|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Join Date: Aug 2012
Posts: 13
Rep Power: 14 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Bad Wörishofen
Posts: 2,711
Blog Entries: 6
Rep Power: 51 ![]() ![]() ![]() |
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 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 ...
__________________
Keep foaming, Tobias Holzmann |
|
![]() |
![]() |
![]() |
![]() |
#3 |
New Member
Join Date: Aug 2012
Posts: 13
Rep Power: 14 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#4 |
Member
Yijiu Jiang
Join Date: Jan 2013
Location: Michigan, US
Posts: 49
Rep Power: 13 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Kevin Habrock
Join Date: Oct 2018
Posts: 22
Rep Power: 7 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Member
Yijiu Jiang
Join Date: Jan 2013
Location: Michigan, US
Posts: 49
Rep Power: 13 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Kevin Habrock
Join Date: Oct 2018
Posts: 22
Rep Power: 7 ![]() |
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 |
|
![]() |
![]() |
![]() |
![]() |
#8 |
New Member
Esmaeel Eftekharian
Join Date: Jan 2016
Location: Sydney, Australia
Posts: 16
Rep Power: 10 ![]() |
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) |
|
![]() |
![]() |
![]() |
![]() |
#9 | |
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 ![]() |
Quote:
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 |
||
![]() |
![]() |
![]() |
Tags |
of4.1, wall heat flux |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Radiation interface | hinca | CFX | 15 | January 26, 2014 17:11 |
An error has occurred in cfx5solve: | volo87 | CFX | 5 | June 14, 2013 17:44 |
Heat transfer BC at wall- why need wall thickness? | Julie | FLUENT | 7 | February 3, 2012 21:41 |
how to export "wall heat flux" to tecplot? | victor | CFX | 3 | November 27, 2008 09:45 |
CFX - wall heat flux | divarano | CFX | 2 | December 4, 2006 16:14 |