
[Sponsors] 
November 22, 2010, 05:41 
Nusselt number over theta

#1 
New Member
Snehal Janwe
Join Date: May 2010
Location: Stuttgart
Posts: 10
Rep Power: 9 
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 0360). 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: 9 
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: 9 
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: 9 
Quote:
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: 9 
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''/(TsT∞) >> 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: 9 
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 

March 17, 2011, 05:46 

#7 
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 9 
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: 9 
You can calculate that in paraFoam. Use Filter > Calculator.
So it is possible to calculate (TTref) on it to generate a new field. In order to get only T surface you will need to Filter > ExtractBlock your patch. 

March 17, 2011, 16:23 

#9 
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 9 
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: 9 
yes...just select your plot, click file > save data.
it will save as .csv for external tools like excel, matlab or R Cran 

March 18, 2011, 15:23 

#11 
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 9 
thank a lot for your guidance.
regards. 

April 9, 2011, 02:26 

#12 
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 9 
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: 9 
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: 8 
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_hotT_ini)*k); } localNusselt.write(); } Info<< "End" << endl; return 0; } 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: 9 
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 

December 3, 2015, 07:14 

#16 
New Member
Mohammad Reza
Join Date: Sep 2015
Posts: 14
Rep Power: 4 
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 

June 6, 2016, 11:49 

#17 
Member
Ram
Join Date: Oct 2015
Posts: 36
Rep Power: 4 
Hey Bana,
Have you managed to figure out how to calculate the bulk temperature in openFOAM? I'm trying to calculate the Nusselt Number for which I need the bulk temperature. Thanks!! Ram 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Mesh Refinement  Luiz Eduardo Bittencourt Sampaio (Sampaio)  OpenFOAM Mesh Utilities  42  January 8, 2017 13:55 
DecomposePar unequal number of shared faces  maka  OpenFOAM PreProcessing  6  August 12, 2010 09:01 
BlockMeshmergePatchPairs  hjasak  OpenFOAM Native Meshers: blockMesh  11  August 15, 2008 07:36 
Unaligned accesses on IA64  andre  OpenFOAM  5  June 23, 2008 10:37 
Trimmed cell and embedded refinement mesh conversion issues  michele  OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...  2  July 15, 2005 04:15 