
[Sponsors] 
August 26, 2013, 12:41 
energy equation for porousSimpleFoam

#1 
Senior Member
mohsen kh
Join Date: Jan 2013
Location: Iran
Posts: 125
Rep Power: 12 
Hi dear foamers
I do not know how to add an energy equation to my solver (porousSimpleFoam).my flow is incompressible and I do not know how to add TEqn.H to my own solver.what should I do with (rho of fluid, Cp of it and also Sigma,k and q"') ? while the equation the equation is something like this: rho(fluid)*Cp(fluid)[sigma dt/dt + Udt/dx]=k d2T/dx2 + q'" + (mu/K) u^2 Sigma = [porosity(rho*cp)f+(1porosity)*(rhoc)s]/(rho*cp)f q"' = (1 porosity) q'"s k= (porosity*kf) + (1 porosity)*ks please help me. fvScalarMatrix TEqn ( fvm::ddt(T) +fvm::div(phi,T) fvm::laplacian(alpha,T) ); TEqn.solve(); what should I do with these kf,ks,.... how and where should I define them? Just right them in transportProperties in constant folder? Best regards Mohsen 

August 31, 2013, 00:50 
energy equation for porousSimpleFoam

#2 
Senior Member
mohsen kh
Join Date: Jan 2013
Location: Iran
Posts: 125
Rep Power: 12 
hi dear Foamers
has anyone write this equation for his/her solver? I need emergent help in this case. I understand how to define my porous zone I want to add the energy equation to my solver I did it but didn't work I am here to ask you if you would help me or not I'm looking forward to your reply my friend I hope you can help me by your useful comments my equation is something like this rho(fluid)*Cp(fluid)[sigma dT/dt + UdT/dx]=k d2T/dx2 + q'" + (mu/K) u^2 Sigma = [porosity(rho*cp)f+(1porosity)*(rhoc)s]/(rho*cp)f q"' = (1 porosity) q'"s k= (porosity*kf) + (1 porosity)*ks I also don't know how and where to define sigma,k... best regards Mohsen 

August 31, 2013, 09:04 

#3 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 125 
Greetings Mohsen,
Have a look into the solver rhoPorousSimpleFoam. The source code for it is located at "applications/solvers/compressible/rhoSimpleFoam/rhoPorousSimpleFoam/". You can see the full path to it by running: Code:
echo $FOAM_SOLVERS/compressible/rhoSimpleFoam/rhoPorousSimpleFoam/ Or you can modify this equation to work the other way around, namely to solve the temperature and then calculate whatever else is needed. Good luck! Best regards, Bruno
__________________


August 23, 2019, 03:57 

#4 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi all,
I am also working with same condition as yours. Now i am moving to heat transfer problem with porous media. May i know how to add energy equation with porousSimpleFoam solver case?? Thanks in advance, Vishsel 

August 25, 2019, 08:53 

#5 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 125 
Quick answer: In the current/modern OpenFOAM solvers, you can add porous mediums on any solver, without the need to modify the solver. See for example: https://openfoamwiki.net/index.php/DarcyForchheimer
__________________


August 26, 2019, 01:56 

#6 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi Bruno,
Thank you for your reply. Actually my case is HX which has solid parts and fluid domains. I need to find out heat transfer, for that i need to include energy equation to porousSimpleFoam solver(my case). How can i add energy equation to my case?? And How to create heat source in openfoam for my case?? Thank you, Vishsel 

August 26, 2019, 22:12 

#8 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi bruno,
I am using openfoam 2.3 version. I need to apply a heat source at wall BC and to see the distribution of heat. Last edited by Vishsel; August 27, 2019 at 03:42. 

August 27, 2019, 19:03 

#9 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 125 
Quick answer: In OpenFOAM 2.3 you have the tutorial case "heatTransfer/chtMultiRegionSimpleFoam/heatExchanger" and demonstrates what you want to do, namely having heat exchange and a porous region.


August 28, 2019, 02:07 

#10 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi bruno,
Thank you for your reply. Thank you in advance Vishsel Last edited by Vishsel; August 30, 2019 at 00:53. 

August 29, 2019, 09:33 

#11 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi bruno,
Thank you for your reply. Actually my need is to generate a heat at surface (i.e @solid wall BC). I have an input like heat flux value, heat generation value in W and how can i give heat flux or heat generation value in fvOptions file. And I have an another doubt, for my case whether i have to use type 1)scalarSemiImplicitSource (or) 2)externalWallHeatFluxTemperature in fvOptions and what are all the changes in fvSchemes & fvSolution files ??And this is my fvOptions file and values 50,137.5 are in watts Code:
walldp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (50 0); } } } walldp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (50 0); } } } wallmp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (137.5 0); } } } wallmp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (137.5 0); } } } Code:
Creating finite volume options from fvOptions Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 No MRF models present Creating porosity model list from porosityProperties Porosity region fturbo: selecting model: DarcyForchheimer creating porous zone: fturbo Using pressure explicit porosity Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.000941837, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.000384228, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.000471979, No Iterations 2 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0245239, No Iterations 11 time step continuity errors : sum local = 0.00735485, global = 9.97032e005, cumulative = 9.97032e005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e005, No Iterations 2 smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.00172232, No Iterations 2 ExecutionTime = 24.492 s ClockTime = 25 s Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss upwind; div(phi,h) bounded Gauss upwind; div(phi,e) bounded Gauss upwind; div(phi,Ekp) bounded Gauss upwind; div(phi,K) bounded Gauss upwind; div(phi,k) bounded Gauss upwind; div(phi,epsilon) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; laplacian(alpha,h) Gauss linear uncorrected; } interpolationSchemes { default linear; } snGradSchemes { default uncorrected; } fluxRequired { default no; p ; } Code:
solvers { p { solver GAMG; tolerance 1e08; relTol 0.05; smoother GaussSeidel; cacheAgglomeration on; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; } "(Ukepsilon)" { solver smoothSolver; smoother symGaussSeidel; nSweeps 2; tolerance 1e07; relTol 0.1; } h { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.1; minIter 1; } } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { fields { p 0.7; } equations { U 0.3; h 0.3; k 0.3; epsilon 0.3; } } Is it correct?? if it is wrong please correct me.. Thank you in advance Vishsel 

August 30, 2019, 05:55 

#12  
Member
Priyanka P
Join Date: Apr 2019
Location: Germany
Posts: 40
Rep Power: 4 
Quote:
Code:
volumeMode specific; // absolute; To calculate the value of 'h' you must divide the total volume where you want to apply this heat to the power in watts. for example: for your Code:
wall dp 1 Code:
0.000333435 Code:
p(W)/volume i.e. 50,137.5 (in watts)/0.000333435 3. You don't really have to change anything in fvschemes and fvSolution for now and changes in fvSolution depends on your mesh quality etc. I also dont have much knowledge about different schemes and solvers. I can only help you with those that I have used so far. Hope it helps! 

August 30, 2019, 06:49 

#13 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi,
Thankyou so much for your reply. I am getting this error while running. Why iam getting this error?? Code:
Creating finite volume options from fvOptions Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 No MRF models present Creating porosity model list from porosityProperties Porosity region fturbo: selecting model: DarcyForchheimer creating porous zone: fturbo Using pressure explicit porosity Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.000941837, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.000384228, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.000471979, No Iterations 2 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0245239, No Iterations 11 time step continuity errors : sum local = 0.00735485, global = 9.97032e005, cumulative = 9.97032e005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e005, No Iterations 2 smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.00172232, No Iterations 2 ExecutionTime = 24.186 s ClockTime = 24 s Time = 2 > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp2 defined for field h but never used smoothSolver: Solving for Ux, Initial residual = 0.198925, Final residual = 0.000183157, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.419724, Final residual = 0.000232691, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.562048, Final residual = 0.000382205, No Iterations 2 GAMG: Solving for p, Initial residual = 0.679735, Final residual = 0.027343, No Iterations 3 time step continuity errors : sum local = 1.36223, global = 0.0140221, cumulative = 0.0139224 smoothSolver: Solving for epsilon, Initial residual = 0.0114781, Final residual = 1.76928e005, No Iterations 2 bounding epsilon, min: 98.6398 max: 65049.1 average: 526.345 smoothSolver: Solving for k, Initial residual = 0.581875, Final residual = 0.000814592, No Iterations 2 ExecutionTime = 38.45 s ClockTime = 38 s Code:
FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // wallmp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wallmp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } walldp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } walldp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } wallmp1 { type scalarCodedSource; active true; selectionMode all; scalarCodedSourceCoeffs { name sourceTime; fieldNames (h); codeInclude #{ #}; codeCorrect #{ Pout<< "**codeCorrect**" << endl; #}; codeAddSup //major problem under this #{ const volScalarField& Tm = mesh_.lookupObject<volScalarField>("T"); Tvol = Tm.weightedAverage(mesh_.V()).value(); //averageValue of the volScalarField const vectorField& C = mesh_.C(); //List of cellcentres const scalarField& V = mesh_.V(); scalarField& hSource = eqn.source(); //defining source forAll(C, i) { hSource[i] = ???? ; // May i know how to write the hSource?? } Pout << "***codeAddSup***" << endl; #}; codeSetValue #{ Pout<< "**codeSetValue**" << endl; #}; // Dummy entry. Make dependent on above to trigger recompilation code #{ $codeInclude $codeCorrect $codeAddSup $codeSetValue #}; } sourceTimeCoeffs { $scalarCodedSourceCoeffs; } } Thankyou in advance Vishnu Last edited by Vishsel; August 30, 2019 at 09:58. 

August 30, 2019, 09:31 

#14 
Member
Priyanka P
Join Date: Apr 2019
Location: Germany
Posts: 40
Rep Power: 4 
What is wall mp 1 , wall dp 1 etc in your case?
And where are you defining it? 

August 30, 2019, 09:53 

#15 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi,
Those are all the boundary surface.. i need to generate the heat source on that surface of the wall wallmp1 wallmp2 walldp1 walldp2 

September 2, 2019, 05:10 

#16 
Member
Priyanka P
Join Date: Apr 2019
Location: Germany
Posts: 40
Rep Power: 4 
I have only generated heat source on a body, but as far as I know to generate heat source on the surface you can directly assign the heat source on that particular surface as below:
Code:
heatSource { type scalarSemiImplicitSource; active true; scalarSemiImplicitSourceCoeffs { selectionMode all; // all, // cellZone hot; // Use this create hea source on a particular region //cellSet c1; // you can define a faceSet and use cellSet for a surface volumeMode specific; // absolute; injectionRateSuSp { h (46428571.43 0); } } } 

September 3, 2019, 06:07 

#17 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Hi all,
Thankyou for your solution. @priyanka But still i am getting this error. And solver for ''h'' is not running. Code:
Creating finite volume options from fvOptions Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wallmp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp1  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: walldp2  applying source for all time  selecting all cells  selected 5338536 cell(s) with volume 0.000333435 No MRF models present Creating porosity model list from porosityProperties Porosity region fturbo: selecting model: DarcyForchheimer creating porous zone: fturbo Using pressure explicit porosity Starting time loop Time = 1 smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 0.000941837, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 0.000384228, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 1, Final residual = 0.000471979, No Iterations 2 GAMG: Solving for p, Initial residual = 1, Final residual = 0.0245239, No Iterations 11 time step continuity errors : sum local = 0.00735485, global = 9.97032e005, cumulative = 9.97032e005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e005, No Iterations 2 smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.00172232, No Iterations 2 ExecutionTime = 24.831 s ClockTime = 25 s Time = 2 > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wallmp2 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp1 defined for field h but never used > FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source walldp2 defined for field h but never used smoothSolver: Solving for Ux, Initial residual = 0.198925, Final residual = 0.000183157, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.419724, Final residual = 0.000232691, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.562048, Final residual = 0.000382205, No Iterations 2 GAMG: Solving for p, Initial residual = 0.679735, Final residual = 0.027343, No Iterations 3 time step continuity errors : sum local = 1.36223, global = 0.0140221, cumulative = 0.0139224 smoothSolver: Solving for epsilon, Initial residual = 0.0114781, Final residual = 1.76928e005, No Iterations 2 bounding epsilon, min: 98.6398 max: 65049.1 average: 526.345 smoothSolver: Solving for k, Initial residual = 0.581875, Final residual = 0.000814592, No Iterations 2 ExecutionTime = 39.094 s ClockTime = 39 s Time = 3 smoothSolver: Solving for Ux, Initial residual = 0.0770133, Final residual = 1.89677e005, No Iterations 2 smoothSolver: Solving for Uy, Initial residual = 0.244463, Final residual = 0.000106983, No Iterations 2 smoothSolver: Solving for Uz, Initial residual = 0.258733, Final residual = 0.000281965, No Iterations 2 GAMG: Solving for p, Initial residual = 0.692126, Final residual = 0.0184881, No Iterations 3 time step continuity errors : sum local = 0.745246, global = 0.0381094, cumulative = 0.0520318 smoothSolver: Solving for epsilon, Initial residual = 0.00822483, Final residual = 1.47114e005, No Iterations 2 smoothSolver: Solving for k, Initial residual = 0.147117, Final residual = 0.00022013, No Iterations 2 ExecutionTime = 53.177 s ClockTime = 53 s Code:
wallmp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wallmp1surface; cellSet wallmp1; volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wallmp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wallmp2surface; cellSet wallmp2; volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } walldp1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone walldp1surface; cellSet walldp1; volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } walldp2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone walldp2surface; cellSet walldp2; volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } Code:
actions ( { name wallmp1surface; type faceSet; action new; source patchToFace; sourceInfo { name wallmp1; } } { name wallmp2surface; type faceSet; action new; source patchToFace; sourceInfo { name wallmp2; } } { name walldp1surface; type faceSet; action new; source patchToFace; sourceInfo { name walldp1; } } { name walldp2surface; type faceSet; action new; source patchToFace; sourceInfo { name walldp2; } } { name wallmp1CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wallmp1surface; option any; } } { name wallmp2CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wallmp2surface; option any; } } { name walldp1CellSet; type cellSet; action new; source faceToCell; sourceInfo { set walldp1surface; option any; } } { name walldp2CellSet; type cellSet; action new; source faceToCell; sourceInfo { set walldp2surface; option any; } } ); Thanks in advance, Vishnu Last edited by Vishsel; September 4, 2019 at 02:58. 

September 3, 2019, 07:06 

#18 
Member
Priyanka P
Join Date: Apr 2019
Location: Germany
Posts: 40
Rep Power: 4 
I just recalled this,
You want to give power as an input to generate heat on your surfaces wallmp1 wallmp2 walldp1 walldp2 Right? If yes, then as far as I know you can not give power as input to a surface. Power can only be given as an input to a volume which means to a cellZone. you can give temperature as input to surfaces but not power because it is a volumetric identity. But maybe you can take opinion from others as I am also not very experienced in OpenFoam. 

September 3, 2019, 08:18 

#19 
Member
Vishnu
Join Date: May 2019
Location: Tamilnadu, India
Posts: 55
Rep Power: 4 
Thank you for your reply.
I have an input like heat flux (W/m2) and heat generation (W). I have taken volume value from Code:
 selected 5338536 cell(s) with volume 0.000333435 But my case was to generate an heat at surface(@wall). Is it possible to give heat flux (W/m2) and heat generation (W) value as an input ??? Last edited by Vishsel; September 3, 2019 at 09:32. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
energy equation in rhoCentralFoam  nakul  OpenFOAM  0  October 10, 2010 16:07 
Pohlhausen energy equation MATLAB help  abe_cooldude  Main CFD Forum  2  May 3, 2010 17:58 
SIMPLE and energy equation convergence  Fabio  Main CFD Forum  0  June 1, 2007 07:06 
How to discretize of energy equation ??  Asghari  FLUENT  0  October 12, 2006 09:09 
energy equation formulation  Pedro  Phoenics  1  July 5, 2001 13:17 