CFD Online Discussion Forums - write out nusselt number (gradient of T, respectively) for timesteps

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)

- OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)

- - write out nusselt number (gradient of T, respectively) for timesteps (http://www.cfd-online.com/Forums/openfoam/69832-write-out-nusselt-number-gradient-t-respectively-timesteps.html)

write out nusselt number (gradient of T, respectively) for timesteps

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!

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

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:

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:

Code:

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

Code:

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!

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

Code:

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();

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

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

Code:

simpleScalarFoam > log &

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

Code:

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

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

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.

Hi Goutam,

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

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

average Nusselt number

Quote:

Originally Posted by sven (Post 235294)

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!

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