[dewey]

It is possible calculate the nusselt number (local, average) with openFoam or with paraview?




I did my simulation with buoyantSimpleFoam

[floquation]

I use swak4Foam for that purpose.

I have attached a topoSetDict and a NusseltDict that I have used.
topoSet creates several horizontal planes, because I have had my NusseltDict calculate the Nusselt number at 10 different planes in order to see whether they yield the same value.
NusseltDict calculates the Nusselt number for each of those planes.

Note that NusseltDict requires some physical parameters, like (height of domain) and (thermal diffusivity). Therefore, I use NusseltDict.template to generate NusseltDict using pyFoamFromTemplate.py.

Altogether, my prepareCase.sh script looks like (I am only showing the part relevant for the Nusselt number):

## Define variables
Wy=2
# Calculate alpha
nu=`grep 'nu \[0 2' constant/transportProperties | sed 's/^[^0-9]*[-(0-9) ]*\] //' | sed 's/;//g'`
Pr=`grep 'Pr \[0 ' constant/transportProperties | sed 's/^[^0-9]*[-(0-9) ]*\] //' | sed 's/;//g'`
nu=`echo ${nu} | sed -e 's/[eE]+*/\\*10\\^/'`
Pr=`echo ${Pr} | sed -e 's/[eE]+*/\\*10\\^/'`
alpha=`echo "($nu)/($Pr)" | bc -l`

# Get temperatures
Ts=(`grep 'value' "0/T.org" | sed -e 's/\s*value\s*uniform\s*//' | sed 's/;//'`)
Ts=(`echo ${Ts[@]} | sed -e 's/[eE]+*/\\*10\\^/'`)
dT=`echo "${Ts[1]}-1*${Ts[0]}" | bc -l | sed 's/-//'`
Tm=`echo "(${Ts[1]}+1*${Ts[0]})/2" | bc -l`

#
PARAMETERS_NUSSELT="{'alpha':$alpha,'dT':$dT,'H':$Wy}"
echo "Parameters_Nusselt: $PARAMETERS_NUSSELT"

## Write dictionaries:
pyFoamFromTemplate.py ./system/NusseltDict $PARAMETERS_NUSSELT || exit 1

## Mesh
echo "----> blockMesh"
blockMesh > ./logs/blockMesh.log || exit 1
## TopoSet
echo "----> topoSet"
topoSet > ./logs/topoSet.log || exit 1

Then, in system/controlDict, make sure to add the following. (I possibly show you too many libs, as I'm not sure which was required for Nusselt. Either way, too many cannot hurt.)

functions
{
    //work-around: otherwise mesh is NULL during construction of FuncObjs.
    doInit {
        type initSwakFunctionObject;
    }

    #include "NusseltDict"
}

libs
(
    "libOpenFOAM.so"
    "libsimpleFunctionObjects.so"
    "libsimpleSwakFunctionObjects.so"
    "libswakFunctionObjects.so"
    "libswakTopoSources.so"
);

Note: I have used this for run-time post-processing.
If you want to post-process it after the simulation, have a look at OF's "postProcess" tool, which can execute FunctionObjects after runtime.

[amdk136]

Hi,

I'm looking to get this plane creation/Nusselt calculation working using your method, however I get the following error after running topoSet:

--> FOAM FATAL ERROR: 
Unknown topoSetSource type expressionToFace

Valid topoSetSource types : 

45
(
boundaryToFace
boxToCell
boxToFace
boxToPoint
cellToCell
cellToFace
cellToPoint
cylinderAnnulusToCell
cylinderAnnulusToFace
cylinderToCell
cylinderToFace
faceToCell
faceToFace
faceToPoint
faceZoneToCell
faceZoneToFaceZone
fieldToCell
labelToCell
labelToFace
labelToPoint
nbrToCell
nearestToCell
nearestToPoint
normalToFace
patchToFace
pointToCell
pointToFace
pointToPoint
regionToCell
regionToFace
rotatedBoxToCell
searchableSurfaceToFaceZone
setAndNormalToFaceZone
setToCellZone
setToFaceZone
setToPointZone
setsToFaceZone
shapeToCell
sphereToCell
surfaceToCell
surfaceToPoint
targetVolumeToCell
zoneToCell
zoneToFace
zoneToPoint
)


    From function static Foam::autoPtr<Foam::topoSetSource> Foam::topoSetSource::New(const Foam::word&, const Foam::polyMesh&, const Foam::dictionary&)
    in file sets/topoSetSource/topoSetSource.C at line 85.

FOAM exiting

Do you have any idea of a fix for this at all? Is it an issue with swak4Foam not working properly? I've simply copy/pasted the topoSetDict into my system directory and run topoSet.

I have also included the libraries in the controlDict that are included in the above post by 'floquation'. I am also using OpenFOAM 6.

Any more information required can be supplied.

Thanks in advance!
Arthur

[floquation]

My guess would be that your swak4Foam is indeed not working, as "expressionToFace" is part of swak, but it is not found.

But if that's the case, I'd expect to see warnings in your log file above the error message you copied. Warnings like "...swak... library not found".
Are there any such warnings in your output?

I assume you already installed a version compatible with OF-6? Installation Problem with OF 6 version

[amdk136]

Hi again,

Here is the rest of the log file from the beginning, there doesn't seem to be any mention about not being able to read swak libraries.

/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 6
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 6-66a81087c208
Exec : topoSet
Date : Nov 28 2018
Time : 11:41:05
Host : "itlrstud054"
PID : 9983
I/O : uncollated
Case : /home/stss2/OpenFOAM/stss2-6/run/correct_geometry/100MM_GEOMETRY/calumsBigToiletFest
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

--> FOAM Warning :
From function static bool Foam::functionObjectList::readFunctionObject(const Foam::string&, Foam::dictionary&, Foam::HashSet<>&, const Foam::word&)
in file db/functionObjects/functionObjectList/functionObjectList.C at line 278
Cannot find functionObject file wallGradT
Create polyMesh for time = 0

Reading topoSetDict

Time = 0
mesh not changed.
Created faceSet plane0_0
Applying source expressionToFace


--> FOAM FATAL ERROR:
Unknown topoSetSource type expressionToFace

Valid topoSetSource types :

45
(
boundaryToFace
boxToCell
boxToFace
boxToPoint
cellToCell
cellToFace
cellToPoint
cylinderAnnulusToCell
cylinderAnnulusToFace
cylinderToCell
cylinderToFace
faceToCell
faceToFace
faceToPoint
faceZoneToCell
faceZoneToFaceZone
fieldToCell
labelToCell
labelToFace
labelToPoint
nbrToCell
nearestToCell
nearestToPoint
normalToFace
patchToFace
pointToCell
pointToFace
pointToPoint
regionToCell
regionToFace
rotatedBoxToCell
searchableSurfaceToFaceZone
setAndNormalToFaceZone
setToCellZone
setToFaceZone
setToPointZone
setsToFaceZone
shapeToCell
sphereToCell
surfaceToCell
surfaceToPoint
targetVolumeToCell
zoneToCell
zoneToFace
zoneToPoint
)


From function static Foam::autoPtr<Foam::topoSetSource> Foam::topoSetSource::New(const Foam::word&, const Foam:olyMesh&, const Foam::dictionary&)
in file sets/topoSetSource/topoSetSource.C at line 85.

FOAM exiting

I am on a university campus computer so can't actually edit or install anything, but I was told that the correct version of swak had been installed on the machine I am using.

I am quite new to OpenFOAM so this is all a bit overwhelming, but thank you for your reply - it's appreciated.

Arthur

[floquation]

Originally Posted by amdk136

Here is the rest of the log file from the beginning, there doesn't seem to be any mention about not being able to read swak libraries.

Weird. Some ideas / hypotheses:

1. You do not yet include the swak4Foam library. What does your controlDict look like?
2. Check whether the swak libraries are indeed available. They should be in the directory $FOAM_USER_LIBBIN (on Linux). Run: "ls $FOAM_USER_LIBBIN" and see what's in there.
3. I never used OF6. Perhaps they removed a feature from swak (unlikely). (Or you only have a partial installation on your system.) If the above doesn't work, do you perhaps have an older OF version installed? Then give that a brief try.

Originally Posted by amdk136

I am on a university campus computer so can't actually edit or install anything, but I was told that the correct version of swak had been installed on the machine I am using.

I am quite new to OpenFOAM so this is all a bit overwhelming, but thank you for your reply - it's appreciated.

I respect that you're new, but then especially you might appreciate this: I am also working on a university (Linux) computer without root access, but I can install openFoam and swak4Foam. I don't know whether you are on Linux, but that's the strength of Linux: I can just compile OF and swak from source and have it "installed" for me personally.

[amdk136]

Floquation,


Thank you again for your reply. It turns out that it was an issue with Swak not compiling correctly. My supervisor has corrected the problem just this morning. The planes now generate.



With regards to being a beginner, I have only recently begun to use Linux so I am still trying to figure it out, although with your help I've also learned what's wrong and how to rectify it. Small steps at a time.


Thank you for your help, it is much appreciated!


Arthur

[farshadexp]

Hi guys;
I have written a function object via swak4FOAM for nusselt number calculation. Is there any cases to verify this code?
I know that the best verification is to compare modeling results with analytical solutions. But I need an OpenFOAM case.
highly appreciated