[sven]

I need to calculate a nusselt number for a body in a crossflow for different time steps. Does OpenFOAM provide a function which can do that? If not, can I somehow use the probing function to write out a temperature gradient at a wall, like I can write out fields at certain points? Has anyone ever done something like this? Thanks a lot!

[santos]

Hi Sven,

You can see how I modified simpleFoam and turbFoam (now its pisoFoam) for determination of Sherwood number:

http://openfoamwiki.net/index.php/Co...mpleScalarFoam
http://openfoamwiki.net/index.php/Co...turbScalarFoam

There is some coding and recompilation involved, but not too difficult. Just make sure you use the adequate dimensions for temperature in place of mass fraction.

Regards,
Jose Santos

[sven]

Hey Sanots,

thanks for your answer. I had a look at your source Code files, especially at simpleScalarFoam.C. I think, what I need is something similar to the following lines in your code:

// Calculates kc and Sh on each patch
         Info<< "Calculating kc and Sh" << endl;

label patchi = mesh.boundaryMesh().findPatchID("electrode1");
label patchj = mesh.boundaryMesh().findPatchID("electrode2");

// kc = 1 / Tb * D * (dT/dy)_wall
                kc.boundaryField()[patchi] =
                  1/Tb.value()*DT.value()*-T.boundaryField()[patchi].snGrad();

                kc.boundaryField()[patchj] =
                  1/Tb.value()*DT.value()*-T.boundaryField()[patchj].snGrad();

I just want to get the gradient, so I guess it should look like this:

label patchi = mesh.boundaryMesh().findPatchID("myPatch");
gradT.boundaryField()[patchi]=T.boundaryField()[patchi].snGrad();

Where "myPatch" is the name of the patch for which I want to get the Temperature gradient.
and at the end of the code I need something like

volScalarField output
           (
                IOobject
                (
                    "Sh",
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),

        output=gradT
           );

        runTime.write();

Is it correct like this? Thanks a lot!

[santos]

Yes, you are on the right track. Look below for my suggestion. Regards!

volScalarField gradT
            (
                IOobject
                (
                    "gradT",
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh,
                dimensionedVector
                (
                    "gradT",
                    T.dimensions()/dimLength,
                    0
                )
            );

label patchi = mesh.boundaryMesh().findPatchID("myPatch");
gradT.boundaryField()[patchi]=T.boundaryField()[patchi].snGrad();
runTime.write();

[sven]

Thanks a lot Santos, I got it working. The solver now writes out the gradT for myPatch in every time directory. However, I want the solver to write all these data only in one file instead of several files. I think I can perhaps use the probe function, but I dont know how to probe on a patch. Do you know how this works or do you have another idea? Thank you very much! I really appreciate your help!

Sven

[santos]

I am not familiar with the probe function, sorry. I normally extract gradT values in one file in other way:

1 - Make your solver write gradT on the screen with the patch name, normally you want an area-averaged value. Look in the solvers I mentioned above for guidance.

2 - Launch the simulation and redirect your output to a log file

simpleScalarFoam > log &

3 - Extract gradT values to another file (here its gradTvalues):

grep <your_patch> <log_file> | awk '{print $8}' > gradTvalues

This line will look for 'your_patch' in you 'log_file' and will extract the 8th entry in that line (in my case its the gradT value, please change it accordingly).

Regards,
Jose Santos

[vilop6]

hi all

i m intersseted by this topic and i will try it to calculate nusselt number, my quastion is how integrate "gradT" over the patch using any intagration method availble or not in openfoam "trapez, simpson, RkX, ..."

regards

[Goutam]

Dear Santos,

Thanks for your help. I have written the code in the file buoyantBousseinsqSimpleFoam.C. After that when I set wmake, then I am getting error. Is this code is ok? I want to calculate GradT.

[aaron_lan]

Hi Goutam,

Have you solved your problem of calculating GradT in buoyantBousseinsqSimpleFoam? I am also very interested in this case.

[Goutam]

No. But I have calculated local and Average Nusselt number. You can see my post on this. I gave the code.

[giovanni10]

Originally Posted by sven

I need to calculate a nusselt number for a body in a crossflow for different time steps. Does OpenFOAM provide a function which can do that? If not, can I somehow use the probing function to write out a temperature gradient at a wall, like I can write out fields at certain points? Has anyone ever done something like this? Thanks a lot!

Dear Sven,
Did you finally find a solution to your problem? Unfortunately, I`m not an expert in C++. So, It is too difficult for me. I would like to calculate the average Nusselt number. I am working on a 2D laterally and volumetrically heated square cavity. I have seen your discussion here. Could you help me? Thanks in advance!

[liuchaofu]

Hi Goutam.Can you tell me how to calculated local and Average Nusselt number.Thank you .

[nwpukaka]

Originally Posted by santos

Yes, you are on the right track. Look below for my suggestion. Regards!

volScalarField gradT
            (
                IOobject
                (
                    "gradT",
                    runTime.timeName(),
                    mesh,
                    IOobject::NO_READ,
                    IOobject::AUTO_WRITE
                ),
                mesh,
                dimensionedVector
                (
                    "gradT",
                    T.dimensions()/dimLength,
                    0
                )
            );

label patchi = mesh.boundaryMesh().findPatchID("myPatch");
gradT.boundaryField()[patchi]=T.boundaryField()[patchi].snGrad();
runTime.write();

Hi, can I ask you a question regarding gradT,

is T.boundaryField()[patchi] temperature value at boundary field?

but what is the definition of snGrad()?

Regards,
Kan

[ssss]

Why not just:

label patchi = mesh.boundaryMesh().findPatchID("myPatch");

surfaceVectorField TGrad = fvc::interpolate(fvc::grad(T));
vectorField TsurfGrad = FvolGrad.boundaryField()[patchi];
vectorField normal = patch().Sf()/patch().magSf();
scalarField snGradT = TsurfGrad & normal;

Gets the patch ID from its name. Calculates the gradient of T in all surfaces. Then gets the gradient only in the surfaces.

After that it calculates the normal in the surface and the last one gets the gradient in the normal direction of the surface(dT/dn = grad(T)*vectorNormal). Hope that is what your looking for

[AliMahmoodi]

Hi every body

i add energy equation to icoFoam and it was compiled successfuly.
Now i d like to calculate Nusselt Number in duct .
Has any one known how it should be possible<

[wenxu]

Dear Jose Santos,

I searched some of your threads, and I found that your are familiar with the OF. Now I want to calculate the gradient explicitly in OF using upwind scheme. I want to calculate the sign distance function: mag(Grad(phi)) = 1.

It is not difficult to implement this on structured mesh based on FDM, but it is not easy for me to implement it on unstructured mesh based on FVM, such as OF.

Could you give me some hints? Thank you in advance!

Best regards,
Wen

[Garfield]

Hi, Santos
I have a question about the bulk temperature in your files, in your files you said that we need to define the bulk temperature (Tb) in the transportProperties dictionary, but the Tb will change with location, could you tell me how to handle that?
Thanks a lot
Best
Garfield

[santos]

Hi Garfield,

My example does not relate to temperature, rather relates to an arbitrary scalar T (http://openfoamwiki.net/index.php/Co...mpleScalarFoam). Tb is in this case a reference value for the scalar (say reference mass fraction of a component) that is used to determine the mass transfer coefficient at the walls.

Regards,
Jose

[Garfield]

Thanks a lot!

[Scram_1]

Hi Santos,
I tried compiling simpleScalarFoam but its throwing up some errors which I'm not able to correct.
This is the error I'm geting. There is no simpleScalarFoam.o file in the Make directory. I'm using OpenFOAM 2.3x on Windows (Cygwin) if that's of any help

csriram91@SRIRAM-PC /cygdrive/c/Users/csriram91/Desktop/simpleScalarFoam
$ cd /opt/OpenFOAM/OpenFOAM-2.3.x/applications/solvers/incompressible/simpleScalarFoam

csriram91@SRIRAM-PC /opt/OpenFOAM/OpenFOAM-2.3.x/applications/solvers/incompressible/simpleScalarFoam
$ wclean

csriram91@SRIRAM-PC /opt/OpenFOAM/OpenFOAM-2.3.x/applications/solvers/incompressible/simpleScalarFoam
$ wmake
Making dependency files...
In file included from /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/faceZoneMesh.H:33:0,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/polyMesh.H:56,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/lnInclude/fvMesh.H:50,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/lnInclude/fvCFD.H:7,
from simpleScalarFoam.C:33:
/opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/faceZone.H:46:32: fatal error: primitiveFacePatch.H: No such file or directory
#include "primitiveFacePatch.H"
^
compilation terminated.
SOURCE=simpleScalarFoam.C ; x86_64-w64-mingw32-g++ -m64 -Dcygwin64 -DWM_DP -DMSWIN -DLITTLE_ENDIAN -Wall -Wextra -Wno-unused-parameter -Wnon-virtual-dtor -O3 -DNDEBUG -DNoRepository -ftemplate-depth-100 -I/opt/OpenFOAM/OpenFOAM-2.3.x/src/turbulenceModels/RAS -I/opt/OpenFOAM/OpenFOAM-2.3.x/src/transportModels -I/opt/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude -I/opt/OpenFOAM/OpenFOAM-2.3.x/src/OSspecific/MSWindows/lnInclude -c $SOURCE -o Make/cygwin64mingw-w64DPOpt/simpleScalarFoam.o
In file included from /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/faceZoneMesh.H:33:0,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/polyMesh.H:56,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/lnInclude/fvMesh.H:50,
from /opt/OpenFOAM/OpenFOAM-2.3.x/src/finiteVolume/lnInclude/fvCFD.H:7,
from simpleScalarFoam.C:33:
/opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/faceZone.H:46:32: fatal error: primitiveFacePatch.H: No such file or directory
#include "primitiveFacePatch.H"
^
compilation terminated.
simpleScalarFoam.dep:3: recipe for target 'Make/cygwin64mingw-w64DPOpt/simpleScalarFoam.o' failed
make: *** [Make/cygwin64mingw-w64DPOpt/simpleScalarFoam.o] Error 1

csriram91@SRIRAM-PC /opt/OpenFOAM/OpenFOAM-2.3.x/applications/solvers/incompressible/simpleScalarFoam

Thanks!
Ram