wallHeatFlux utility for an incompressible case
Hello Foamers,
my current work is to simulate the heat transfer coefficient by a circular cylinder in cross-flow. If i run the case with buoyantSimpleFoam (compressible & kOmegaSST) everything is fine, i can use the wallHeatFlux utility. But if I run the case with buoyantBoussinesqSimpleFoam (incompressible & kOmegaSST) , i have several problems: 1.) How can i generate a Thermophysical model for an incompressible fluid? I can't use hRhoThermo or icoPolynomial etc. 2.) Run the case with hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>; make no sense?! But OpenFoam creates in 0-directory a mut-file wich is only for compressible and writes new k and omega files with compressible wallfunctions, then it calculates for time=0 and at time=10 theres an error. Is the utility only for compressible fluids? And there must be a conflict between kOmegaSST and wallHeatFlux, because set RASModel laminar and the case run. Please help me i am a newbie in CFD regards ------------------------------------------------------------------------------ Wall heat fluxes [W] KUGEL 3.47426 Time = 10 Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>> Reading/calculating face flux field phi Selecting RAS turbulence model kOmegaSST --> Upgrading k to employ run-time selectable wall functions Backup original k to k.old Writing updated k --> Upgrading omega to employ run-time selectable wall functions Backup original omega to omega.old Writing updated omega --> Creating mut to employ run-time selectable wall functions Writing new mut --> Creating alphat to employ run-time selectable wall functions Writing new alphat bounding k, min: 0 max: 1.1343e-09 average: 2.76378e-13 #0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::operator/<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #6 Foam::compressible::RASModels::kOmegaSST::F2() const in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #7 Foam::compressible::RASModels::kOmegaSST::kOmegaSS T(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&, Foam::word const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #8 Foam::compressible::RASModel::adddictionaryConstru ctorToTable<Foam::compressible::RASModels::kOmegaS ST>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #9 Foam::compressible::RASModel::New(Foam::GeometricF ield<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::basicThermo const&, Foam::word const&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #10 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/wallHeatFlux" #11 __libc_start_main in "/lib/libc.so.6" #12 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/wallHeatFlux" Floating point exception |
I have solved my first problem and added wallHeatFluxRho, now i can use hRhoThermo etc.
But my current problem is that I can't use wallHeatFluxRho or wallHeatFlux with kOmegaSST. I tried to change pressure values from zero to 1e-12 on whole calculation field on first time step, without sucess. as in http://www.cfd-online.com/Forums/openfoam/72534-wallheatflux-utility-openfoam1-6-a.html In my opinion, this would solve my problem if openfoam don't calculate the first time step. But I need a solution for the next time steps. Nobody has an idea to solve this problem? regards |
wallheatflux for incompressible flows
1 Attachment(s)
Hi,
I modified the standard wallHeatflux utility which comes default with OF into a version for incompressible flows already a while ago. Also removed a bug out of the code. Well, have a look at the code, it works for me. One remark though: the utility does not seem to work when you use groovyBC for your temperature boundary conditions. It does not crash, but the resulting wall heat flux will not be correct. In case you want to use this utility in combination with groovyBC, you have to edit your results file T and change all groovyBC bc's into fixedValues (while leaving the non-uniform list of temperature at the wall as generated by groovyBC). Then the generated heatflux will be correct. Eelco |
Quote:
|
I use groovyBC for the temperature (required for the heatFlux utility) only for setting gradients (for imposing either the wall heatflux or a heat transfer coeffcient). Is this possible via a non-mixed BC as well?
I noticed that all utilities (also the ones coming with OF) do not handle groovyBC correctly. A quick way for me to work around is is to change all type groovyBC; lines to type fixedValue;; using two ;;, such you can change it back easily. Use sed to do it quickly sed -ie 's/groovyBC/fixedValue;/' `find [0-9]* -name T` wallHeatFluxIncompressible sed -ie 's/fixedValue;;/groovyBC;/' `find [0-9]* -name T` Let me know if you want to report the bug on Mantis. eelco |
Quote:
The problem probably is that groovyBC is not fully evaluated when being loaded. The reason is that the expression may depend on fields that are created later during startup. Also groovyBC does not force the loading of fields because it expects all fields to be in memory. Yes. Please add a bug on the Mantis. If possible add a SMALL example case with a description of the expected result ("Heatflux on patch wall should be 666") |
Quote:
Code:
evaluateDuringConstruction true; |
1 Attachment(s)
Bernard,
I just tested your suggestion. Indeed setting evaluateDuringConstruction works: the correct value is obtained for external utilities. However, I often use a field from the solver in groovyBC, for instance to use the turbulent heat diffusivity to calculate the gradT based on that. Apparently, if evaluateDuringConstruction is used, this is not allowed. If I swhich of this option the simulation runs, but erronous results for wallHeatFluxIncomressible are obtained. Replacing groovyBC with fixedValue before running wallHeatFluxIncomressible helps. I have uploaded the bug to mantis, you can get it there. But I will also upload the case here for other people to have a look at. The wall heat flux utitlity for incompressible flows is added (it does not come with OF). I noticed that it seems that there is still something wrong with the utility, because in the turbulent case the heat flux calculate is scale with a factor rho0. Perhaps the scalign with rho is done twice somehow? Do you see what goes wrong. Well anyway, perhaps there is a better workarround beside replacing groovyBC which also works with fields used in BC. Hope you can solve it Regards Eelco |
Quote:
About kappat: this is a classic chicken/egg-problem in the solver: T is constructed first, the turbulence-field later (this is the reason why the evaluation does not happen during the initialization). |
2 Attachment(s)
For those interested: Bernard fixed a bug in groovyBC so that now it is allowed to used external applications on fields which contain groovyBC boundaries.
https://sourceforge.net/apps/mantisb...iew.php?id=134 Here I am adding the test case containing and slightly improved version of WallHeatfluxIncomressible + the test case I use to set wall heat fluxed using groovyBC. If you run the case you can see that the wall heat flux imposed is now exactly 1 W/m2 (as specified by groovyBC). Good luck! Regards Eelco |
Hi eelcovv,
thanks for the utility and test case! Now I can run the test case without problem; but I met some difficulty when trying to obtain the wall heat flux. When executing WallHeatFluxIncompressible, I got: Create time Create mesh for time = 0 Time = 0 Reading field p --> FOAM FATAL IO ERROR: cannot find file file: /home/jing/OpenFOAM/jing-2.1.0/run/testCases/hotRoomGroovyBC/0/p at line 0. From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73. Then I checked the /0 folder; there is only p_rgh rather than p there. I checked out some old threads but am still confused. Would you give me a hint on how to get an initial p file? I'm very new to openFoam and have been learning from the forum. Thanks in advance for the help! Best regards, Jing |
1 Attachment(s)
Hi Jing,
The solver buoyantBoussinesqSimpleFoam uses p_rgh which is p minus the hydrostatic pressure rho*g*height. p is only later calculated and generated by the solver. So in the 0 directory it is not present yet, that's why the utility stops, because it apparently needs it. I you realy want to calculate the heat flux at time 0 (which does not make sense because the temperature field still needs to be calculated) then you can copy p_rgh to p. I actually realise that the pressure is not required for calculating the heat flux, so you can also comment out the lines in the utility that read the pressure. I checked and it works. See the new version. p is now not required anymore. Regards Eelco |
This is probably a really dumb question, but before I mess something up by attempting to add this, I wanted to double check I was doing it correctly. I've unpacked the file and placed it in the OpenFOAM-2.1.1/applications/utilities/postProcessing/wall directory. What should happen next?
(I apologize. I'm new to OpenFOAM, CFD, and C++. I'd really appreciate the help!) |
Quote:
Unpack the the folder into your Openfoam Folder so that you have a structure like /home/user/OpenFOAM/user-2.1.1/wallHeatFluxIncompressible where user is your username. Then navigate into this folder on a terminal and just run wmake in that directory. After a short while you have a working wallHeatFluxIncompressible utility that you can use. If you can't call it in the terminal, just re source your .bashrc or just start a new terminal. This description assumes that you installed OpenFOAM through the sources and carried out all required steps as described in http://www.openfoam.org/download/ubuntu.php |
Many thanks to Eelco for the incompressible heat flux utility.
Saved my rear. Be aware you may have to set tolerances very tightly to get steady state heat out to equal heat in. Being converged on temperature does not mean you are converged on the wall temp gradients. Jack |
Hi eelcovv
thanks for the utility and test case! I use chtmultiregionsimplefoam solver for incompressible fluid and solid temperature is changed each time step. can i use your utility to calculate wallheatflux? would you plz help me calculate nusselt number(from wallheatflux) in this case? |
Quote:
Ed: I've coded part of the algorithm directly into the solver and it works like a charm. What is wrong with this utility then, or with OF at all, if such a utility cannot access the Temperature field of the calculated solution?! Why the same code works seamlessly when integrated into the solver? Very inconsistent. By the way Eelco, is there any particular reason you define extra volScalarField object to write heatflux data into file? Why not use readily available heatFlux surface scalar field? |
1 Attachment(s)
Hi Dear eelcovv
my case is incompressible and laminar . I have changed the wallHeatFluxIncompressible, I've compiled that but when I write wallHeatFluxIncompressible at terminal,terminal says: Code:
Create mesh for time = 0 can you help me please? i've attached my wallHeatFluxIncompressible thanks a lot. Arjang |
Hi Arjang,
OK, I found this thread, after answering to the PM you had sent me. At first, I was going to suggest that you read this thread: http://www.cfd-online.com/Forums/ope...ltiregion.html But from that error message, it looks like you didn't notice two very important details:
Bruno |
Thanks Dear Bruno :)
|
hi
Is there a example/tutorial on how to use the wallHeatFluxIncompe utility? What should be included in the wallHeatFluxDict? Thx! |
Greetings aevub,
Well... I had already mentioned in my previous post where a "wallHeatFluxDict" can be found: Quote:
This is because the one mentioned on the quoted post is for a modified version of the one in #12. As for an example case... my guess is that you can use any tutorial case that uses heat transfer and uses incompressible flow. Best regards, Bruno |
Hello,
i have an other problem with using the wallHeatFluxIncompressible tool. I'm computing a case with the buoyantBoussinesqPimpleFoam in OF 2.2 with k-w SST and wall-functions. When i'm using the tool it makes the error: --> FOAM FATAL IO ERROR: Unknown patchField type kappatJayatillekeWallFunction for patch type wall Valid patchField types are : ... Sure i can change the wall function and recompute it but is there a solution with this wall-function? thanks |
Greetings to all!
I've created a git repo for the utility wallHeatFluxIncompressible by Eelco van Vliet: https://github.com/wyldckat/wallHeatFluxIncompressible In addition, I've adapted the code to work with OpenFOAM 2.2.x and 2.3.x. Note: When using OpenFOAM 2.2.0, you should use the code that is meant for OpenFOAM 2.1.x, because the field names in 2.2.0 are still using the old field naming convention "kappat" and "kappaEff", while 2.2.1 and above use "alphat" and "alphaEff". @Chris: I don't know if you've managed to solve the problem you had, but if you're using OpenFOAM 2.2.1 or 2.2.2 or 2.2.x, then try using the code from the repository I've indicated above. Best regards, Bruno |
2 Attachment(s)
Hi all!
I have created a simple model (attached) of natural convection inside a rectangular domain. I used the wallHeatFluxIncompressible utility to check the heat flux balance. I got the expected result, 10 W/m2 were applied to wall4 as BC and 10 W/m2 are coming out wall3 which had a constant temperature BC: Quote:
Could someone explain why this is happenning? |
Quote:
Code:
surfaceScalarField heatFlux =fvc::interpolate(kappaEff*Cp0*rho0)*gradT; This is the only thing I can imagine that can explain it, but I'm pretty sure I'm not right. |
Greetings to all!
@kmargaris: From the files in the case you provided, I had to guess that you used the solver buoyantBoussinesqPimpleFoam. The answer by ssss seems to be correct. More details:
Essentially, the inverted equation implemented in the boundary condition would be this: Code:
q_ = gradient()*(Cp0*alphaEffp) I took a quick look at the compressible implementation of this boundary condition... and it's essentially the same equation, i.e.: Code:
q_/(alphaEff*thermo.Cp)
So, essentially, the problem is that the heat flux used in the boundary condition is actually "q/rho", i.e. the possibly named kinematic heat flux... Mmm... I'll report this on the bug tracker... edit: Bug reported at http://www.openfoam.org/mantisbt/view.php?id=1433 Best regards, Bruno |
@wyldckat: Thanks for the explanation and for submitting the bug report.
It seems that this bug only affects the post processing; the actual heat flux boundary condition is applied correctly in this case, right? |
Hi kmargaris,
The boundary condition is incorrect. It would only be correct if Cp0 value was in fact "Cp*rho". In other words, you can fix the problem for the boundary condition if you simply define "rho" as 1.0 and that "Cp0" is the result of "Cp*rho". Best regards, Bruno |
Dear wyldckat
@ wyldckat
hello, I tried to use your 'wallHeatFluxIncompressible' in my problem. (buoyantBoussinesqPimpleFoam with LES, oneEqEddy) (I think my result is reasonable when I comparing the temperature and velocity with literature.) Your utility was completely working and calculating wallHeatFlux! When I plot the wallHeatFlux, the trend is similar with literature, however, the magnitude is totally different. (e.g. literature: 100, my case: 0.1) Do you have any idea for this problem? I use Cp0 =1.005, rho0=1.166 Thank you |
Greetings hswzzz,
I'm sorry to say that you haven't provided enough information in order to deduce what might be wrong. Nonetheless, if I have to guess, since the discrepancy is at a scale of 1000, then my guess is that you were not careful enough with the units of the final mesh. OpenFOAM deals with metre by default and you probably planned for the mesh to be in millimetre. Best regards, Bruno |
Hi Foamers,
Sorry for restarting the thread again.i am using buoyant boussinesq simpleFoam. i have read most of the threads here how to calculate wall heat flux. now i got a question may be its dumb, I have given temprature b.c on a surface patch is it now possible to find the heat flux on this patch after the simulaion? i tired the wallheatflux command on the terminal. can somebody help me. Thank You. regards, Naresh |
Hi Bruno,
I also used the turbulentHeatFluxtemperature to specify the heat flux boundary conditions for a patch and i got unphysical result. i m using buoyantboussinesqsimpleFoam. Now i understand the reason. Thanks for the explanation. That being said is there any other posibility to specify heatFlux boundary condition for a patch? 2. i have another doubt could you please through some light on why should Cp0 should be specified as 1.0. because for TurbulenceHeatFluxTemperature B.C Cp0 is specified as 1006 though they both has the same dimensions m^2/s^2/k This is very crucial for me right now . thank you. regards, Naresh Yathuru |
Greetings Naresh,
Quote:
Usage instructions are given in post #19. Quote:
It's not "Cp0" that should be set to "1.0", it's "rho0" that should be "1.0", as already explained in post #29: Quote:
Best regards, Bruno |
Hello bruno,
thank you so much for the reply. I have read the posts you have mentioned already. and sorry if my question was not clear. My question was concerning the wallHeatfluxIncompressible. in the readme file it says the following: Modified version of wallHeatFlux based on suggestion of to change combustion flow to normal flows http://www.cfd-online.com/Forums/ope...ance-flow.html I replaced the createField with the boussinesqSimpleFoam In this version it is required to specify values for the density, heat capacity, and Prandtl numbers in the transportProperties dictionary like Code:
// Laminar Prandtl number may be this is a silly question could you tell me please which value should i use for cp0 and rho0 when i use turbulentwallheatFlux B.C and if i m using the wallheatfluxincompressible utility to find the flux on the patches. should i use Cp0 = 1.0 or 1005. Thank you, regards, Naresh |
Hi Naresh,
Quote:
In other words, if you don't indicate how your case was originally created and defined, I don't know how is should be handled at the end of the simulation. Best regards, Bruno |
Quote:
Code:
dimensions [0 0 0 1 0 0 0]; and this how i specified my transport properties Quote:
when i use turbulentHeatFluxtemperature boundary condition i specify cp0 as 1005. but according to the read me file in the wallheatfluxincompressible it says Quote:
i m a little confused. Thank you Regards, Naresh |
Hi Eelcovv
Can you please suggest how to use the "wallHeatFluxIncompressible" utilty file. I mean is it like just cope paste the files to the respective directory and than running the utility command from the terminal will work?? Warm regards Gautam |
Hi goutham,
I use it this way. I copy pase the respective files eg, GradT and other required files in the 0 folder before starting the simulation. after the simulation is done u can type wallHeatfluxTemperature and the patchname in yout terminal . it is basically a post processing utility. i assume u already installed the wallHeatFluxIncompressible utility successfully and checked . All the best. Naresh |
Hi Naresh
Thanks for your reply. I just downloaded the zipfile given in this thread. After that I am not understanding if to copy the folder to "/applications/utilities" or some other steps to follow. Please help me. Thanking you Gautam |
All times are GMT -4. The time now is 08:35. |