CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   Question about temperature boundary condition (http://www.cfd-online.com/Forums/openfoam-pre-processing/131259-question-about-temperature-boundary-condition.html)

vasava March 12, 2014 06:25

Question about temperature boundary condition
 
I am simulating a simple case of fluid heated by a hot pipe with chtmultiregionFoam. I do not want to impose any temperature boundary condition at the outlet and observe rise in the temperature of the fluid as it moves from inlet to outlet.

What condition I must use??

Here are contents of my T file.

Code:

boundaryField
{
    inlet
    {
        type            fixedValue;
        value          uniform 278;//300;//
    }
    outlet
    {
        type            inletOutlet;
        value          uniform 278;//300;//
        inletValue      uniform 278;//300;//
    }
    innerfluid2pipe
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value          uniform 278;//300;//
        neighbourFieldName T;
        kappa          fluidThermo;
        kappaName      none;
    }
}


akrasemann March 12, 2014 11:38

I assume this is your T file for the fluid region. Therefore the T file of the solid regions is missing.

Can you specify how you process the multiple regions? Usually the splitMeshRegions utility creates patches named <solidRegion_i>_to_<*> and <fluidRegion_j>_to_<*>. This has obviously not happend in your case, but might be OK, if you use third party software for mesh generation, e.g. enGrid does split the regions with its export function.

The next step would be to clarify where your heat source and heat sink is. Otherwise you end up with an isothermal domain.

vasava March 13, 2014 09:29

Thanks for the reply.

My other T file looks this

Code:

boundaryField
{
    outerwalls
    {
        type            fixedValue;
        value          uniform 300;//
    }
    pipe2 innerfluid
    {
        type            compressible::turbulentTemperatureCoupledBaffleMixed;
        value          uniform 278;//300;//
        neighbourFieldName T;
        kappa          fluidThermo;
        kappaName      none;
    }
}


But what it has to do will the other T files?? Am just curious.


About the mesh creation: I create my mesh in Ansys meshing, import it in fluent, delete interface, convert the interface to interior, save case, convert case file to foam, and use splitmeshregion. This gives me three regions.

akrasemann March 13, 2014 09:55

I'm not familiar with your mesh generation process, but it seems to work fine.
How do you get 3 regions? You have got the fluid inside the pipe and the pipe itself. Where is the third one? A surrounding fluid?

With respect to your fluid T file:
inlet: fixedValue -> 278K set
outlet: inletOutlet -> zeroGradient, if the flux vector is pointing outwards your boundary patch face and fixedValue (in your case 278K) in case of backflow, i.e. the flux is pointing inwards.
innerfluid2pipe: thermally coupled

This looks so far reasonable.

Looking at the T file for your solid, I recognize, that you specify at pipe2innerfluid, that the solid kappa is the same as the fluid kappa, i.e. I would expect: kappa -> solidThermo.

By applying fixedValue 300K to the outerwalls patch you create a heat source. The heat is then transported by conduction (depending on the thermal conductivity of your solid) to the pipe2innerfluid patch, which is thermally coupled with your fluid, making the fluid the heat sink. Given that the fluid is kept at 278K at the inlet, only a small increase in temperature will be observed at the outlet.

So can you explain in detail, what exactly your problem is?

vasava March 14, 2014 03:39

Thank you for your comments.

Quote:

Originally Posted by akrasemann (Post 479774)
How do you get 3 regions?

Sorry i described mesh generation for some other case. I have 2 regions one fluid and one is pipe.

Quote:

Originally Posted by akrasemann (Post 479774)
So can you explain in detail, what exactly your problem is?

The pipe is hot (relative to fluid) and the hot pipe heats up the cold fluid. I ran some test cases and they seem to be going fine. No other errors and the temperature of the fluid coming out at the outlet also seems reasonable.

My concern was that since I am putting a temperature value for the outlet (value uniform 278;) the temperature would remain 278 and not increase.

Next I am planning to extend it to three and more regions for heat exchange. Right now I am just ensuring that everything works with this basic case.

akrasemann March 14, 2014 03:52

You are welcome

vasava March 14, 2014 03:53

Quote:

Originally Posted by akrasemann (Post 479774)
Looking at the T file for your solid, I recognize, that you specify at pipe2innerfluid, that the solid kappa is the same as the fluid kappa, i.e. I would expect: kappa -> solidThermo.

I copied that condition from tutorial 'multiRegionHeater' and 'multiRegionLiquidHeater'. Could you please elaborate on the reason for using ' kappa -> solidThermo' instead of ' kappa -> fluidThermo'.

vasava March 14, 2014 05:04

Could you please answer that last question??

akrasemann March 14, 2014 06:13

In my OF 2.2.2 installation the T files of the multiRegionHeater tutorial are as follows:

heater (solid region):
Code:

    T
    {
        internalField  uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
                value          uniform 300;
            }
            "heater_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa          solidThermo;
                kappaName      none;
                value          uniform 300;
            }
            minY
            {
                type            fixedValue;
                value          uniform 500;
            }
        }

whereas for bottomAir (fluid region)
Code:

    T
    {
        internalField  uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
            }

            "bottomAir_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa          fluidThermo;
                kappaName      none;
                value          uniform 300;
            }
        }

which sounds reasonable to me, as ones specifies the thermal conductivity (kappa) of the active region.

vasava March 14, 2014 07:38

This was fruitful discussion. thanks again and see you around!!


All times are GMT -4. The time now is 12:36.