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

Wall heat flux in OF 4.1

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

Like Tree4Likes
  • 3 Post By Tobi
  • 1 Post By y_jiang

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 2, 2016, 05:02
Default Wall heat flux in OF 4.1
  #1
RMF
New Member
 
Join Date: Aug 2012
Posts: 13
Rep Power: 9
RMF is on a distinguished road
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
RMF is offline   Reply With Quote

Old   December 6, 2016, 04:41
Default
  #2
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Augsburg
Posts: 2,330
Blog Entries: 6
Rep Power: 39
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to 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:
Code:
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.

Code:
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.
arvindpj, Kevin.H and hipa like this.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   December 6, 2016, 15:16
Default
  #3
RMF
New Member
 
Join Date: Aug 2012
Posts: 13
Rep Power: 9
RMF is on a distinguished road
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
RMF is offline   Reply With Quote

Old   October 10, 2018, 15:25
Default
  #4
Member
 
Yijiu Jiang
Join Date: Jan 2013
Location: Michigan, US
Posts: 49
Rep Power: 9
y_jiang is on a distinguished road
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
y_jiang is offline   Reply With Quote

Old   November 20, 2018, 03:58
Default
  #5
New Member
 
Kevin Habrock
Join Date: Oct 2018
Posts: 22
Rep Power: 3
Kevin.H is on a distinguished road
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 donīt 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 doesnīt 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



Kevin.H is offline   Reply With Quote

Old   November 20, 2018, 12:31
Default
  #6
Member
 
Yijiu Jiang
Join Date: Jan 2013
Location: Michigan, US
Posts: 49
Rep Power: 9
y_jiang is on a distinguished road
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 likes this.
y_jiang is offline   Reply With Quote

Old   November 21, 2018, 03:12
Default
  #7
New Member
 
Kevin Habrock
Join Date: Oct 2018
Posts: 22
Rep Power: 3
Kevin.H is on a distinguished road
Thanks for your quick answer
But in OpenFOAM 4.1 this file doesnīt 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 donīt 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
Attached Images
File Type: jpg Error.JPG (86.4 KB, 64 views)
Kevin.H is offline   Reply With Quote

Old   March 12, 2019, 03:32
Default
  #8
New Member
 
Esmaeel Eftekharian
Join Date: Jan 2016
Location: Sydney, Australia
Posts: 14
Rep Power: 6
Esmaeelef is on a distinguished road
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)
Esmaeelef is offline   Reply With Quote

Old   August 25, 2019, 16:44
Default
  #9
Senior Member
 
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 182
Rep Power: 2
Raza Javed is on a distinguished road
Quote:
Originally Posted by Tobi View Post
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:
Code:
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.

Code:
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
Raza Javed is offline   Reply With Quote

Reply

Tags
of4.1, wall heat flux

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Radiation interface hinca CFX 15 January 26, 2014 18:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 18:44
Heat transfer BC at wall- why need wall thickness? Julie FLUENT 7 February 3, 2012 22:41
how to export "wall heat flux" to tecplot? victor CFX 3 November 27, 2008 10:45
CFX - wall heat flux divarano CFX 2 December 4, 2006 17:14


All times are GMT -4. The time now is 07:02.