# energy equation for porousSimpleFoam

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

 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+(1-porosity)*(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+(1-porosity)*(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/` This solver relies on enthalpy/energy exchanges, as solved in the file "EEqn.H". From it you can extract the current temperature from the "he" variable... although I'm not sure how exactly . 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 __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

 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 __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

 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, 17:06 #7 Retired Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,962 Blog Entries: 45 Rep Power: 125 Quick question: Which OpenFOAM version are you using?

 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: ```wall-dp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (50 0); } } } wall-dp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (50 0); } } } wall-mp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (137.5 0); } } } wall-mp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (137.5 0); } } }``` It might be wrong in fvSchemes, because solver for ''h'' is not running. Solving iterations are shown below Code: ```Creating finite volume options from fvOptions Selecting finite volume options model type scalarSemiImplicitSource Source: wall-mp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-mp-2 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-2 - 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 f-turbo: selecting model: DarcyForchheimer creating porous zone: f-turbo 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 = -9.97032e-005, cumulative = -9.97032e-005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e-005, No Iterations 2 smoothSolver: Solving for k, Initial residual = 1, Final residual = 0.00172232, No Iterations 2 ExecutionTime = 24.492 s ClockTime = 25 s``` fvSchemes 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 ; }``` fvSolution Code: ```solvers { p { solver GAMG; tolerance 1e-08; relTol 0.05; smoother GaussSeidel; cacheAgglomeration on; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; } "(U|k|epsilon)" { solver smoothSolver; smoother symGaussSeidel; nSweeps 2; tolerance 1e-07; relTol 0.1; } h { solver PCG; preconditioner DIC; tolerance 1e-06; 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:
 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.
1.if you use,

Code:
`volumeMode      specific; // absolute;`
then you must calculate the value of 'h' using your power, which I can see is your case.

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`
in the log that you have attached the volume is

Code:
`0.000333435`
so the value of h would be,

Code:
`p(W)/volume i.e.  50,137.5 (in watts)/0.000333435`
2. scalarSemiImplicitSource should be OK because that works for most of the cases in heat transfer

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: wall-mp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-mp-2 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-2 - 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 f-turbo: selecting model: DarcyForchheimer creating porous zone: f-turbo 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 = -9.97032e-005, cumulative = -9.97032e-005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e-005, 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 wall-mp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-2 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 = 1.76928e-005, 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``` This is my fvOptions file: I don't have much knowledge about this. Please correct me.. Code: ```FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // wall-mp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wall-mp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wall-dp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } wall-dp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } wall-mp-1 { 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("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; } }``` About my case .. please see above post.. 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 wall-mp-1 wall-mp-2 wall-dp-1 wall-dp-2

 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); } } }``` you can create faceSet using 'topoSet' utility of OpenFoam.

 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: wall-mp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-mp-2 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-1 - applying source for all time - selecting all cells - selected 5338536 cell(s) with volume 0.000333435 Selecting finite volume options model type scalarSemiImplicitSource Source: wall-dp-2 - 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 f-turbo: selecting model: DarcyForchheimer creating porous zone: f-turbo 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 = -9.97032e-005, cumulative = -9.97032e-005 smoothSolver: Solving for epsilon, Initial residual = 0.065236, Final residual = 4.46237e-005, 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 wall-mp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-mp-2 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-1 defined for field h but never used --> FOAM Warning : From function void option::checkApplied() const in file fvOptions/fvOption.C at line 368 Source wall-dp-2 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 = 1.76928e-005, 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 = 1.89677e-005, 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 = 1.47114e-005, 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``` and my fvOptions file Code: ```wall-mp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wall-mp-1surface; cellSet wall-mp-1; volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wall-mp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wall-mp-2surface; cellSet wall-mp-2; volumeMode specific; injectionRateSuSp { h (149954.264 0); } } } wall-dp-1 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wall-dp-1surface; cellSet wall-dp-1; volumeMode specific; injectionRateSuSp { h (412374.225 0); } } } wall-dp-2 { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { cellZone wall-dp-2surface; cellSet wall-dp-2; volumeMode specific; injectionRateSuSp { h (412374.225 0); } } }``` topoSetDict file Code: ```actions ( { name wall-mp-1surface; type faceSet; action new; source patchToFace; sourceInfo { name wall-mp-1; } } { name wall-mp-2surface; type faceSet; action new; source patchToFace; sourceInfo { name wall-mp-2; } } { name wall-dp-1surface; type faceSet; action new; source patchToFace; sourceInfo { name wall-dp-1; } } { name wall-dp-2surface; type faceSet; action new; source patchToFace; sourceInfo { name wall-dp-2; } } { name wall-mp-1CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wall-mp-1surface; option any; } } { name wall-mp-2CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wall-mp-2surface; option any; } } { name wall-dp-1CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wall-dp-1surface; option any; } } { name wall-dp-2CellSet; type cellSet; action new; source faceToCell; sourceInfo { set wall-dp-2surface; option any; } } );``` May i know why i am getting this error ?? 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 wall-mp-1 wall-mp-2 wall-dp-1 wall-dp-2 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` So, that's why i have assigned in W/m3. 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.