[Goutam]

I have used the following code created by Johan Magnusson. It creates the tool NusseltCalc. Only problem is, when I run NusseltCalc then I got the error:

Command not found. Could you please help me?

I am adding the code as an attachment.

[markusrehm]

Hi,

have you correctly compiled the tool? You need to do a "wmake", see the Wiki for more information on that topic.

Markus

[Goutam]

Dear Members,

This is the code for local Nusselt number:

volScalarField wall_localNusselt
(
IOobject
(
"wall_localNusselt",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedScalar("wall_localNusselt ",dimless,0.0)
);

forAll(wall_localNusselt.boundaryField(),patchi)
{
wall_localNusselt.boundaryField()[patchi] = length*patchHeatFlux[patchi]/((T_hot-T_ini)*k);
}

wall_localNusselt.write();
}

I want to write a code for Average Nusselt Number.

[Goutam]

The code was correct. NusseltCalc is working now.

[Goutam]

How to calculate average Nusselt number?

[markusrehm]

DearGoutam,

I have not used the code but it would be helpful to see the error message.

Markus

[Goutam]

Looking for a response?

[markusrehm]

Hello Goutam,

please be a bit more precise. As far as I understand, the code you posted above calculates the patch-averaged Nusselt number.

Because patchHeatFlux should be the heat flux over the patch in [W/m2], right?

Markus

[Goutam]

Dear Markus,

This code will calculate heat flux and Local Nusselt NUmber at each patch. I am using this code and its working properly.

If you want to calculate average Nusselt number, then just write in the terminal window:

patchAverage wall_localNusselt your_patch_name

You will get your average Nusselt number.

Cheers !!!

[giovanni10]

Originally Posted by Goutam

Dear Members,

This is the code for local Nusselt number:

volScalarField wall_localNusselt
(
IOobject
(
"wall_localNusselt",
runTime.timeName(),
mesh,
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedScalar("wall_localNusselt ",dimless,0.0)
);

forAll(wall_localNusselt.boundaryField(),patchi)
{
wall_localNusselt.boundaryField()[patchi] = length*patchHeatFlux[patchi]/((T_hot-T_ini)*k);
}

wall_localNusselt.write();
}

I want to write a code for Average Nusselt Number.

What does (T_hot-T_ini) stand for ?
-- wall_localNusselt.boundaryField()[patchi] = length*patchHeatFlux[patchi]/((T_hot-T_ini)*k); --

I want to calculate the localNusselt number at a wall which is called "right". I have a rectangular cavity which has 4 walls with the following names: bottom, right, left and top. So, the Nusselt number is calculated as the integration of dT/dx for limits from y=0 to 1, at x=0, which is the "right" wall.
How can I alter your code?
I am using an incompressible Magnetohydrodynamics` solver.
Thanks a lot for your help!

[shash]

Originally Posted by Goutam

Dear Markus,

This code will calculate heat flux and Local Nusselt NUmber at each patch. I am using this code and its working properly.

If you want to calculate average Nusselt number, then just write in the terminal window:

patchAverage wall_localNusselt your_patch_name

You will get your average Nusselt number.

Cheers !!!

Hi Goutam,

I have used the same code and terminal command for calculating the nusselt number for a case of fin tube heat exchanger using chtMultiRegionSimpleFoam solver but i am getting:

Create time

Create mesh for time = 0

Time = 0
    No field NusseltNumber

Time = 1600
    No field NusseltNumber

Time = 1700
    No field NusseltNumber

Time = 1800
    No field NusseltNumber

Time = 1900
    No field NusseltNumber

Time = 2000
    No field NusseltNumber

End

Can you help me with what i m doing wrong.

[shash]

Hi,
From what i understand from code, this is not a post processing utility rather a runtime utility and i need to create a volumetric scalar field NusseltNumber for it to work.
Plz let me know your views.

[Goutam]

Originally Posted by shash

Hi Goutam,

I have used the same code and terminal command for calculating the nusselt number for a case of fin tube heat exchanger using chtMultiRegionSimpleFoam solver but i am getting:

Create time

Create mesh for time = 0

Time = 0
    No field NusseltNumber

Time = 1600
    No field NusseltNumber

Time = 1700
    No field NusseltNumber

Time = 1800
    No field NusseltNumber

Time = 1900
    No field NusseltNumber

Time = 2000
    No field NusseltNumber

End

Can you help me with what i m doing wrong.

This code is developed for 3D cubical domain that is can be used for 2D cavity problem. That's why, this will not work for tube. You need to modify the code according to your problem. Thanks

[gomeslorenzo]

Hello there,

I'm trying to compile the tool but I keep receiving this error:

NusseltCalc.C: In function 'int main(int, char**)':
NusseltCalc.C:61:38: error: missing template arguments before '->' token

My file is attached.

Any ideas why?

Thanks.

[alexeym]

Hi,

RASModel is class name, did you mean turbulence->alphaEff()? (also this method is available only for compressible turbulence models, in case of incompressible model you have to calculate is as nu/Pr + nut/Prt)

[gomeslorenzo]

Thanks for the quickly reply. That killed that error but now I can't find a way to link the libraries I need. The error is this:

/usr/bin/ld: cannot find -lcompressibleTurbulenceModel
/usr/bin/ld: cannot find -lcompressibleRASModels
/usr/bin/ld: cannot find -lcompressibleLESModels
/usr/bin/ld: cannot find -lLESdeltas
/usr/bin/ld: cannot find -lreactionThermophysicalModels
/usr/bin/ld: cannot find -lfiniteVolume
/usr/bin/ld: cannot find -lgenericPatchFields
/usr/bin/ld: cannot find -lspecie
/usr/bin/ld: cannot find -lfluidThermophysicalModels
/usr/bin/ld: cannot find -lsolidThermo

I tryied to create a symbolic link to /usr/bin/ld but the response is that the file already exists.

My options file in /Make dir is this:

EXE_INC = \
    -I$(LIB_SRC)/turbulenceModels \
    -I$(LIB_SRC)/TurbulenceModels/compressible/lnInclude \
    -I$(LIB_SRC)/turbulenceModels/compressible/turbulenceModel/lnInclude \
    -I$(LIB_SRC)/TurbulenceModels/turbulenceModels/lnInclude \
    -I$(LIB_SRC)/transportModels/incompressible/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/reactionThermo/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/solidThermo/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude 
    
EXE_LIBS = \
    -lcompressibleTurbulenceModel \
    -lcompressibleRASModels \
    -lcompressibleLESModels \
    -lLESdeltas \
    -lreactionThermophysicalModels \
    -lfiniteVolume \
    -lgenericPatchFields \
    -lspecie \
    -lfluidThermophysicalModels \
    -lsolidThermo

Thanks for the attention.

[alexeym]

Hi,

it looks much like you've forgotten to set up environment variables.

[gomeslorenzo]

I´m kind of new at this. How can I do that?

[jameswilson620]

basically we can calculate local nusselt numbers over a patch as we've seen in the discussion above. To get an average nusselt number, you must do some area weighting in the case of a non uniform mesh. Below, you calculate the local nusselt number at each face on heatedPatchID and multiply by the faces area. You must also calculate the total patch area. Once each local nusselt number is weighted by its own area of its face on the boundary, you divide the entire sum of area weighted nusselt numbers by the total area. This results in an averaged nusselt number.

Take a uniform mesh for example:
e.g. (A1*Nu1 +A2*Nu2 +... An*Nun)/Atotal = NUM/DEN where A1 is the face area of face 1 on heatedPatchID and Atotal is the entire patch area

and if A1 = A2 = An (uniform mesh), then A1 = Atotal/n = A2 = .. = An

resulting in Atotal(Nu1 + Nu2 + ... +Nun)/(Atotal*n) = (Nu1 + Nu2 + ... +Nun)/n), which quite simply in a basic average of n components. This is how we integrate numerically along a dimension in most cases where we divide the area weighted sum by the total area of that boundary of interest whether it be length, area or volume.

	        label heatedPatchID = mesh.boundaryMesh().findPatchID("heatedBoundaryName");

		const polyPatch& cPatch = mesh.boundaryMesh()[heatedPatchID];

		scalar patchArea = 0.0; 
                scalar eps = 1e-99; //avoid divide by zero

                forAll(cPatch, facei) //Cycle through all of the boundary faces of heatedPatchID to find total patch area
		{
                        localArea = magSf.boundaryField()[heatedPatchID][facei];
			patchArea += localArea; //building DEN
                }
                // i suppose scalar patchArea = sum(magSf.boundaryField()[heatedPatchID]); //would suffice

                scalar averageNusseltNumber = sum(T.boundaryField()[heatedPatchID].snGrad()  * magSf.boundaryField()[heatedPatchID])/(T.boundaryField()[heatedPatchID]-Tsat.value()+eps)/(patchArea + eps); //calculating NUM/DEN

you should get creative with making a dictionary containing your heated boundary names so that the solver reads this dict. at run time to avoid having to hard code the names of the boundaries and recompile every time you have a new case. Put all of this in a header nusseltSomething.H, throw in an info line or have the contents written to a file. I hope this helps

Any comments are welcome.

James

[student666]

Hi,

I'm facing this problem when i type wmake

michele@micheleXubuntu:~/OpenFOAM/michele-2.3.1/run/nusseltCalc$ wmake
g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/opt/openfoam231/src/turbulenceModels -I/opt/openfoam231/src/turbulenceModels/compressible/turbulenceModel/lnInclude -I/opt/openfoam231/src/thermophysicalModels/specie/lnInclude -I/opt/openfoam231/src/thermophysicalModels/reactionThermo/lnInclude -I/opt/openfoam231/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam231/src/thermophysicalModels/solidThermo/lnInclude -I/opt/openfoam231/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam231/src/OpenFOAM/lnInclude -I/opt/openfoam231/src/OSspecific/POSIX/lnInclude   -fPIC -Xlinker --add-needed -Xlinker --no-as-needed Make/linux64GccDPOpt/nusseltCalc.o -L/opt/openfoam231/platforms/linux64GccDPOpt/lib \
         -lcompressibleTurbulenceModel -lcompressibleRASModels -lcompressibleLESModels -lLESdeltas -lreactionThermophysicalModels -lfiniteVolume -lgenericPatchFields -lspecie -lfluidThermophysicalModels -lsolidThermo -lOpenFOAM -ldl   -lm -o /opt/openfoam231/platforms/linux64GccDPOpt/bin/nusseltCalc
/usr/bin/ld: cannot open output file /opt/openfoam231/platforms/linux64GccDPOpt/bin/nusseltCalc: Permission denied
collect2: error: ld returned 1 exit status
make: *** [/opt/openfoam231/platforms/linux64GccDPOpt/bin/nusseltCalc] Error 1
michele@micheleXubuntu:~/OpenFOAM/michele-2.3.1/run/nusseltCalc$

why permission is denied?

thanks a lot

Michele