[tnk]

Hi, all!

I am trying to use pressureInletVelocity BC for U-field

boundaryField
{
    inlet
    {
        type            pressureInletVelocity;
        value           uniform (0 0 0);
    }

that work fine in sonicFoam solver.
However in rhoSonicFoam I'm getting the following message on fist timestep

.....    
request for surfaceScalarField phi from objectRegistry region0 failed
    available objects of type surfaceScalarField are

4
(
weightingFactors
limitedLinearVLimiter(rhoU)
differenceFactors_
phiv
)
.....

Does anyone know the cause of this error, and how to solve this?

OpenFOAM-1.5

------------
Best regards
Leonid

[cliffoi]

rhoSonicFoam does not use the default phi variable, but rather phiv. You must explicitely specifiy the name of the flux field in the inlet boundary definition.

boundaryField
{
inlet
{
type pressureInletVelocity;
value uniform (0 0 0);
phi phiv;
}

[Julian K.]

I encountered the same problem for rhoSonicFoam. I explicitly defined the name of the flux field in the inlet boundary definition, as you suggested, cliffoi. However, eventually, I got the very same error again.

[cliffoi]

This suggests to me the same problem but in a different place. The default name phi is used in numerous places in OpenFOAM. If you can isolate where the error is taking place, the solution should be the same or similar.

[Julian K.]

I found the correct definition for the boundary condition 'totalPressure':

...
boundaryField
{
    inlet
    {
    type            totalPressure;
    p0        uniform 1.01325e+05;
    U        U;
    phi        phi;
    rho        none;
    psi        none;
    gamma        1.4; 
    value        uniform 1.01325e+05;
    }

...