[MDietrich]

Hi everyone.
I am modeling an natural river with a bridge. A am using interfoam for solver. I want to know how to fixed the water height in outlet to force the model to have that height at outlet. I want to know which Boundary Conditions must use. Tranks for you help.

[GrivalszkiP]

Hi!

I have the same problem, did you get any solution?

Thanks,

Péter

[mcgoldba]

Same here. Any solution?

Thanks,
Marc

[Federico_]

I posted something in similar below in which I use variableHeightFlowRate but I'd like to understand more about it. It should fix same values of alpha of the inlet with the mass conservation

[mcgoldba]

Hi Federico,

Thank you for the reply. I have tried something similar with the variableHeightFlowRate, however it didn't seem to work for me. I am attempting to simulate a water channel with something similar to an infinite reservoir at the outlet (with a fixed water level). However, the water level drops as the simulation progresses with the variableHeightFlowRate specification. I am now trying with a codedFixedValue boundary as follows. However, I am questioning whether or not it is a numerical issue since my mesh is somewhat coarse.

 
fixedWaterLevel                                              
 {                                                            
     code                                                     
     #{                                                       
         const vectorField Cf = patch().Cf();                 
         scalarField& field = *this;                          
                                                              
         forAll(Cf, facei)                                    
         {                                                    
             field[facei]=(Cf[facei].y() <= -1.68584 ? 1 : 0);
         }                                                    
     #};                                                      
 }

Here -1.68584 is the constant water level I want to specify, and gravity is acting in the "y" direction.

[So_LL]

Hi

Did you find a solution to this need?

I've seen elsewhere to fix the velocity of the outlet to V=Qinlet/Achannel for the depth you require, but this leads to a significant impact from the downstream BC on the modeled velocity. And if running LES, the need to extent the mesh further downstream is quickly overwhelming computationally.

Did you find a more elegant solution?

[Mahmoud Abbaszadeh]

Originally Posted by So_LL

Hi

Did you find a solution to this need?

I've seen elsewhere to fix the velocity of the outlet to V=Qinlet/Achannel for the depth you require, but this leads to a significant impact from the downstream BC on the modeled velocity. And if running LES, the need to extent the mesh further downstream is quickly overwhelming computationally.

Did you find a more elegant solution?

Hi. Have you found any solution?

[dalasrevo]

I am working on a similar problem:
I have a section consisting of a basin open to the atmosphere at the top, fed by a lateral inlet. Then follows a piping (closed at the top, so a section under pressure, because the water level before and after the piping is higher), followed by a basin open to the atmosphere at the top.
The model is fed by a constant volume flow Q at the inlet. In reality, there is a flap at the outlet which keeps the water level in the lower basin constant at the desired level.
At the inlet I work so far with
inlet
{
type variableHeightFlowRateInletVelocity;
volumetricFlowRate 0.5;
flowRate 0.5;
alpha alpha.water;
value uniform (0 0 0);
}

But how do I keep the water level in the lower pool constant?
I have my patches open to the atmosphere with

top1
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

defined.

Someone gave me the tip to "lower the model area by x cm", with x as the desired water level, but I can't figure out how to do that.

[KateBradbrook]

Hello, you can try the following:
make sure the file hRef exists in constant director with a line "value ***;"
Where *** is your desired outlet water level.

Then try the following outlet boundary conditions:
p_rgh
outlet
{
type totalPressure; //fixedValue also possible for static pressure
rho rho;
p0 uniform 0;
value uniform 0;
}

U
outlet
{
type inletOutlet;
inletValue uniform (0 0 0);
value $internalField;
}

alpha.water
outlet
{
type zeroGradient;
}

[dalasrevo]

I solved my problem with a different approach, namely by calculating the expected flux for my water phase at the outlet (using the area to determine the expected velocity) and then using the following boundary condition in U:

    

outlet
    {
        type       outletPhaseMeanVelocity;
        Umean  XXX;
        alpha     alpha.water;
        value     uniform (0.312 0 0);
    }

[Verdant Frond]

I have a (somewhat) similar case and this seems to be working well for my setup.

Thank you!

Originally Posted by dalasrevo

I solved my problem with a different approach, namely by calculating the expected flux for my water phase at the outlet (using the area to determine the expected velocity) and then using the following boundary condition in U:

    

outlet
    {
        type       outletPhaseMeanVelocity;
        Umean  XXX;
        alpha     alpha.water;
        value     uniform (0.312 0 0);
    }

[pipihei]

Originally Posted by Verdant Frond

I have a (somewhat) similar case and this seems to be working well for my setup.

Thank you!

Did you find the downstream velocity is not correct using the setup?