[Werne]

Hello,

I want to use the boundary condition "flowRateInletVelocity" to define a constant massflow of 5g/s at the inlet.
However, I don't know how to define the density of my fluid.
My syntax looks like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.2                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    INLET
    {
        type            flowRateInletVelocity;
        massFlowRate        constant 0.005;
        value           uniform (0 0 0);
    }

    OUTLET
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
    }

If I use this setup, the solver quits with the error:

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

Where do I have to define the density, so that I can use this boundary condition?
I'm using pimpleFoam.

[kmefun]

https://github.com/OpenFOAM/OpenFOAM...hVectorField.H

Description
This boundary condition provides a velocity boundary condition, derived
from the flux (volumetric or mass-based), whose direction is assumed
to be normal to the patch.
For a mass-based flux:
- the flow rate should be provided in kg/s
- if \c rhoName is "none" the flow rate is in m3/s
- otherwise \c rhoName should correspond to the name of the density field
- if the density field cannot be found in the database, the user must
specify the inlet density using the \c rhoInlet entry
For a volumetric-based flux:
- the flow rate is in m3/s
\heading Patch usage
\table
Property | Description | Required | Default value
massFlowRate | mass flow rate [kg/s] | no |
volumetricFlowRate | volumetric flow rate [m3/s]| no |
rhoInlet | inlet density | no |
\endtable
Example of the boundary condition specification for a volumetric flow rate:
\verbatim
myPatch
{
type flowRateInletVelocity;
volumetricFlowRate 0.2;
value uniform (0 0 0); // placeholder
}
\endverbatim
Example of the boundary condition specification for a mass flow rate:
\verbatim
myPatch
{
type flowRateInletVelocity;
massFlowRate 0.2;
rho rho;
rhoInlet 1.0;
}
\endverbatim
The \c flowRate entry is a \c DataEntry type, meaning that it can be
specified as constant, a polynomial fuction of time, and ...
Note
- \c rhoInlet is required for the case of a mass flow rate, where the
density field is not available at start-up
- the value is positive into the domain (as an inlet)
- may not work correctly for transonic inlets
- strange behaviour with potentialFoam since the U equation is not solved