[Mat_fr]

Hi Foamers,


I would like to use the flowRateOutletVelocity boundary condition with a compressible fluid (I am using compressibleInterFoam).


I want to impose a mass flow rate, so I am using the following specifications:

        

        type                flowRateOutletVelocity;
        massFlowRate        0.03;
        rho                 rho;

With this settings, I am getting the following error


--> FOAM FATAL ERROR:
Did not find registered density field rho and no constant density 'rhoOutlet' specified


which is strange as the volScalarField rho is speficied in my time folder.


I don't want to use a constant density to estimate the mass flow rate (as with rhoOutlet option), but I want to use the density field rho computed by the solver.
Is it even possible ?


Thanks for your help,
Mat

[jherb]

It might be thermo:rho or something like rho.air or even thermo:rho.air

[Mat_fr]

Good call, but unfortunately it's not working either. I have tried the different combinations.

[jherb]

Ok, then perhaps this helps:


First try a different boundary condition to get it to run at all. Then also add a writeObject funtion object to the controlDict with object "banana". This should show all available object in the internal database.


https://github.com/OpenFOAM/OpenFOAM...s/writeObjects

[Mat_fr]

Thanks for your help Joachim,


None of the fields in the list given by the writeObject funtion solves this error. Which is strange.



I have tried also with the flowRateInletVelocity boundary condition, but it's the same problem.


When I look to a tutorial example (for instance in tutorials/compressible/rhoPimpleFoam/RAS/squareBendLiq/0/U), we can see the following BC:


inlet
{
type flowRateInletVelocity;
massFlowRate constant 5;
rhoInlet 1000; // Guess for rho
}


Perhaps the comment means that rhoInlet is only used as a guess for the first time step, and then the inlet velocity is adapted in function of the given flow rate and the calculated rho ?
Should be the same with the outlet BC then.



Regards,
Mat

[jherb]

This is the source code of the boundary condition:
https://github.com/OpenFOAM/OpenFOAM...orField.C#L185


So if it does not find a field with the name for rho, you have specified, it tries to use rhoOutlet (see also the description in the header file: https://github.com/OpenFOAM/OpenFOAM...hVectorField.H)


It is not an initial guess but used as constant during the whole run.


But I still do not understand, why it does not find rho: The field is defined in the solver: https://github.com/OpenFOAM/OpenFOAM...teFields.H#L44


But is this field (the weighted average density) what you want for your boundary? Otherwise, two density fields are references here: https://github.com/OpenFOAM/OpenFOAM...teFields.H#L41


If you modify this file, you might get the names by adding something like (not tested):

Info<<"rho1: "<< rho1.name() << endl;
Info<<"rho2: "<< rho2.name() << endl;

Which version of OpenFOAM do you use?

[Mat_fr]

I am using openfoam-6.


I got the names with your piece of code:


-->

rho1: thermo:rho.h2
rho2: thermo:rho.water



Already tried them, and still the same error.

[jherb]

One last idea: What is in the "object" name in the header of the files with the density stored in the time directory?

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "200";
    object      XXXXXX;
}

[Mat_fr]

Hi



Thanks a lot for your time.


The header specifies "rho", but it's still not working.


I have made the test with the compressible/rhoPimpleFoam/RAS/squareBendLiq tutorial.


By default for this tutorial, the inlet BC for U is using a constant density and reads:

    inlet
    {
        type            flowRateInletVelocity;
        massFlowRate    5.0;
        rhoInlet        1000;    // Guess for rho
    }

And if I change it for a variable density with the lines below, it is working in this case!

    inlet
    {
        type            flowRateInletVelocity;
        massFlowRate    5.0;
        rho             rho;
    }

So I think it is a problem of compatibility between the solver and the BC.


Regards,
Mat

[jherb]

I guess your are right. You might try to get an answer from the OpenFOAM foundation by posting this problem on their bug tracker: https://bugs.openfoam.org/


You most probably get a request for funding to implement it, but perhaps also an explanation, why it does not work.


You could try to call db().foundObject<volScalarField>(rhoName_) (or mesh.foundObject<volScalarField>(rhoName_) ) in the solver itself with different names and output, if something was found.



Perhaps, the boundary conditions are evaluated the first time before the rho field exists. But this is just a guess. Another one is, that the name is not correct (some permutation of thermo/rho/rho1/rho.water/...


You could try to add