[RMF]

Hello community,

I haven't used OF for a while and now I started again with some simulation. When starting to use OF 4 a noticed that the utility wallHeatFlux isn't longer available. The documentation states that the post processing tools were replaced by postProcess, which includes e.g. the functionally of yPlus and wallShearStress. Unfortunately, I haven't found any information on how to use that tool to calculate the wallHeatFlux. Is this really not possible anymore with standard tools?

Regards
RMF

[Tobi]

Dear RMF,

I am not sure the version of OpenFOAM where they introduced the postProcess utility but I think it was around 3.x. As you already know, you should use the postProcess utility. Doing that the first attempt is to use the help argument:

postProcess -help

As you already know, this tool works with the FOAM functions. The output of the above command will tell you, that you can use postProcess with the argument -func or -funcs. The only thing that is missing, are the functions you can execute. The list can be checked using foamList -functionObjects. You will see the list of functions that you can use. However, doing the same with postProcess -list will give you the available functions that you can use directly. If some function is not listed, you have to include the library to the controlDict.

Hope I got everything right; I am using function libs not every day. However, the wallHeatFlux is (if I got it correct) not a function in 4.x because it is in the postProcessing folder named toBeFunctionObjects. Hence, it is still a normal application that you can execute using wallHeatFlux.

shorty@buoyantCavity: wallHeatFlux 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.x-1ca4bbf1d288
Exec   : wallHeatFlux
Date   : Dec 06 2016
Time   : 09:40:26
Host   : "PC114"
PID    : 32754
Case   : /home/shorty/OpenFOAM/shorty-4.x/run/tutorials/heatTransfer/buoyantSimpleFoam/buoyantCavity
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Time = 0
Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

Reading/calculating face flux field phi

Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}


Wall heat fluxes [W]
frontAndBack
    convective: 0
    radiative:  -0
    total:      0
topAndBottom
    convective: 0
    radiative:  -0
    total:      0
hot
    convective: 401.737
    radiative:  -0
    total:      401.737
cold
    convective: -132.097
    radiative:  -0
    total:      -132.097

Time = 100
...

Now I am wondering why you had the question because the old utility still exists.

[RMF]

Dear Tobi,

thanks for your answer. I was confused because I hadn't found the wallHeatFlux utility (I didn't try to execute it and looked just for the code, otherwise I would have noticed directly that the old tool still exists :-))
Meanwhile I had found the Location of the tool as well.

Regards,
RMF

[y_jiang]

Hi Tobi,


I came across your post. I think the thing is that the wallHeatFlux is no longer existed in $FOAM_APP. Instead there is just postProcess.C. Of course, I can still find the wallHeatFlux.C and wallHeatFlux.H here $FOAM_SRC/functionObjects/field/wallHeatFlux.


My question is that if I want to modify the original wallHeatFlux to create a new utility for heat transfer coefficient, what should I do? Could you please give me some hints on it?


BTW, I am working on OF 5.0

[Kevin.H]

Hello Foamers ,
scince a few days I work with the buoyantSimpleFoam solver (OF 4.1) on a heatTransfer case . Now I try to implement the function wallHeatFlux in my Simulation, but everytime I get the message:


--> FOAM FATAL ERROR:
Unknown function type wallHeatFlux


I have read through a lot of threads but i don´t get the Point about this topic.
At first i thought I could implement this function like the wallShearStress function in my System/ControlDict Folder like this: (https://www.openfoam.com/documentati...lHeatFlux.html)


wallHeatFlux1
{
type wallHeatFlux;
libs ("libfieldFunctionObjects.so");
patches (".*rotor_wall");
writeControl timeStep;
writeInterval 1000;
}
wallShearStress1
{
type wallShearStress;
// libs ("libfieldFunctionObjects.so");
writeControl timeStep;
writeInterval 1000;
}

This doesn´t work.


Then I also read that I could change the
(...)utilities/postProcessing/toBeFunctionObjects/wallHeatFlux/Make/files document. (page 29, http://www.tfd.chalmers.se/~hani/kur...run_report.pdf )
But I work in a company for my thesis and I am not allowed to change the Install Datas .

Now my Questions:
Does the first Option (Control Dict) still exist for OpenFoam 4.1 and if yes, can somebody maybe help me with my code or post his solution?
Is there maybe a third way to get the wallHeatFlux?

Best regards
Kevin

[y_jiang]

Kevin,

Copy the file here openfoamx/etc/caseDicts/postProcessing/fields/wallHeatFlux to your system folder. And add #includeFunc wallHeatFlux under functions in your controlDict.
Then, run your job.

[Kevin.H]

Thanks for your quick answer
But in OpenFOAM 4.1 this file doesn´t exist. I have copied it from OpenFOAM 5.0 and implemented this file in my case now. But it still doesn't work (Picture).

Could it be that this function is not integrated in the functionObjectList.C in OpenFOAM 4.1?

EDIT:
It works! I think I undestand now what Tobi wants to tell me with his post! I don´t have to integrate this function in my controlDict. The only think I have to do is to write "wallHeatFlux" in my Terminal. I was a little bit confused, because I did not know that this simple way to get results exist in OF too.
Again thank you Yijiu Jiang and Tobi

Best regards
Kevin

[Esmaeelef]

Hi Tobi,

I am using OF 4.1 and need to calculate heat fluxes on some boundaries. When I use wallHeatFlux utility, the following error comes up. I would be very thankful if you could give me some suggestions to resolve this issue. Thank you very much

Create mesh for time = 0

Time = 0
Selecting thermodynamics package
{
type hePsiThermo;
mixture singleStepReactingMixture;
transport sutherland;
thermo janaf;
energy sensibleEnthalpy;
equationOfState perfectGas;
specie specie;
}

Selecting chemistryReader foamChemistryReader
Fuel heat of combustion :5.00312e+07
stoichiometric air-fuel ratio :17.0854
stoichiometric oxygen-fuel ratio :3.98918
Maximum products mass concentrations:
H2O: 0.124183
CO2: 0.151685
N2: 0.724132
Reading/calculating face flux field phi

new cannot satisfy memory request.
This does not necessarily mean you have run out of virtual memory.
It could be due to a stack violation caused by e.g. bad use of pointers or an out of date shared library
Aborted (core dumped)

[Raza Javed]

Originally Posted by Tobi

Dear RMF,

I am not sure the version of OpenFOAM where they introduced the postProcess utility but I think it was around 3.x. As you already know, you should use the postProcess utility. Doing that the first attempt is to use the help argument:

postProcess -help

As you already know, this tool works with the FOAM functions. The output of the above command will tell you, that you can use postProcess with the argument -func or -funcs. The only thing that is missing, are the functions you can execute. The list can be checked using foamList -functionObjects. You will see the list of functions that you can use. However, doing the same with postProcess -list will give you the available functions that you can use directly. If some function is not listed, you have to include the library to the controlDict.

Hope I got everything right; I am using function libs not every day. However, the wallHeatFlux is (if I got it correct) not a function in 4.x because it is in the postProcessing folder named toBeFunctionObjects. Hence, it is still a normal application that you can execute using wallHeatFlux.

shorty@buoyantCavity: wallHeatFlux 
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.x-1ca4bbf1d288
Exec   : wallHeatFlux
Date   : Dec 06 2016
Time   : 09:40:26
Host   : "PC114"
PID    : 32754
Case   : /home/shorty/OpenFOAM/shorty-4.x/run/tutorials/heatTransfer/buoyantSimpleFoam/buoyantCavity
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Time = 0
Selecting thermodynamics package 
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

Reading/calculating face flux field phi

Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}


Wall heat fluxes [W]
frontAndBack
    convective: 0
    radiative:  -0
    total:      0
topAndBottom
    convective: 0
    radiative:  -0
    total:      0
hot
    convective: 401.737
    radiative:  -0
    total:      401.737
cold
    convective: -132.097
    radiative:  -0
    total:      -132.097

Time = 100
...

Now I am wondering why you had the question because the old utility still exists.

Hi,

I have one question here, When I write wallHeatFlux, it gave me error that thermoPhysicalProperties is missing in constant directory.

Then I put that file, and now it is giving me that turbulenceProperties is missing in constant folder.

Can you please tell, that what are the pre-requisites of using wallHeatFlux?

Thank you