bloerb]

The best advice i can give is to learn the basics of the code language. Which is difficult because there nearly no documentation but it is quite straightforward:

bouyantpressure

    // If the variable name is "p_rgh", "ph_rgh" or "pd"
    // assume it is p? - rho*g.h and set the gradient appropriately.
    // Otherwise assume the variable is the static pressure.
    if
    (
        dimensionedInternalField().name() == "p_rgh"
     || dimensionedInternalField().name() == "ph_rgh"
     || dimensionedInternalField().name() == "pd"
    )
    {
        gradient() = -rho.snGrad()*(g.value() & patch().Cf());
    }
    else
    {
        gradient() = rho*(g.value() & patch().nf());
}

If your field name is p_rgh you set grad p = - rho*g ...
|| is c++ lingo for "or"
gradient is always the surface normal gradient of the field your boundary condition is applied for
rho.snGrad is the surface normal gradient of the density field.
"&" is the scalar product and Cf is the face center vector nf is the face normal vector. Hence the gradient in normal direction equals rho*g or n*grad(rho)*g

fixedFluxPressure

        gradient() = (phiHbyAp - phip)/patch().magSf()/(*DppPtr);

This one is different as you can see. phip is the flux at the patch. The flux is the velocity at the face of a cell (times density for compressible solvers). magSf is the surface area vector. To understand phiHbyAp you need to understand how to simple algorithm in openfoam works, but it is a predicted flux. DppPtr is the pressure diffusivity field. I have seen good explanations on this forum for this boundary condition so you should be able to find something. The basic idea is that this becomes a zeroGradient if phiHbyAp - phip equals zero. Which it should. It is simply calculated a bit differently for better performance.

Not quite what you might be looking for but it should get you started.

[mo_na]

you can also check out this thread:
http://www.cfd-online.com/Forums/ope...tml#post514589