# Nusselt number over theta

 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 22, 2010, 05:41 Nusselt number over theta #1 New Member   Snehal Janwe Join Date: May 2010 Location: Stuttgart Posts: 10 Rep Power: 8 Hello everybody, I have successfully simulated the case of flow around a circular cylinder with heat transfer using OpenFOAM. For heat transfer I have calculated the nusselt number over the cylinder surface. I just wanted to know, how can I plot Nusselt number over theta(angle 0-360). Thanks in advance

 November 22, 2010, 14:18 #2 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 use paraFoam to do that extract your cylinder boundary with extractBlock plot on intersection and select appropriate axis (z?) select variables... Is your cylinder fully rough?

 March 13, 2011, 04:57 calculating nusselt number #3 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 hello ; I added energy equation to simplefoam and simulated heat transfer around a cube but I don't know how to calculate nusselt number and plot it.all walls of the cube are under constant heat flux. would you help me? thanks.

March 13, 2011, 11:25
#4
Senior Member

Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 104
Rep Power: 7
Quote:
 Originally Posted by anijdon hello ; I added energy equation to simplefoam and simulated heat transfer around a cube but I don't know how to calculate nusselt number and plot it.all walls of the cube are under constant heat flux. would you help me? thanks.
Hi anijdon,

See the tool,

Code:
 wallHeatFlux
Let me know if you have difficulties.

regards,

aeroThermal

 March 13, 2011, 16:05 #5 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 thanks, do you mean wallHeatFluxLaminar utility?but it calculates wall heat flux which is my input data as boundary conditions and I don't need it.I think I need termal gradient to calculate h=q''/(Ts-T∞) >> Nu=hL/k. but I don't know how!!!

 March 16, 2011, 14:00 #6 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 yes...of course you have the heat flux! so it is simpler! do it in paraFoam... 1) extract your cylinder boundary with extractBlock 2) use calculator to evaluate \dot{q}^" / (DeltaT) 3) plot on intersection and select appropriate axis (z?) 4) select variables... Regards, aerothermal Goutam and Sherlock_1812 like this.

 March 17, 2011, 05:46 #7 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 hello. thanks a lot . but my problem is that I don't know how to calculate DeltaT.

 March 17, 2011, 10:50 #8 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 You can calculate that in paraFoam. Use Filter -> Calculator. So it is possible to calculate (T-Tref) on it to generate a new field. In order to get only T surface you will need to Filter -> ExtractBlock your patch. maddalena and Goutam like this.

 March 17, 2011, 16:23 #9 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 I'm sorry, it was so easy.thanks a lot for your helping. excuse me, can we export the result of caculating to matlab or save the data in a separate file?(I'm not well in paraview) thanks kind regards

 March 17, 2011, 16:35 #10 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 yes...just select your plot, click file -> save data. it will save as .csv for external tools like excel, matlab or R Cran Goutam likes this.

 March 18, 2011, 15:23 #11 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 thank a lot for your guidance. regards.

 April 9, 2011, 02:26 #12 Member   Maryam Mousazadeh Join Date: Oct 2010 Posts: 47 Rep Power: 7 hello dear aerothermal; excuse me, I have another problem with heat transfer in openfoam. I want to simulate an incompressible nanofluid flow with heat transfer using simpleFoam (i.e. solver includes an energy equation).The conductivity of the fluid is temperature dependent . I don't know haw can modify the solver and case directories to these properties become temperature dependent ;I took down this threat in this site but I have not received any answer so far, would you help me? I attach special formula of nonofluids: formuls.zip kind regards

 November 10, 2011, 09:57 #13 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 Dear Maryam, your zip file is empty. Regards, aerothermal

 February 19, 2012, 09:34 #14 Senior Member   Goutam Saha Join Date: Dec 2011 Location: UK Posts: 131 Rep Power: 6 dear friends, I have calculated the local Nusselt number. Please see the code. How I will calculate the average Nusselt Number? #include "fvCFD.H" #include "hCombustionThermo.H" #include "basicThermo.H" #include "RASModel.H" #include "wallFvPatch.H" int main(int argc, char *argv[]) { timeSelector::addOptions(); #include "setRootCase.H" #include "createTime.H" instantList timeDirs = timeSelector::select0(runTime, args); #include "createMesh.H" forAll(timeDirs, timeI) { runTime.setTime(timeDirs[timeI], timeI); Info<< "Time = " << runTime.timeName() << endl; mesh.readUpdate(); #include "createFields.H" #include "readRefValues.H" surfaceScalarField heatFlux ( fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h) ); const surfaceScalarField::GeometricBoundaryField& patchHeatFlux = heatFlux.boundaryField(); Info<< "\nWall heat fluxes [W]" << endl; forAll(patchHeatFlux, patchi) { if (typeid(mesh.boundary()[patchi]) == typeid(wallFvPatch)) { Info<< mesh.boundary()[patchi].name() << " " << sum ( mesh.magSf().boundaryField()[patchi] *patchHeatFlux[patchi] ) << endl; } } Info<< endl; volScalarField wallHeatFlux ( IOobject ( "wallHeatFlux", runTime.timeName(), mesh ), mesh, dimensionedScalar("wallHeatFlux", heatFlux.dimensions(), 0.0) ); forAll(wallHeatFlux.boundaryField(), patchi) { wallHeatFlux.boundaryField()[patchi] = patchHeatFlux[patchi]; } wallHeatFlux.write(); Info << "\nNusselt Number:" << endl; volScalarField localNusselt ( IOobject ( "localNusselt", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedScalar("localNusselt",dimless,0.0) ); forAll(localNusselt.boundaryField(),patchi) { localNusselt.boundaryField()[patchi] = length*patchHeatFlux[patchi]/((T_hot-T_ini)*k); } localNusselt.write(); } Info<< "End" << endl; return 0; } aerothermal likes this. Last edited by Goutam; March 4, 2012 at 09:18.

 March 22, 2012, 08:58 Average Nusselt #15 Senior Member     Guilherme da Silva Join Date: Aug 2010 Location: Sao Paulo - Brazil Posts: 104 Rep Power: 7 Two ways: 1) in your code, sum all your Nusselt number values for one patch (not all patches) times de area of each element; sum all areas of elements/cells of the same patch; divide the nusselt values sum by the area sum 2) in paraFoam, use filter "extractBlock" to extract the patch you want the average, use filter "integrate variables", it will open an spreadsheet, look for Area value in Cells or Points, look for Nusselt value in Cells or Points, divide Nusselt integrated value by the Area integrated value. Regards, aerothermal Goutam likes this.

 December 3, 2015, 07:14 #16 New Member   Mohammad Reza Join Date: Sep 2015 Posts: 14 Rep Power: 2 Hi friends I have a question, I want to calculate Nusselt number in a heated pipe at each cross section but for the temperature difference it needs to calculate the bulk temperature which requires computation of integral of U*T over each section (since my simulation is axisymmetric I need to calculate integration along radius instead). Do you have any idea on how to compute the integral in openfoam? thanks in advance

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43 maka OpenFOAM Pre-Processing 6 August 12, 2010 09:01 hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36 andre OpenFOAM 5 June 23, 2008 10:37 michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15

All times are GMT -4. The time now is 09:45.