[saidc.]

Hi,

I'm trying to do turbulent natural convection heat transfer case with chtMultiRegionFoam. The geometry is here. By the way geometry is 3D. The sphere that is at the origin of the coordinate system is 1023.15 K and the fluid (helium) is 523.15K.

• It starts well to run but after few iterations initial temperature value decreasing. Although the decrease is small, the initial temperature value eventually becomes negative. I first thought it might be because of the mesh, so i refined the mesh but result was the same. Then i tried temperature limits on fvOptions, but this didn't work either.

• Another problem is the results aren't looks like LES. I've researched similar cases and if we were to compare, my results are disgusting, behave like laminar.

For curiosity I changed my case to cavity and made all boundaries wall (adiabatic bc) and it works much better than inlet-outlet one. Unfortunately I want to do this with patches.

I think i'm doing something wrong on boundary conditions but i can't figure it out. What should I change, what should I try? I am open to any suggestions. Files are attached.

Kind regards,
Said.

For quick look:

fluid/T

internalField   uniform $Tinitial;
boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform $Tinitial;
    }
    outlet
    {
        type            inletOutlet;
        inletValue      uniform $Tinitial;
        value           uniform $Tinitial;
    }
	wall
    {
        type           zeroGradient;
    }
    fluid_to_sphere
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        neighbourFieldName T;
        kappa           kappa;
        Tnbr            T;
        value           uniform $Tinitial;
    }	
}

fluid/p_rgh

internalField   uniform $pInitial;
boundaryField
{
    outlet
    {
        type            fixedValue;
        value           uniform $pInitial;
    }
    inlet
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }
    wall
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }	
    fluid_to_sphere
    {
        type            fixedFluxPressure;
        gradient        uniform 0;
        value           uniform $pInitial;
    }
}

fluid/p

internalField   uniform $pInitial;
boundaryField
{
    outlet
    {
        type            calculated;
        value           uniform $pInitial;
    }
    inlet
    {
        type            calculated;
        value           uniform $pInitial;
    }
    wall
    {
        type            calculated;
        value           uniform $pInitial;
    }
    fluid_to_sphere
	{
        type            calculated;
        value           uniform $pInitial;	
	}
}

fluid/U

internalField   uniform (0 0 0);
boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    outlet
    {
        type        pressureInletOutletVelocity;
        inletValue      uniform (0 0 0);
        value           uniform (0 0 0);
    }
    wall
    {
        type 	fixedValue;
	value 	uniform (0 0 0);		
    }	
    akiskan_to_kure
    {
        type 	fixedValue;
	value   uniform (0 0 0);	
    }
}

[dlahaye]

What do mean by "Then i tried temperature limits on fvOptions, but this didn't work either." ?

[saidc.]

Originally Posted by dlahaye

What do mean by "Then i tried temperature limits on fvOptions, but this didn't work either." ?

Hi dlahaye,

When i add temperature limit for fluid region, solver stops iteration after like 200 iterates. I mean 0 iteration, all parameters are stay same. For example, first 200 iteration initial temperature value decreasing but still positive, after 200 iteration initial temperature is becomes negative, after last iteration parameteres never change.

kind regards,
Said.

[Tobi]

Check out your fluid field in the domain? The negative temperature should occur in e.g. some cell or due to unphysical values for p and U. A work-around to fix your problem is to start with another solver (without your sphere). E.g., rhoSimpleFoam/rhoPimpleFoam. I supose that there is a problem somewhere else and the outcome destroyes your energy equation. You can also test with "incompressiblePerfectGas".

[keitaro7_14]

Please attach a runnable example if you want us to help you, with the corresponding scripts (Allrun, etc.). You uploaded a case which is not directly runnable.

A priori your case does not seem too complicated.

[saidc.]

Originally Posted by keitaro7_14

Please attach a runnable example if you want us to help you, with the corresponding scripts (Allrun, etc.). You uploaded a case which is not directly runnable.

A priori your case does not seem too complicated.

Hi Tobi and Juan,

Case file is 85 mb so i can't upload here. link, this is github download link. Rar file has everything you need, just download and type ./Allrun.

Also i'll try Tobi's advice as soon as possible.

kind regards,
Said.

[peterhess]

Hello Sadic

In:

templates\0\fluid

p_rgh is overall 0.

This is not allowed and should be 1.013e5 (if zou have atmospharic pressure).

That is the main resion for the negative temperature in this solver.

Regards

Peter