
[Sponsors] 
How I can introduce my power heat (W) in chtMultiRegionFoam? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 2, 2015, 10:43 
How I can introduce my power heat (W) in chtMultiRegionFoam?

#1 
Member
amine
Join Date: Jan 2014
Location: FRANCE
Posts: 84
Rep Power: 12 
Hi,
Can anyone explain me how I can introduce power heat (W) in chtMultiRegionFoam solver? In my case I have 1.5 W in my LED. Thanks 

June 2, 2015, 11:16 

#2 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
__________________
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! 

June 5, 2015, 06:41 

#3 
Member
amine
Join Date: Jan 2014
Location: FRANCE
Posts: 84
Rep Power: 12 
Hi Alex,
I have try to do a sample 2D test with fvOptions. I think that fvOptions don't have any effect. I use OF2.3.0 and chtMultiRegionFoam. fvOptions: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6.x   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; class dictionary; format ascii; location "system"; object fvOptions; } cylindre_Source_scalar { type scalarSemiImplicitSource; selectionMode cellZone; cellZone cylindre; active true; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (10 0); } } } Thanks 

June 5, 2015, 08:14 

#4  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
Quote:
Code:
cylindre_Source_scalar { type scalarSemiImplicitSource; selectionMode all; active true; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (10 0); } } } Btw, can you post your log file so that we can see if fvOptions is correctly read by the solver? In the output of the solver it says if any fvOptions have been read or not... 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! 

June 7, 2015, 09:14 

#5 
Member
amine
Join Date: Jan 2014
Location: FRANCE
Posts: 84
Rep Power: 12 
Hi Alex
I tried your solution but it's doesn't work. This is my solve log thanks 

June 7, 2015, 15:01 

#6  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
Quote:
Code:
Creating finite volume options from "system/fvOptions" Selecting finite volume options model type scalarSemiImplicitSource Source: cylindre_Source_scalar  applying source for all time  selecting all cells  selected 176 cell(s) with volume 2.786796e06
__________________
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! 

June 7, 2015, 16:34 

#7 
Senior Member
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13 
Code:
scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (10 0); } } Code:
Selecting finite volume options model type scalarSemiImplicitSource Source: cylindre_Source_scalar  applying source for all time  selecting all cells  selected 176 cell(s) with volume 2.786796e06 to get 1.5W you need a number more like 5E5
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET 

June 7, 2015, 18:02 

#8  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
Quote:
@aminem: Otherwise you can also use Code:
scalarSemiImplicitSourceCoeffs { volumeMode absolute; injectionRateSuSp { h (1.5 0); } } 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! 

June 8, 2015, 06:23 

#9 
Member
amine
Join Date: Jan 2014
Location: FRANCE
Posts: 84
Rep Power: 12 
Hi,
In my fvOptions I have put absolute in volumeMode. Now fvOptions have an effect on temperature. I have doubt on what BC I must put. As you can see in attached figure I want to put my solid in open air volume. I have put freestream BC, but I have this error: Code:
Solving for fluid region fluide diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #4 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:? #5 at ??:? #6 at ??:? #7 at ??:? #8 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #9 at ??:? Thanks for your help 

June 8, 2015, 12:28 

#10 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
Hi aminem,
We could do a exchange.... I usually use inletOulet for U,T,p_rgh and I have obtained good results, however, you would also try with fixedPressure in p_rgh. My doubt is about injectRateSuSp inside a solid.... it doesn't work but if I use it inside a fluid, it works..... I don't know the problem, could you help me? U { type inletOutlet; inletValue uniform ( 0 0 0 ); value uniform ( 0 0 0 ); } T { type inletOutlet; inletValue uniform 300; value uniform 300; } p_rgh { type inletOutlet; inletValue uniform 1E5; value uniform 1E5; } 

June 9, 2015, 10:11 

#11 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
My simulation is like your model, with atmospheric conditions but I have a bulb with a lightwire. The problem is the wire... it has 3D mesh and I want to introduce power/m^3 inside the wire using fvOptions. It hasn't worked.....the wire hasn't increased the temperature...... I checked the unit and these were correct....
In my fvOptions file: heatSource { type scalarSemiImplicitSource; active on; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRate { h (5e+09 0); } } } thanks! 

June 9, 2015, 10:14 

#12 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
You need to provide more information Cartuns11, otherwise no one will be able to help you...
__________________
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! 

June 9, 2015, 10:59 

#13 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
ok!
The model is a chtMultiRegionSimpleFoam simulation without radiation. It consists in a bulb with wire and support inside the atmospheric air (openning conditions). The target is the temperatures of the bulb, wire, support and domain0 (air atmospheric). The input is the power of wire, which is a solid. The support is also a solid and the bulb and the air are a fluids. The wire volume is 5e09 [m^3] and I have to introduce 5e+09 [W/m^3]. The best way is fvOptions....but, when I carry out the solver, the temperature of wire doesnt increase.....it maintains same value. I did proves which consisted in the power introducing in a fluid with the same method.......and inside the fluid, it worked..... I don't understand it.... I have loaded some image and some codes....All codes of wire. fvOptions Code:
heatSource { type scalarSemiImplicitSource; active true; selectionMode all; scalarSemiImplicitSourceCoeffs { volumeMode specific; injectionRateSuSp { h (5e+09 0); } } } Code:
solvers { p { solver GAMG; tolerance 1e7; relTol 0.01; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } k { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } omega { solver smoothSolver; smoother GaussSeidel; tolerance 1e8; relTol 0.1; nSweeps 1; } } SIMPLE { nNonOrthogonalCorrectors 0; } potentialFlow { nNonOrthogonalCorrectors 10; } relaxationFactors { fields { p 0.5; } equations { U 0.7; k 0.7; omega 0.7; } } cache { grad(U); } Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwindV grad(U); div(phi,k) bounded Gauss upwind; div(phi,omega) bounded Gauss upwind; div((nuEff*dev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } Code:
thermoType { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } mixture { specie { nMoles 1; molWeight 12; } transport { kappa 95; } thermodynamics { Hf 0; Cp 176; } equationOfState { rho 19300; } } 

June 10, 2015, 02:36 

#14 
Senior Member
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13 
Need to see the solver log file
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET 

June 10, 2015, 06:21 

#15 
Member
amine
Join Date: Jan 2014
Location: FRANCE
Posts: 84
Rep Power: 12 
Hi Curtuns1,
1/We need to see your Log file to know if the fvOptions file is read. 2/You must put fvOptions in system/wire directory. 3/I think you need to put a cellZone indication in your fvOptions file? For me it's work for one source. I try to do this with multiple sources. 

June 10, 2015, 07:22 

#16 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
Hi,
I've loaded the solver log. The solver works but the temperature of wire doesn't increase...... I think that the solver reads fvOptions correctly..... In addition, The problem isn't the units, because I have put values between [5E20 to 5E20]..... but the temperature hasn't moved..... In a other forum, I've read about this and the introducing power inside a solid using fvOptions doesn't work. It could be a problem of code.... The fvOptions is just in the wire folder. BOMBILLADIRECCIO: bulb CASQUILLODIRECCIO: support FILAMENTODIRECCIO: wire domain0:air Code:
\**/ Build : 2.3.0f5222ca19ce6 Exec : chtMultiRegionSimpleFoam parallel Date : Jun 10 2015 Time : 11:47:18 Host : "agonzalezPrecisionWorkStationT7500" PID : 713 Case : /home/agonzalez/Desktop/CloudFlow/Modelo_FOCO_SEAT/prbomb2 nProcs : 8 Slaves : 7 ( "agonzalezPrecisionWorkStationT7500.714" "agonzalezPrecisionWorkStationT7500.715" "agonzalezPrecisionWorkStationT7500.716" "agonzalezPrecisionWorkStationT7500.717" "agonzalezPrecisionWorkStationT7500.718" "agonzalezPrecisionWorkStationT7500.719" "agonzalezPrecisionWorkStationT7500.720" ) Pstream initialized with: floatTransfer : 0 nProcsSimpleSum : 0 commsType : nonBlocking polling iterations : 0 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region BOMBILLADIRECCIO for time = 0 Create fluid mesh for region domain0 for time = 0 Create solid mesh for region CASQUILLODIRECCIO for time = 0 Create solid mesh for region FILAMENTODIRECCIO for time = 0 *** Reading fluid mesh thermophysical properties for region BOMBILLADIRECCIO Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport polynomial; thermo hPolynomial; equationOfState icoPolynomial; specie specie; energy sensibleEnthalpy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to turbulence Selecting turbulence model type laminar Adding to ghFluid Adding to ghfFluid Selecting radiationModel none Adding fvOptions No finite volume options present *** Reading fluid mesh thermophysical properties for region domain0 Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport polynomial; thermo hPolynomial; equationOfState icoPolynomial; specie specie; energy sensibleEnthalpy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to turbulence Selecting turbulence model type laminar Adding to ghFluid Adding to ghfFluid Selecting radiationModel none Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region CASQUILLODIRECCIO Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Selecting radiationModel none Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region FILAMENTODIRECCIO Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Selecting radiationModel none Adding fvOptions Creating finite volume options from fvOptions Selecting finite volume options model type scalarSemiImplicitSource Source: heatSource  applying source for all time  selecting all cells  selected 3256 cell(s) with volume 5.422112e09 Time = 1 Solving for fluid region BOMBILLADIRECCIO DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.005970245, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.006041075, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0007919736, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.01634446, Final residual = 0.0001542216, No Iterations 2 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.7937571, Final residual = 0.007827255, No Iterations 47 time step continuity errors : sum local = 0.159732, global = 2.600357e10, cumulative = 2.600357e10 Min/max rho:1.156291 1.156291 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.009871374, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.008090986, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0001421311, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.0006556001, Final residual = 6.4236e06, No Iterations 2 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.9536995, Final residual = 0.00745634, No Iterations 34 DICPCG: Solving for p_rgh, Initial residual = 0.1693578, Final residual = 0.0016451, No Iterations 33 time step continuity errors : sum local = 0.004237694, global = 8.872091e05, cumulative = 8.872117e05 Min/max rho:1.170813 1.170813 Solving for solid region CASQUILLODIRECCIO DICPCG: Solving for h, Initial residual = 0.5277625, Final residual = 0.0003224809, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 Solving for solid region FILAMENTODIRECCIO DICPCG: Solving for h, Initial residual = 0.4530837, Final residual = 0.0004174483, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 ExecutionTime = 6.63 s ClockTime = 7 s Time = 2 Solving for fluid region BOMBILLADIRECCIO DILUPBiCG: Solving for Ux, Initial residual = 0.2284703, Final residual = 0.0001765353, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.2329958, Final residual = 0.0001731993, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.2032166, Final residual = 0.0001470408, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.9999981, Final residual = 0.006117996, No Iterations 4 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.8656138, Final residual = 0.007022698, No Iterations 47 time step continuity errors : sum local = 0.05913433, global = 1.469776e10, cumulative = 8.872132e05 Min/max rho:1.156291 1.156291 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.03329544, Final residual = 2.302509e05, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.03612496, Final residual = 2.331844e05, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.02318816, Final residual = 1.174436e05, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.009117826, No Iterations 2 Min/max T:299.9999 300 DICPCG: Solving for p_rgh, Initial residual = 0.9949871, Final residual = 0.008860348, No Iterations 30 DICPCG: Solving for p_rgh, Initial residual = 0.08539426, Final residual = 0.0008468964, No Iterations 32 time step continuity errors : sum local = 0.02833294, global = 0.0002961078, cumulative = 0.0002073865 Min/max rho:1.170812 1.170813 Solving for solid region CASQUILLODIRECCIO DICPCG: Solving for h, Initial residual = 0.8983162, Final residual = 0.0002216541, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 Solving for solid region FILAMENTODIRECCIO DICPCG: Solving for h, Initial residual = 0.2041466, Final residual = 0.0002220012, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 ExecutionTime = 7.46 s ClockTime = 8 s Time = 3 Solving for fluid region BOMBILLADIRECCIO DILUPBiCG: Solving for Ux, Initial residual = 0.2255419, Final residual = 0.0002050287, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.1777021, Final residual = 0.0001137957, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.7969785, Final residual = 0.0006711936, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.4353527, Final residual = 0.001637115, No Iterations 4 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.6657176, Final residual = 0.005987832, No Iterations 46 time step continuity errors : sum local = 0.02866349, global = 2.892586e11, cumulative = 0.0002073865 Min/max rho:1.156291 1.156291 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.1704313, Final residual = 9.563561e05, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.1710087, Final residual = 6.118017e05, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.05492389, Final residual = 8.961354e05, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.9856835, Final residual = 0.005686893, No Iterations 2 Min/max T:299.9969 300.0023 DICPCG: Solving for p_rgh, Initial residual = 0.8956926, Final residual = 0.00844547, No Iterations 38 DICPCG: Solving for p_rgh, Initial residual = 0.001688192, Final residual = 1.664736e05, No Iterations 35 time step continuity errors : sum local = 0.006222197, global = 0.001343636, cumulative = 0.001136249 Min/max rho:1.170803 1.170825 Solving for solid region CASQUILLODIRECCIO DICPCG: Solving for h, Initial residual = 0.8825567, Final residual = 0.0003003737, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 Solving for solid region FILAMENTODIRECCIO DICPCG: Solving for h, Initial residual = 0.1137917, Final residual = 0.000146549, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 ExecutionTime = 8.34 s ClockTime = 9 s Time = 4 Solving for fluid region BOMBILLADIRECCIO DILUPBiCG: Solving for Ux, Initial residual = 0.1771537, Final residual = 0.0001553637, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.1853754, Final residual = 0.0001522035, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.6621283, Final residual = 0.0005294418, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.280204, Final residual = 0.001580275, No Iterations 4 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.7542199, Final residual = 0.005754844, No Iterations 44 time step continuity errors : sum local = 0.01850979, global = 1.039983e10, cumulative = 0.001136249 Min/max rho:1.156291 1.156291 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.1450099, Final residual = 0.001142569, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.1362821, Final residual = 0.001065343, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1069051, Final residual = 0.0009845638, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.5549841, Final residual = 0.003314565, No Iterations 2 Min/max T:299.9962 300.0023 DICPCG: Solving for p_rgh, Initial residual = 0.1746192, Final residual = 0.001707782, No Iterations 40 DICPCG: Solving for p_rgh, Initial residual = 0.001101075, Final residual = 1.08441e05, No Iterations 39 time step continuity errors : sum local = 0.00453244, global = 0.001133385, cumulative = 0.002269634 Min/max rho:1.170803 1.170828 Solving for solid region CASQUILLODIRECCIO DICPCG: Solving for h, Initial residual = 0.5303216, Final residual = 0.0001219209, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 Solving for solid region FILAMENTODIRECCIO DICPCG: Solving for h, Initial residual = 0.06639977, Final residual = 8.910753e05, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 ExecutionTime = 9.44 s ClockTime = 10 s Time = 5 Solving for fluid region BOMBILLADIRECCIO DILUPBiCG: Solving for Ux, Initial residual = 0.140732, Final residual = 0.0001026456, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.2060334, Final residual = 0.0001278458, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.1182916, Final residual = 7.821812e05, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.4115059, Final residual = 0.003101837, No Iterations 4 Min/max T:300 300 DICPCG: Solving for p_rgh, Initial residual = 0.5854837, Final residual = 0.004143481, No Iterations 44 time step continuity errors : sum local = 0.007204766, global = 2.257701e10, cumulative = 0.002269634 Min/max rho:1.156291 1.156291 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.1652503, Final residual = 0.001428339, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.1539691, Final residual = 0.001333403, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1358239, Final residual = 3.548498e05, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.4827221, Final residual = 7.081489e05, No Iterations 4 Min/max T:299.9895 300.0014 DICPCG: Solving for p_rgh, Initial residual = 0.1503564, Final residual = 0.001128931, No Iterations 35 DICPCG: Solving for p_rgh, Initial residual = 0.004037298, Final residual = 4.023457e05, No Iterations 29 time step continuity errors : sum local = 0.003569743, global = 0.0009190757, cumulative = 0.001350558 Min/max rho:1.170807 1.170856 Solving for solid region CASQUILLODIRECCIO DICPCG: Solving for h, Initial residual = 0.4428948, Final residual = 0.0001086157, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 Solving for solid region FILAMENTODIRECCIO DICPCG: Solving for h, Initial residual = 0.05024991, Final residual = 7.156336e05, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300 ExecutionTime = 10.33 s ClockTime = 11 s 

June 10, 2015, 08:01 

#17 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
Are you sure the fvSolution's code you provided above belongs to the wire? I don't think so...
Regarding what you say about a problem in the code, you are wrong, there's no problem in the code, I have run several simulations with heat sources in solids and they work well for me... With regard to the units, as per what you say, the bulb is providing only 1W. I don't know if it is correct or not but it seems a low value... Have you set up properly your initial and boundary conditions?
__________________
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! 

June 12, 2015, 04:16 

#18 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
I've checked all.... but I haven't found any error.... may be, there is one but I haven't seen it.
The units are correct, because the wire volume is 5e09 m^3 and the heat flux is 5e+09 W/m^3, therefore I have 25 W inside wire. I'm going to carry out other models... I'll tell you if I achieve to solve the problem. Thanks. Greetings 

June 12, 2015, 06:30 

#19 
New Member
Join Date: May 2015
Location: Barcelona
Posts: 24
Rep Power: 11 
Hi everybody,
I have found the ""error/solution""............. The heat source of fvOptions works, if the model is no steadyState..... All time, I've been carrying out steadyState simulations (chtMultiRegionSimpleFoam) but when I have used chtMultiRegionFoam the heat source has been introduced.... I would like to do the model in steadyState with chtMultiRegionFoam...... any idea? could I do it? is it possible? I'm thinking that the problem is in fvSchemes and fvSolution Thanks 

June 12, 2015, 09:25 

#20 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 22 
Hi Cartuns11,
I'm glad you could make it work in a transient state solver, however, it must work in steady state too because I have been working with chtMultiRegionSimpleFoam with solid generating regions for a while with no problem... I suggest you something... Why don't you try to run one of the tutorial cases you can find within the "$FOAM_TUTORIALS/heatTransfer/chtMultiRegionSimpleFoam" directory first? You should add a heat source in one of the regions since no one of the tutorials contains volumetric heat generation, but if you are able to make the tutorial run properly obtaining physical results (I'm sure you can do it!) you can then adapt the geometry of your case to the parameters (fvSolution, fvSchemes...) used in the tutorial. Hope it helps, 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! 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
chtMultiRegionFoam connection between solid and fluid region of heat exchanger  ahab  OpenFOAM  1  December 18, 2019 01:37 
dieselFoam problem!! trying to introduce a new heat transfer model  vivek070176  OpenFOAM Programming & Development  10  December 24, 2014 00:48 
Constant velocity of the material  Sas  CFX  15  July 13, 2010 09:56 
Problem of heat balance in Coal Boiler simulation  DG  FLUENT  9  December 25, 2008 21:57 
Concentric tube heat exchanger (AirWater)  Young  CFX  5  October 7, 2008 00:17 