[dodobenq]

Hey Guys,

I'm trying to simulate the natural convection boundary layer along a vertical flat plate. The aim of this case is to investigate the heat-transfer from the wall (hot) to the surrounding air.
At first I tried to use the Cavity-Case with one heated wall. But then I got some interactions with the surrounding walls, e. g. the ambient temperature raises up. Therefore I'm trying to "open" the bottom and the top of the cavity and thereby in theory the hot air raise up and fresh air moves in. But now I have some problems in finding the right BC. I am thankful for all help and information!!!

Some facts:
- I'm using buoyantPimpleFoam
- I'm using kOmegaSST
- The Cavity has 4 types of patches: hot(wall), top(patch), bottom(patch), side(wall)

Now my BC:
k

hot
    {
        type            fixedValue;
        value           uniform 1e-12;
    }
top 
    {
        type            zeroGradient;
    }
bottom
    {
        type            fixedValue;
        value           uniform 0.00015;
    }
side
    {
        type            fixedValue;
        value           uniform 1e-12;
    }

omega

hot
    {
        type            fixedValue;
        value           uniform 1e-12;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        beta1           0.075;
    }
top
    {
        type            zeroGradient;
    }
bottom  
    {
        type            fixedValue;
        value           uniform 0.0045;
    }
side 
    {
        type            fixedValue;
        value           uniform 1e-12;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        beta1           0.075;
    }

p

ALL
        type            calculated;
        value           uniform 100000;

p_rgh

hot
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
top              
    {
        type         fixedValue;
    value        uniform 100000;
    }
bottom
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
side        
    {
        type         fixedFluxPressure;
        value         uniform 100000;

T

hot
    {
        type            fixedValue;
        value           uniform 333.15; // 60°C
    }
top               
    {
        type            zeroGradient;
    }
bottom           
    {
        type            fixedValue;
        value           uniform 289.15; 
    }
side            
    {
        type            fixedValue;
        value           uniform 289.15; 
    }

U

hot
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
top              
    {
        type            zeroGradient;
    }
bottom   
    {
      type        outletInlet;
    phi        phi;
    outletValue    uniform (0 0 0);
    value        uniform (0 0 0);
    }
side            
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

mut

hot
    {
        type            mutkWallFunction;
        Cmu             0.09; 
        kappa           0.41; 
        E               9.8;  
        value           uniform 0;
    }
top       
    {
        type            calculated;
    }
bottom            
    {
        type            calculated;
    }
side           
    {
        type            mutkWallFunction;
        Cmu             0.09; 
        kappa           0.41; 
        E               9.8;  
        value           uniform 0;
    }

nut

hot
    {
        type            nutLowReWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0;
    }
top                // oben
    {
        type            calculated;
    }
bottom            // unten 
    {
        type            calculated;
    }
side            // Seite 
    {
        type            nutLowReWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0;
    }

Kind Regards,
Dominik

[dodobenq]

Can anybody help me?

[jherb]

What is the problem with your settings? Does the simulation run?

For k I would suggest for both, top and bottom turbulentIntensityKineticEnergyInlet and for omega compressible::turbulentMixingLengthFrequencyInlet. Actually, I am not sure at all why there is a compressible version for omega but non for k.
For side use you have to decide if you want to use some wall function approach.

Could you get some outflow at the bottom?

Is a fixed temperature boundary condition at hot correct? The alternative could be the boundary condition compressible::turbulentHeatFluxTemperature

[dodobenq]

Thanks jherb for your answer!
The number of Iterations explodes after 2 seconds of simulated time :/

I'll try to put your suggestions in the case.
But now I've some further questions:
1) Is there also a "turbulentIntensityKineticEnergyOUTLET" for the patch "top" or
do I have to set it to "turbulentIntensityKineticEnergyInlet" as well?

2) "turbulentIntensityKineticEnergyInlet" - This functions says, that the inlet is turbulent, right? But I want to simulate a natural convection without any turbulence at the inlet

In the meantime I changed the patch "side" from "wall" to "patch".

THANKS!

[agustinvo]

Hello

I am dealing as well with this case. I am checking my BC's on each boundary you say.

What I don't understand at all is the fixed p and p_rgh. The solver only solves one of them, then it get the other.

What is the error you get?

[dodobenq]

Hey Augustin!

I've found another solution for this case on this german website: http://ww3.cad.de/foren/ubb/Forum527...9.shtml#000020

The main problem for this case is the p_rgh-file.
On the website they suggest:

U
    hot
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    top                // oben
    {        
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    bottom            // unten 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    side            // Seite 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }

    front            // vorne 
    {
        type            pressureInletOutletVelocity;
    value        uniform (0 0 0);
    }
---------------------------------
T 
    hot
    {
        type            fixedValue;
        value           uniform 333.15; 
    }

    top                // oben
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15;
    }

    bottom            // unten 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15; 
    }

    side            // Seite 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15;  
    }

    front            // vorne 
    {
        type         inletOutlet;
    inletValue    uniform 289.15;
    value        uniform 289.15; 
    }
------------
p_rgh
    hot
    {
        type         fixedFluxPressure;
        value         uniform 100000;
    }
   
    top                // oben
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }

    bottom            // unten 
    {
        type         totalPressure;
        value         uniform 100000;
    U        U;
    gamma        1;
    p0        uniform    100000;
    phi        phi;
    psi        none;
    rho        rho;
    }

    side            // Seite 
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }

    front            // vorne 
    {
        type         inletOutlet;
    inletValue    uniform 100000;
    value        uniform 100000;
    }

I'm trying to run this case now and will report my solutions.

[agustinvo]

Hi Dominik

Which kind of fluid are you trying to simulate?

I am interested in incompressible ones, but buoyantBoussinesqPimpleFoam is not appropriate for my case. I have to use the incompressible options in buoyantPimpleFoam (the simulation takes a long time) or create a new incompressible solver with buoyancy forces, but this last one does not want to work!

[dodobenq]

Hey!

I'm using compressible gas within a non-steady flow. I want to investigate the heat transfer on a vertical/horizontal flat plate with natural/forced convection.

Kind Regards

[jherb]

Here is the source code of turbulentIntensityKineticEnergyOUTLET:
https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

You could use it for both inlet and outlet, as for the outlet case it automatically is switched to zeroGradient.

You might also set the turbulence at the open boundaries to an outletInlet with an inletvalue of 0 (or perhaps a very small number).

Originally Posted by dodobenq

Thanks jherb for your answer!
The number of Iterations explodes after 2 seconds of simulated time :/

I'll try to put your suggestions in the case.
But now I've some further questions:
1) Is there also a "turbulentIntensityKineticEnergyOUTLET" for the patch "top" or
do I have to set it to "turbulentIntensityKineticEnergyInlet" as well?

2) "turbulentIntensityKineticEnergyInlet" - This functions says, that the inlet is turbulent, right? But I want to simulate a natural convection without any turbulence at the inlet

In the meantime I changed the patch "side" from "wall" to "patch".

THANKS!

[agustinvo]

Hi Dominic! Did you obtain some results?

Are you comparing with any benchmark?