[WaterHammer1985]

I want to use the totalPressureIncompressible (postProcess -func totalPressureIncompressible) but keep getting the following error message:


Error Message

[69] --> FOAM FATAL ERROR:

    request for volScalarField rhoInf from objectRegistry region0 failed
    available objects of type volScalarField are

17
(
interfaceProperties:K
nut
epsilon_0
alpha.water
rho
k
p_rgh
(0.5*magSqr(U))
nu
gh
nu1
p
rho_0
nu2
alpha.air
k_0
epsilon
)

In the system/controlDict, I have:

functions
{
pressure
    {
        type            pressure;
        functionObjectLibs ("libfieldFunctionObjects.so");
        writeControl    outputTime;
        rhoInf  1000;
        rho     rhoInf;
        pRef    0;
        calcTotal   yes;
        calcCoeff   no;
  }

}

How do I get this to work properly? I'm using interIsoFoam for the solver but don't think that should matter...

[yambanshee]

try this:

functions
{
    totalPressure
    {
        #includeEtc "caseDicts/postProcessing/pressure/totalPressureIncompressible.cfg"

        pRef    0.0;
        rhoInf  1000;
    }
}

If you go to openfoam/ect/caseDicts/postProcessing/pressure you can see that the file included here eventually leads down to a similar function call to what you are requesting here

[WaterHammer1985]

Thanks for the suggestion. I just tried it but am still getting same error. I looked through the files you point to and agree that it leads to similar function call. I've tried adding "rhoInf 1000;" to those files also (throw it on the wall and see what sticks technique) but still get the same error. Any other ideas on how I can get it hooked up?


~/system/controlDict

functions
{
    totalPressure
    {
        #includeEtc "caseDicts/postProcessing/pressure/totalPressureIncompressible.cfg"

        pRef    0.0;
        rhoInf  1000;
    }

}

totalPressureIncompressible.cfg

#includeEtc "caseDicts/postProcessing/pressure/pressure.cfg"

calcTotal     yes;
calcCoeff     no;
rho           rhoInf;

pressure.cfg

type            pressure;
libs            ("libfieldFunctionObjects.so");

executeControl  writeTime;
writeControl    writeTime;
log             false;

[SvenBent]

I think the solver "acts" as compressible solver, and use the density in the NS-equations. Therefore, the rhoInf functionality is not available. If you look at the error message, you can see that rho and rho_0 are available from the objectRegistry.

[69] --> FOAM FATAL ERROR:

    request for volScalarField rhoInf from objectRegistry region0 failed
    available objects of type volScalarField are

17
(
interfaceProperties:K
nut
epsilon_0
alpha.water
rho
k
p_rgh
(0.5*magSqr(U))
nu
gh
nu1
p
rho_0
nu2
alpha.air
k_0
epsilon
)

I would guess that you can get the total pressure from each phase, say rho is the density of water, you would get the totalPressure field for the water phase and vice versa.

Try running the function below:

functions
{
pressure
    {
        type            pressure;
        functionObjectLibs ("libfieldFunctionObjects.so");
        writeControl    outputTime;
        rho     rho; 
        pRef    0;
        calcTotal   yes;
        calcCoeff   no;
  }

}

Best regards

Mathias

[WaterHammer1985]

Thanks for the advice, that worked!