|
[Sponsors] |
March 31, 2015, 18:07 |
|
#21 |
New Member
Join Date: Nov 2014
Posts: 3
Rep Power: 12 |
Hello alexeym,
I am trying to implement a source term for turbulent dissipation in a simulation using the standard k-epsilon model following your explanation about the scalarCodedSource. I ended up with this fvOptions file (where there is also a source for the momentum equation): Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.3.0 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // momentumSource { type vectorSemiImplicitSource; selectionMode cellZone; cellZone disk; active true; vectorSemiImplicitSourceCoeffs { volumeMode absolute; injectionRateSuSp { U ((0 0 -180e3) 0); } } } dissipationSource { type scalarCodedSource; selectionMode cellZone; cellZone disk; active true; scalarCodedSourceCoeffs { fieldNames (epsilon); redirectType sourceTime; codeInclude #{ #}; codeCorrect #{ Pout<< "**codeCorrect**" << endl; #}; codeAddSup #{ const Time& time = mesh().time(); const scalarField& V = mesh_.V(); const vectorField& C = mesh_.C(); const scalarField& nut_ = nut(); const vectorField& U_ = U(); const scalarField& k_ = k(); const scalarField& Pt = nut_*2*magSqr(symm(fvc::grad(U_))); scalarField& epsilonSource = eqn.source(); forAll(C, i) { epsilonSource[i] -= 0.37*Pt[i]*Pt[i]/k_[i]*V[i]; } Pout << "***codeAddSup***" << endl; #}; codeSetValue #{ Pout<< "**codeSetValue**" << endl; #}; // Dummy entry. Make dependent on above to trigger recompilation code #{ $codeInclude $codeCorrect $codeAddSup $codeSetValue #}; } sourceTimeCoeffs { // Dummy entry } } // ************************************************************************* // Code:
--> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source dissipationSource defined for field epsilon but never used Thanks |
|
April 1, 2015, 02:50 |
|
#22 |
Senior Member
|
Hi,
My advice: implement your own turbulence model I.e. you take k-epsilon family model, copy it, rename it, add your code. There are certain conditions for fvOptions to work, see, for example, UEqn.H of pimpleFoam: Code:
tmp<fvVectorMatrix> UEqn ( fvm::ddt(U) + fvm::div(phi, U) + turbulence->divDevReff(U) == fvOptions(U) ); UEqn().relax(); fvOptions.constrain(UEqn()); During last workshop there was an idea of implementation of turbulence models, which use fvOptions framework. I do not know if there is any progress, for me it is still on TODO list. |
|
April 28, 2015, 06:36 |
fvOptions heatsource in chtmultiregionsimpleFoam case in openfoam2.3.x
|
#23 |
New Member
Sandeep Rapol
Join Date: Feb 2015
Posts: 11
Rep Power: 11 |
Hello everyone
I am implementing volumetric heat source in chtmultiregionsimplefoam with help of fvoptions files in that "duration ....." and " h(.... 0)" so my problem is 1) how to convert 200 W source into enthalpy h(... 0) with help of "duration ...." in sec 2) in that "fvOptions" file "duration..." so which time put here in duration |
|
April 28, 2015, 06:49 |
|
#24 | |
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
Quote:
1) You don't need to convert nothing into nothing. For the case of using chtMultiRegionSimpleFoam you just have to put the thermal power value into the first place within the brackets, like that: Code:
energySource { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode absolute;//specific;// injectionRateSuSp { h (q 0); // q in [W]; or in [W/m³] if you use specific mode } } } Hope it helps. Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! |
||
April 28, 2015, 07:03 |
|
#25 | |
Senior Member
|
@faraday
Quote:
Code:
inline bool Foam::fv::option::inTimeLimits(const scalar time) const { return ( (timeStart_ < 0) || ( (mesh_.time().value() >= timeStart_) && (mesh_.time().value() <= (timeStart_ + duration_)) ) ); } Code:
bool Foam::fv::option::isActive() { if (active_ && inTimeLimits(mesh_.time().value())) { --- return true; } else { return false; } } |
||
April 28, 2015, 07:10 |
|
#26 |
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
Thanks for the clarification Alexey! I didn't remember that because I never had to specify the duration of the source.
Everything must be clear now for @Sandeep.
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! |
|
April 28, 2015, 08:42 |
fvOptions heatsource in chtmultiregionsimpleFoam case in openfoam2.3.x
|
#27 |
New Member
Sandeep Rapol
Join Date: Feb 2015
Posts: 11
Rep Power: 11 |
hello alex,
thank you for the replay , I used that syntax in fvOptions file but result showing no heat generation, it shows constant temperature when I use my fvOptins that showing heat generation it include "duration....." of time -------#---------------------------#-----------------------------#-------------------- heatSource { type scalarSemiImplicitSource; active on; timeStart 0.; duration 1e3; selectionMode cellSet; cellSet IC1; scalarSemiImplicitSourceCoeffs { // volumeMode absolute; // Values are given as <quantity> volumeMode specific; // Values are given as <quantity>/m3 injectionRateSuSp // Semi-implicit source term S(x) = S_u + S_p x { h (200000 0); } } } --------------------#--------------------------------#-----------------------#------------------#--- am trying to implement 200 W/m3 volumetric heat generating source for circuit board cooling |
|
April 28, 2015, 09:09 |
|
#28 |
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
Well, I don't understand why my specification is not working. As per what I see you are using a cellSet as a selection mode, while I sellect all cells belonging to one region. If you just copypasted all my specification of course it's not going to work...
Another point I don't get is why you are setting a generation of 200000 when you say your generation is supposed to be of 200 W/m2... If you give a higher value than the one you need, obviously the effect will be more visual and bigger... Regards, Alex Ps: excuse me if I wrote something wrong, I'm writing from my phone
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! |
|
April 29, 2015, 08:01 |
|
#29 |
New Member
Sandeep Rapol
Join Date: Feb 2015
Posts: 11
Rep Power: 11 |
hello alex,
you are on the right way you see in src/fvOptios/lninclude/fvOptionListTemplates.C at line no 135 ds = rho.dimensions()*fld.dimensions()/dimTime*dimVolume rho * h *1/time * vol kg/m3 * j/kg * m3 / sec j/s W so here is dimTime in sec plese tell me how to implement 200 W/m3 heat generating source |
|
April 29, 2015, 08:47 |
|
#30 |
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
check this out!
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! |
|
April 30, 2015, 07:25 |
|
#31 |
New Member
Sandeep Rapol
Join Date: Feb 2015
Posts: 11
Rep Power: 11 |
hello alex
thank you for your humble reolay in fvoptions volumeMode absolute; // Values are given as <quantity> volumeMode specific; // Values are given as <quantity>/m3 what is "absolute" and "specific" if my heat generating element is 200 W having dimension 0.2m*0.01m*0.05m 1) if I consider "absolute" then total element given value is 200 W is this correct or not? 2) if I consider "specific" then total element each cell point given value is 200 W is this correct or not? |
|
April 30, 2015, 08:40 |
|
#32 |
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 |
Dear Sandeep,
the meaning of "absolute" and "specific" is given behind "//". Then, if you consider "absolute" mode you just have to give the constant source term a value of 200. On the other hand, if you prefer to use "specific" mode you have to use a value of 200/(0.2*0.01*0.05). That's all! Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! |
|
May 4, 2015, 05:49 |
|
#33 |
New Member
Sandeep Rapol
Join Date: Feb 2015
Posts: 11
Rep Power: 11 |
thank you alex,
which parameter analyze in post processing.I thought that only temp of oullet, & velocity is analyze in chtmultiregionSimpleFoam and chtmultiRegionFoam please suggest me |
|
May 11, 2015, 15:08 |
|
#34 |
New Member
Join Date: Nov 2014
Posts: 3
Rep Power: 12 |
Hi,
I would like to follow up my previous post regarding the implementation of a source term for the turbulent dissipation rate with scalarCodedSource. I eventually implemented my own turbulence model of the k-epsilon family. This is the main modification which takes into account the possible source term: Code:
// Dissipation equation tmp<fvScalarMatrix> epsEqn ( fvm::ddt(epsilon_) + fvm::div(phi_, epsilon_) - fvm::laplacian(DepsilonEff(), epsilon_) == C1_*G*epsilon_/k_ - fvm::Sp(C2_*epsilon_/k_, epsilon_) + fvOptions(epsilon_) ); epsEqn().relax(); fvOptions.constrain(epsEqn()); epsEqn().boundaryManipulate(epsilon_.boundaryField()); solve(epsEqn); fvOptions.correct(epsilon_); bound(epsilon_, epsilonMin_); S = 0.37 G^2 / k where G is the the generation of turbulent kinetic energy computed in the sandard k-epsilon model and k is the turbulent kinetic energy. In order to do this, I added the following piece of code to fvOptions: Code:
dissipationSource { type scalarCodedSource; selectionMode cellZone; cellZone diss; active true; scalarCodedSourceCoeffs { fieldNames (epsilon); redirectType sourceTime; codeInclude #{ #include "fvCFD.H" #}; codeCorrect #{ Pout<< "**codeCorrect**" << endl; #}; codeAddSup #{ const scalarField& V = mesh_.V(); const vectorField& C = mesh_.C(); const volScalarField& nut = mesh().lookupObject<volScalarField>("nut"); const volVectorField& U = mesh().lookupObject<volVectorField>("U"); const volScalarField& k = mesh().lookupObject<volScalarField>("k"); const volScalarField& G = nut*2*magSqr(symm(fvc::grad(U))); // as computed in the k-epsilon model scalarField& epsilonSource = eqn.source(); forAll(C,i) { epsilonSource[i] -= 0.37*G[i]*G[i]/k[i]; } Pout << "***codeAddSup***" << endl; #}; codeSetValue #{ Pout<< "**codeSetValue**" << endl; #}; // Dummy entry. Make dependent on above to trigger recompilation code #{ $codeInclude $codeCorrect $codeAddSup $codeSetValue #}; } sourceTimeCoeffs { // Dummy entry } } Can you see any errors in the code? Thanks |
|
September 8, 2016, 15:40 |
|
#35 |
Senior Member
Nima Samkhaniani
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,267
Blog Entries: 1
Rep Power: 25 |
Dear Alex
How to set multiple discrete heat sources using scalarSemiImplicitSource ?
__________________
My Personal Website (http://nimasamkhaniani.ir/) Telegram channel (https://t.me/cfd_foam) |
|
January 3, 2017, 12:24 |
what for solver using EEqn.C?
|
#36 | |
Senior Member
|
Quote:
just a clarification for buoyantSimpleFoam. This solver uses EEqn.C file, so you have to specify the thermal model. In case you set the following dict for thermophysicalProperties Code:
{ type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } but if you consider a fluid with Cp = 4.186kJ/(kg*K) and rho = 1000 kg/m3, if you want to have 1W/m3 you have to set h value (q parameter [specific] ) equal to 0,000000239 Code:
q = Q = rho*Cp*T/t ==> 1/1000/4186 Last edited by student666; January 3, 2017 at 13:36. |
||
January 4, 2017, 18:38 |
|
#37 |
Senior Member
|
I performed this simple test case.
3D simulation. All patches have been set to "walls"(T=293K), but patch named "fondo" has been set to zeroGradient for T. cellZone "c0" , at the bottom (coord z=0), has 500W power source. laminar. simulation performed with openFoam v4.1 run Code:
blockMesh topoSet renumberMesh -overwrite buoyantPimpleFoam > log.1 Code:
wallHeatFlux Code:
Time = 2.554868161131 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 laminar Wall heat fluxes [W] pareti convective: -497.79226 radiative: -0 total: -497.79226 fondo convective: 0 radiative: -0 total: 0 Time = 2.9167083871732 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 laminar Wall heat fluxes [W] pareti convective: -498.87276 radiative: -0 total: -498.87276 fondo convective: 0 radiative: -0 total: 0 Time = 3.27661601896623 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 laminar Wall heat fluxes [W] pareti convective: -499.42118 radiative: -0 total: -499.42118 fondo convective: 0 radiative: -0 total: 0 End Regards. |
|
February 14, 2017, 03:37 |
|
#38 |
New Member
Join Date: Dec 2016
Posts: 10
Rep Power: 9 |
Hello,
I'm trying to implement a volumetric source with scalarCodedSource. At the surface the equation: q=q0 * e^(re^2/r^2) In the depth the value q0 is described with functions. I'm using Openfoam 4.1 and the solver buoyantBoussinesqSimpleFoam. After calling the function I get this: Code:
Creating finite volume options from "constant/fvOptions" --> FOAM FATAL ERROR: Attempt to return primitive entry ITstream : /home/cfd/OpenFOAM/cfd-4.1/run/elektronen/constant/fvOptions.heatSource.scalarCodedSourceCoeffs.codeInclude, line 31, IOstream: Version 2.0, format ASCII, line 0, OPENED, GOOD primitiveEntry 'codeInclude' comprises on line 31 the verbatim string "\ \ " as a sub-dictionary From function virtual const Foam::dictionary& Foam::primitiveEntry::dict() const in file db/dictionary/primitiveEntry/primitiveEntry.C at line 189. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::primitiveEntry::dict() const at primitiveEntry.C:? #3 Foam::dictionary::substituteScopedKeyword(Foam::word const&) at ??:? #4 Foam::entry::New(Foam::dictionary&, Foam::Istream&) at ??:? #5 Foam::dictionary::read(Foam::Istream&, bool) at ??:? #6 Foam::dictionary::dictionary(Foam::fileName const&, Foam::dictionary const&, Foam::Istream&) at ??:? #7 Foam::dictionaryEntry::dictionaryEntry(Foam::keyType const&, Foam::dictionary const&, Foam::Istream&) at ??:? #8 Foam::entry::New(Foam::dictionary&, Foam::Istream&) at ??:? #9 Foam::dictionary::read(Foam::Istream&, bool) at ??:? #10 Foam::dictionary::dictionary(Foam::fileName const&, Foam::dictionary const&, Foam::Istream&) at ??:? #11 Foam::dictionaryEntry::dictionaryEntry(Foam::keyType const&, Foam::dictionary const&, Foam::Istream&) at ??:? #12 Foam::entry::New(Foam::dictionary&, Foam::Istream&) at ??:? #13 Foam::dictionary::read(Foam::Istream&, bool) at ??:? #14 Foam::dictionary::dictionary(Foam::fileName const&, Foam::dictionary const&, Foam::Istream&) at ??:? #15 Foam::dictionaryEntry::dictionaryEntry(Foam::keyType const&, Foam::dictionary const&, Foam::Istream&) at ??:? #16 Foam::entry::New(Foam::dictionary&, Foam::Istream&) at ??:? #17 Foam::dictionary::read(Foam::Istream&, bool) at ??:? #18 Foam::operator>>(Foam::Istream&, Foam::dictionary&) at ??:? #19 Foam::IOdictionary::readFile(bool) at ??:? #20 Foam::IOdictionary::IOdictionary(Foam::IOobject const&) at ??:? #21 Foam::fv::options::options(Foam::fvMesh const&) at ??:? #22 Foam::fv::options::New(Foam::fvMesh const&) at ??:? #23 ? at ??:? #24 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #25 ? at ??:? Abgebrochen (Speicherabzug geschrieben) My fvOption-file looks like this: Code:
heatSource { type scalarCodedSource; active true; selectionMode all; scalarCodedSourceCoeffs { fieldNames (T); name sourceTime; codeInclude #{ #}; codeCorrect #{ Pout<< "**codeCorrect**" << endl; #}; codeAddSup #{ scalarField& TSource = eqn.source(); //Values for checking the equations const scalar power = 1000; const scalar Radius = 0.5; const scalar rho = 1000; const scalar Cp = 4.19; const scalar xCenter = 3; const scalar yCenter = 0.01; const scalar zCenter = 2; // Equations // -Face centers const List<point>& cf = p.Cf(); const scalar xCF = cf[c][0]; const scalar XF = xCenter - xCF; const scalar check+ = xCenter + Radius; const scalar check- = xCenter - Radius; if ((xCF < check+) && (xCF > check-)) { const scalar r2 = XF * XF; const scalar re2 = Radius * Radius; const scalar factor = r2/re2; const scalar pre = exp(factor); const scalar qfa_ [c] = power * exp; const scalar TzuF_ [c] = (1/(rho*Cp))*qfa } else { const scalar qfa_ [c] = 0; }; // -Depth centers or cell centers TSource -= Tzuf; Pout << "***codeAddSup***" << endl; #}; codeSetValue #{ Pout<< "**codeSetValue**" << endl; #}; // Dummy entry. Make dependent on above to trigger recompilation code { $codeInclude $codeCorrect $codeAddSup $codeSetValue }; } sourceTimeCoeffs { // Dummy entry } } regards Chris |
|
February 14, 2017, 05:53 |
|
#39 |
Member
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 13 |
Hi Chris,
I'm not too much into the scalarCodedSource fvOptions but just by looking at the error message it tells you that on line 31 of your code something is going wrong. More precisely it is in the section codeInclude (I suppose that is line 31 when looking at the entiere fvOptions file including its header. This section supposedly must be filled and cannot be left blank. As I'm not familiar with this tool I can't help you any further but maybe it helps. Regards Hannes |
|
February 14, 2017, 06:42 |
|
#40 |
New Member
Join Date: Dec 2016
Posts: 10
Rep Power: 9 |
Thanks for your reply.
I look into this. |
|
Tags |
fvoptions, heat source, scalarcodedsource |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
OpenFoam 2.2 fvOptions temperature limits | fredo490 | OpenFOAM Running, Solving & CFD | 12 | January 17, 2020 00:59 |
Building a solver with fixedTemperatureConstraint using fvOptions | Fluido | OpenFOAM Programming & Development | 9 | February 15, 2018 01:30 |
How to set fvOptions | yurifrey | OpenFOAM Pre-Processing | 5 | February 22, 2016 19:14 |
[swak4Foam] Setting BC for a passive scalar (groovy vs fvOptions) | Tobi | OpenFOAM Community Contributions | 0 | May 23, 2013 15:53 |
A new Howto on the OpenFOAM Wiki Compiling OpenFOAM under Unix | mbeaudoin | OpenFOAM Installation | 2 | April 28, 2006 09:54 |