CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Temperature Gradient at Wall (http://www.cfd-online.com/Forums/openfoam/65701-temperature-gradient-wall.html)

sven June 23, 2009 13:48

Temperature Gradient at Wall
 
I am simulating a laminar channel flow with heated walls. To calculate y nusselt number I first want to calculate the temperature gradient at the wall. Unfortunately I couldnt find some function similar to "WallGradU" which is able to calculate the wall temperature gradient, like "WallGradU" does it for the velocity gradient. Has anyone an idea how I could get the temperature gradient out of OpenFOAM? Can the "WallGradU" function be edited to get the temperature gradient?

awacs June 23, 2009 22:18

Hi sven,

I am interested in this problem too. I am new to OpenFOAM. I want to simulate the filling process of non-newtonian fluids into a heated cavity.The energy equation was added to the interFoam solver to calculate the temperature field.
At the heated wall:

1) The temperature of non-newtonian fluid is assumed equal to the wall's (in my case,the thermal conductivity of the wall is much larger than that of the non-newtonian fluid ).

2) A coupled solver such as chtMultiRegionFoam can be created to solve this problem. Combination of heatConductionFoam and interHeatFoam (interFoam with energy equation) for conjugate heat transfer between a solid region and fluid region.

I am working on the second part.

If there is any development, please let me know.

Best regards,
Jitao

santos June 24, 2009 04:27

Hi Sven,

Make a copy of wallGradU, replace U with T, volVectorField with volScalarField and dimensionedVector with dimensionedScalar. It should work!

Regards,
Jose Santos

Quote:

Originally Posted by sven (Post 220245)
I am simulating a laminar channel flow with heated walls. To calculate y nusselt number I first want to calculate the temperature gradient at the wall. Unfortunately I couldnt find some function similar to "WallGradU" which is able to calculate the wall temperature gradient, like "WallGradU" does it for the velocity gradient. Has anyone an idea how I could get the temperature gradient out of OpenFOAM? Can the "WallGradU" function be edited to get the temperature gradient?


svens June 24, 2009 12:16

Hi Santos - thanks for your reply.

I have the same intention like sven and tried your advise.
Sadly I received some errors while creating the new wallGradT:

Line 80 - error: Expected primary-expressions before '(' token
Line 83 - error: 'scalar' is not a class of namespace

PHP Code:

#include "fvCFD.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

int main(int argcchar *argv[])
{
    
timeSelector::addOptions();
    
#include "setRootCase.H"
#   include "createTime.H"
    
instantList timeDirs timeSelector::select0(runTimeargs);
#   include "createMesh.H"

    
forAll(timeDirstimeI)
    {
        
runTime.setTime(timeDirs[timeI], timeI);
        
Info<< "Time = " << runTime.timeName() << endl;

        
IOobject Theader
        
(
            
"T",
            
runTime.timeName(),
            
mesh,
            
IOobject::MUST_READ
        
);

        
// Check U exists
        
if (Theader.headerOk())
        {
            
mesh.readUpdate();

            
Info<< "    Reading T" << endl;
            
volScalarField T(Theadermesh);

            
Info<< "    Calculating wallGradT" << endl;

            
volScalarField wallGradT
            
(
                
IOobject
                
(
                    
"wallGradT",
                    
runTime.timeName(),
                    
mesh,
                    
IOobject::NO_READ,
                    
IOobject::AUTO_WRITE
                
),
                
mesh,
                
dimensionedScalar
                
(                                                 <- line 80
                    
"wallGradT",
                    
T.dimensions()/dimLength,
                    
scalar::zero                              <- line 83
                
)
            );

            
forAll(wallGradT.boundaryField(), patchi)
            {
                
wallGradT.boundaryField()[patchi] =
                    -
T.boundaryField()[patchi].snGrad();
            }

            
wallGradT.write();
        }
        else
        {
            
Info<< "    No T" << endl;
        }
    }

    
Info<< "End" << endl;

    return 
0;


I am an absolutely beginner and I didn't find a solution for these errors so far.
About some additional help I would be really helpful.

Thanks a lot & regards
svens

santos June 24, 2009 12:20

Replace scalar::zero with 0 and all should be well.

Regards,
Jose Santos

svens June 24, 2009 15:23

It works! Perfect - thanks so much.

deji July 23, 2010 05:04

Question: I am able to compute the mean temperature gradient at a specified patch of my choosing. The is essentially 3D, hence the I have a 2D plane wall temperature gradient. Can anyone give me any feedback or advice as to how I can average the temperature gradient along a wall direction, so that I end with an output that comprises two columns such as: x dTmean/dn
x1 *****
x2 *****

Thanks.

Deji

farhagim November 1, 2010 18:25

Hello Jitao,

I would like to know if you were successful with your implementation. I am interested in such a coupled solver ( combination of heatConductionFoam and interHeatFoam ). I would be so grateful if you can help me.

Thanks,

Mehran


Quote:

Originally Posted by awacs (Post 220270)
Hi sven,

I am interested in this problem too. I am new to OpenFOAM. I want to simulate the filling process of non-newtonian fluids into a heated cavity.The energy equation was added to the interFoam solver to calculate the temperature field.
At the heated wall:

1) The temperature of non-newtonian fluid is assumed equal to the wall's (in my case,the thermal conductivity of the wall is much larger than that of the non-newtonian fluid ).

2) A coupled solver such as chtMultiRegionFoam can be created to solve this problem. Combination of heatConductionFoam and interHeatFoam (interFoam with energy equation) for conjugate heat transfer between a solid region and fluid region.

I am working on the second part.

If there is any development, please let me know.

Best regards,
Jitao



All times are GMT -4. The time now is 02:05.