CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Nusselt number over theta

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

Like Tree8Likes
  • 1 Post By aerothermal
  • 2 Post By aerothermal
  • 2 Post By aerothermal
  • 1 Post By aerothermal
  • 1 Post By Goutam
  • 1 Post By aerothermal

Reply
 
LinkBack Thread Tools Display Modes
Old   November 22, 2010, 05:41
Default Nusselt number over theta
  #1
New Member
 
Snehal Janwe
Join Date: May 2010
Location: Stuttgart
Posts: 10
Rep Power: 7
snehal is on a distinguished road
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
snehal is offline   Reply With Quote

Old   November 22, 2010, 14:18
Default
  #2
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
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?
aerothermal is offline   Reply With Quote

Old   March 13, 2011, 04:57
Default calculating nusselt number
  #3
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
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.
anijdon is offline   Reply With Quote

Old   March 13, 2011, 11:25
Default
  #4
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
Quote:
Originally Posted by anijdon View Post
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
I might solve your problem.
Let me know if you have difficulties.

regards,

aeroThermal
Goutam likes this.
aerothermal is offline   Reply With Quote

Old   March 13, 2011, 16:05
Default
  #5
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
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!!!
anijdon is offline   Reply With Quote

Old   March 16, 2011, 14:00
Default
  #6
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
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.
aerothermal is offline   Reply With Quote

Old   March 17, 2011, 05:46
Default
  #7
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
hello.
thanks a lot . but my problem is that I don't know how to calculate DeltaT.
anijdon is offline   Reply With Quote

Old   March 17, 2011, 10:50
Default
  #8
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
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.
aerothermal is offline   Reply With Quote

Old   March 17, 2011, 16:23
Default
  #9
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
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
anijdon is offline   Reply With Quote

Old   March 17, 2011, 16:35
Default
  #10
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
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.
aerothermal is offline   Reply With Quote

Old   March 18, 2011, 15:23
Default
  #11
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
thank a lot for your guidance.
regards.
anijdon is offline   Reply With Quote

Old   April 9, 2011, 02:26
Default
  #12
Member
 
Maryam Mousazadeh
Join Date: Oct 2010
Posts: 47
Rep Power: 6
anijdon is on a distinguished road
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
anijdon is offline   Reply With Quote

Old   November 10, 2011, 09:57
Default
  #13
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
Dear Maryam,

your zip file is empty.

Regards,

aerothermal
aerothermal is offline   Reply With Quote

Old   February 19, 2012, 09:34
Default
  #14
Senior Member
 
Goutam Saha
Join Date: Dec 2011
Location: UK
Posts: 128
Rep Power: 5
Goutam is on a distinguished road
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.
Goutam is offline   Reply With Quote

Old   March 22, 2012, 08:58
Default Average Nusselt
  #15
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
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.
aerothermal is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Mesh Refinement Luiz Eduardo Bittencourt Sampaio (Sampaio) OpenFOAM Mesh Utilities 41 January 17, 2013 03:43
DecomposePar unequal number of shared faces maka OpenFOAM Pre-Processing 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


All times are GMT -4. The time now is 03:06.