[aelmoe]

Hey all,

First of all: i have been looking for a solution quite a while in this forum and couldn't find a suitable answer.

I am currently setting up a case, where i want do depict the velocitys in a river where a discharge channel of an hydropowerplant rejoins the main river channel.


Presteps were blockMesh, surfaceFeatureExtract, snappyHexMesh and setFields.


I only have Input / Inlet data in m³/s hence i think i have to use the flowRateInletVelocity boundary for both my Inlets (1: main channel; 2: discharge channel) in 0/U.



As i view my resuluts after the solving, it seems like everything "flow" or "velocity" is going over the atmosphere patch.

so far i have tried to just set a volumetricFlowRate and switch the additonal properties extrapolateProfile as well as the value for the volumetricFlowRate on and off.

Do you have any recommendation, so that the velocity is flowing on the soil of my mesh (i named it for projectpurposes Diff_Ref)?


My code for U ist

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

internalField   uniform (1 0 0);

boundaryField
{
    inlet1
    {
        type            flowRateInletVelocity;
        volumetricFlowRate constant 1.4;
        //value           uniform (1.4 0 0);
        extrapolateProfile  yes;
    }
    inlet2
    {
        type            flowRateInletVelocity;
        volumetricFlowRate constant 0.6;
        //value           uniform (0.6 0 0);
        //extrapolateProfile  yes;
    }
    outlet
    {
        type            freestream;
        freestreamValue uniform (1 0 0);
    }
    frontAndBack
    {
        type            noSlip;
    }    
    soil
    {
        type            noSlip;
    }
    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    Diff_Ref
    {
        type            slip;
    }
}

my complete case can be seen here:


https://1drv.ms/u/s!AgK-q6eTTXN1xEDHd2pGFGA-l3hx?e=HHaZax


Thanks in advance,
aelmoe

[amirhosseintaran]

Dear aelmoe , have you tried inlet-outlet bc ( for velocity and maybe alpha) for your atmospheric patch ?

[Tobermory]

From a quick check of your inlet boundaries, you have set the following for alpha:

    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }
    inlet2
    {
        type            fixedValue;
        value           uniform 1;
    }

i.e. setting alpha = 1 across the whole of the inlet patch. In other words, you are setting the water level to the top of the domain. The fixed volume flow boundary then controls the flow rate, and so it makes sense I think that the code fills the domain with water, from the inlets downward.

You need to do something more realistic with the water levels at the two inlets. Funkysetboundaryfield (part of swak4Foam) is a good tool for this, although you should also be able to do it with the vanilla distribution using some simple coding. Good luck.