|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Snehal Janwe
Join Date: May 2010
Location: Stuttgart
Posts: 10
Rep Power: 16 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
|
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? |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#4 | |
Senior Member
|
Quote:
See the tool, Code:
wallHeatFlux Let me know if you have difficulties. regards, aeroThermal |
||
![]() |
![]() |
![]() |
![]() |
#5 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
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!!!
|
|
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
|
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 |
|
![]() |
![]() |
![]() |
![]() |
#7 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
hello.
thanks a lot . but my problem is that I don't know how to calculate DeltaT. |
|
![]() |
![]() |
![]() |
![]() |
#8 |
Senior Member
|
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. |
|
![]() |
![]() |
![]() |
![]() |
#9 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#10 |
Senior Member
|
yes...just select your plot, click file -> save data.
it will save as .csv for external tools like excel, matlab or R Cran |
|
![]() |
![]() |
![]() |
![]() |
#11 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
thank a lot for your guidance.
regards. |
|
![]() |
![]() |
![]() |
![]() |
#12 |
Member
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 15 ![]() |
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 ![]() would you help me ![]() I attach special formula of nonofluids: formuls.zip kind regards |
|
![]() |
![]() |
![]() |
![]() |
#13 |
Senior Member
|
Dear Maryam,
your zip file is empty. Regards, aerothermal |
|
![]() |
![]() |
![]() |
![]() |
#14 |
Senior Member
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 131
Rep Power: 14 ![]() |
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; } Last edited by Goutam; March 4, 2012 at 08:18. |
|
![]() |
![]() |
![]() |
![]() |
#15 |
Senior Member
|
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 |
|
![]() |
![]() |
![]() |
![]() |
#16 |
Member
Mohammad Reza
Join Date: Sep 2015
Posts: 44
Rep Power: 10 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#17 |
Member
Join Date: Oct 2015
Posts: 63
Rep Power: 10 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#18 |
New Member
Goind Sharma
Join Date: Sep 2018
Posts: 25
Rep Power: 7 ![]() |
Hi,
I am using openfoam v10, trying to find Nusselt number. As far I explore it, I found that its now momentumTranportModel class which encompasses laminar and turbulent models. I am trying to figure out how do I setup my calculation, but finding difficult. surfaceScalarField heatFlux ( fvc::interpolate ( ( turbulence.valid() ? turbulence->alphaEff()() : thermo->alpha() ) ) * fvc::snGrad(h) ); Can someone tell, how do I modify this code for openfoam v 10? Regards, Govind |
|
![]() |
![]() |
![]() |
![]() |
#19 |
New Member
Goind Sharma
Join Date: Sep 2018
Posts: 25
Rep Power: 7 ![]() |
Hello Gautam,
can you please explain me: fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h). My understanding is "h" stands for heat-flux. But from heat transfer calculation, q (heat-flux) = -k_eff * grad(T) Its somewhat confusing me, can you please clear me? Regards, Govind |
|
![]() |
![]() |
![]() |
![]() |
#20 |
Senior Member
|
h is enthalpy, see e.g. https://en.wikipedia.org/wiki/Enthalpy
k_eff īs the sum of laminar and turbulent (therefore total) thermal conductivity, see e.g. Turbulent thermal conductivity |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[mesh manipulation] Mesh Refinement | Luiz Eduardo Bittencourt Sampaio (Sampaio) | OpenFOAM Meshing & Mesh Conversion | 42 | January 8, 2017 12:55 |
DecomposePar unequal number of shared faces | maka | OpenFOAM Pre-Processing | 6 | August 12, 2010 09:01 |
[blockMesh] BlockMeshmergePatchPairs | hjasak | OpenFOAM Meshing & Mesh Conversion | 11 | August 15, 2008 07:36 |
Unaligned accesses on IA64 | andre | OpenFOAM | 5 | June 23, 2008 10:37 |
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues | michele | OpenFOAM Meshing & Mesh Conversion | 2 | July 15, 2005 04:15 |