[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 .