
[Sponsors] 
chtMultiRegionSimpleFoam: Thermal Conduction + SurfaceToSurface Radiation 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 31, 2015, 12:39 
chtMultiRegionSimpleFoam: Thermal Conduction + SurfaceToSurface Radiation

#1 
Senior Member
Sergei
Join Date: Dec 2009
Posts: 232
Rep Power: 16 
Problem Formulation
I am about to model a complex problem of conjugate heat transfer in a set of fluids/solids coupled to each other through shared boundaries (interfaces). Thermal conduction defines heat transfer in solid regions. Thermal conduction, thermal radiation and convection govern heat transfer in fluid regions. chtMultiRegionSimpleFoam solver seems to be an adequate choice to solve such a problem. Before I go into the world of real engineering problems I consider a rather simple test case. A sketch of my geometry is here. Yes, the mesh is quite coarse and not optimal (an external mesher was utilized to construct polyhedral cells). Anyway, I guess I can live with it. We have 3 concentric spherical layers: inner (cellZone_1), central (cellZone_2) and outer (cellZone_3) regions. The inner surface of cellZone_1 is at constant temperature 300°K; the outer surface of cellZone_3 is at constant temperature 2000°K; cellZone_2 is thermally coupled with cellZone_1 and cellZone_3 at its surfaces. А sample line to plot some results along is shown below. Part 1 To start off I narrowed a complex general case to a simple problem avoiding all the heat transfer options except thermal conduction in solid regions (with thermal conductivity “kappa” = 10 W/(m K)). OpenFOAM handled its job quite well! A graph in which the values of temperature are plotted along the sample line is shown here. OpenFOAM solution is compared with proprietary software solution. Perfect coincidence! Part 2 Then I added some complexity to the simulation problem – now the central region is considered to be transparent for gray thermal radiation to transfer between region boundaries (surfacetosurface radiation with nonparticipating medium). Here comes the problem. All 3 regions remain solid as in the simplest case mentioned before: Code:
//“constant/regionProperties” regions ( fluid () solid (cellZone_1 cellZone_2 cellZone_3) Code:
//“constant/cellZone_2/radiationProperties” radiation on; radiationModel viewFactor; viewFactorCoeffs { smoothing true; constantEmissivity true; } solverFreq 3; absorptionEmissionModel none; scatterModel none; sootModel none; For inner and outer regions I have "constant/cellZone_1/radiationProperties" and "constant/cellZone_3/radiationProperties": Code:
//“constant/cellZone_1/radiationProperties”, “constant/cellZone_3/radiationProperties” radiation on; radiationModel opaqueSolid; absorptionEmissionModel none; scatterModel none; sootModel none; Initial and boundary conditions are defined in a strange way. First of all why should we ever need pressure “p” file for our solid regions? Doesn’t we solve only for energy? When I remove this pressure file the solver starts to complain about it. Code:
[2] > FOAM FATAL IO ERROR: [2] cannot find file [2] [2] file: /home/geeko/OpenFOAM/geeko2.4.0/run/my_cases/radiation_sphere/processor2/0/cellZone_1/p at line 0. [2] [2] From function regIOobject::readStream() [2] /home/geeko/OpenFOAM/geeko2.4.0/run/my_cases/radiation_sphere/processor1/0/cellZone_1/p at line 0. [1] [1] From function regIOobject::readStream() [1] in file db/regIOobject/regIOobjectRead.C at line 73. Code:
//"0/cellZone_1/T", "0/cellZone_3/T" ".*_to_.*" { type compressible:: turbulentTemperatureRadCoupledMixed; value uniform 300; Tnbr T; kappa solidThermo; kappaName none; QrNbr Qr; Qr none; } Code:
//"0/cellZone_2/T" ".*_to_.*" { type compressible::turbulentTemperatureRadCoupledMixed; value uniform 300; Tnbr T; kappa solidThermo; kappaName none; QrNbr none; Qr Qr; } The way we specify radiation heat flux “Qr” on boundaries leaves no alternative. Note radiation "emissivity uniform 1". Code:
// "0/cellZone_2/Qr" ".*_to_.*" { type greyDiffusiveRadiationViewFactor; value uniform 0; emissivityMode solidRadiation; Qro uniform 0; emissivity uniform 1; } With all this setup I can say it didn't do me any good. I didn’t manage to obtain correct solution in OpenFOAM. It turned out that thermal radiation cannot be solved in solid regions. The temperature profile along my sample line is the same as in the noradiation case. Correct solution obtained with proprietary software is shown in the picture above (it is marked as “proprietary, radOn”) as a reference. OpenFoam “Qr” field is zero everywhere at the end of simulation. No radiation transfer is observed: Part 3 Well, what if I made my central region (cellZone_2) fluid, not solid? Let’s see if we could benefit from it. Code:
//“constant/regionProperties” regions ( fluid (cellZone_2) solid (cellZone_1 cellZone_3) ); Code:
//“system/cellZone_2/fvSolution” SIMPLE { … frozenFlow on; } Code:
// “constant/cellZone_2/thermophysicalProperties” thermoType { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } pRef 100000; mixture { specie { nMoles 1; molWeight 28.9; } thermodynamics { Cp 1000; Hf 0; } transport { mu 1.8e05; Pr 0.0018; //Pr=mu*Cp/kappa } equationOfState { rho 1e2; } } Can anyone comment on this? What is the relation between “kappa” and “rho”? Then I switched radiation on (“viewFactorsModel”). “radiationProperties” file for fluid region remained the same as it was in the allsolids case. “radiationProperties” files for inner and outer solid regions had to be altered. Specifically “absorptionEmissionModel” cannot be “none” anymore. I had to set “absorptionEmissionModel constantAbsorptionEmission” otherwise the solver blows up and shows this message: Code:
Time = 1 Solving for fluid region cellZone_2 DILUPBiCG: Solving for h, Initial residual = 0.5466406, Final residual = 0.02687252, No Iterations 2 [0] #0 Foam::error::printStack(Foam::Ostream&) at ??:? [0] #1 Foam::sigFpe::sigHandler(int) at ??:? [0] #2 ? in "/lib64/libc.so.6" [0] #3 Foam::radiation::viewFactor::calculate() at ??:? [0] #4 Foam::radiation::radiationModel::correct() at ??:? [0] #5 ? at ??:? [0] #6 __libc_start_main in "/lib64/libc.so.6" [0] #7 ? at /home/abuild/rpmbuild/BUILD/glibc2.17/csu/../sysdeps/x86_64/start.S:126 [linux:06114] *** Process received signal *** [linux:06114] Signal: Floating point exception (8) [linux:06114] Signal code: (6) [linux:06114] Failing at address: 0x3e8000017e2 [linux:06114] [ 0] /lib64/libc.so.6(+0x35450) [0x7f42d69d6450] [linux:06114] [ 1] /lib64/libc.so.6(gsignal+0x35) [0x7f42d69d63d5] [linux:06114] [ 2] /lib64/libc.so.6(+0x35450) [0x7f42d69d6450] [linux:06114] [ 3] /opt/OpenFOAM/OpenFOAM2.4.0/platforms/linux64GccDPOpt/lib/libradiationModels.so(_ZN4Foam9radiation10viewFactor9calculateEv+0xd83) [0x7f42d8cfd273] [linux:06114] [ 4] /opt/OpenFOAM/OpenFOAM2.4.0/platforms/linux64GccDPOpt/lib/libradiationModels.so(_ZN4Foam9radiation14radiationModel7correctEv+0x1f) [0x7f42d8cbf55f] [linux:06114] [ 5] chtMultiRegionSimpleFoam() [0x441202] [linux:06114] [ 6] /lib64/libc.so.6(__libc_start_main+0xf5) [0x7f42d69c2a15] [linux:06114] [ 7] chtMultiRegionSimpleFoam() [0x44a08d] [linux:06114] *** End of error message *** Code:
“constant/cellZone_1/radiationProperties”, “constant/cellZone_3/radiationProperties” Radiation on; radiationModel opaqueSolid; absorptionEmissionModel constantAbsorptionEmission; constantAbsorptionEmissionCoeffs { absorptivity absorptivity [ 0 1 0 0 0 0 0 ] 0; emissivity emissivity [ 0 1 0 0 0 0 0 ] 1; E E [ 1 1 3 0 0 0 0 ] 0; } As I said before I am not interested in having radiation within inner and outer regions. All I want is surfacetosurface radiation in central region. Moreover, no matter what emissivity defined on the boundaries (in “0/Qr” file) is, it seems to have no effect on the solution. This is totally opposed to my goal. Conclusion To sum everything up I can say that I failed to get chtMultiRegionSimpleFoam working the way I need. Should anyone have positive experience working with the solver please share your thoughts on the subject. You can download my OpenFOAM cases from this links: radiation_sphere_solid: http://s000.tinyupload.com/?file_id=...00567809681193 radiation_sphere_fluid: http://s000.tinyupload.com/?file_id=...41445147881545 Last edited by Zeppo; November 1, 2015 at 07:26. 

November 6, 2015, 09:00 

#2  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 17 
Hi Zeppo!
Interesting post yours! As I developed my Final Thesis using this solver and working with radiation I think I can help you with most of your doubts in this post. Geometry is quite simple, wich is good when you first try to model a system with the intention to understand how physical phenomena is modelled with OF. Now I will try to respond to your main hesitations with the most accurate information I can give you. Take into account that I developed my Final Thesis with OF 2.3.x, so my explanations are referred to this version's code, some aspects may have changed from this version on (the newst verision launched is 3.0.x). Simple case. No comment about it. Quote:
Besides that, I think that view factors method can't handle participating media, just surface to surface radiation... Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
Quote:
I hope that my words have come in handy for your purpose and may help you with your future simulations! 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! 

November 7, 2015, 12:46 

#3  
Senior Member
Sergei
Join Date: Dec 2009
Posts: 232
Rep Power: 16 
Hello Alex.
Quote:
Quote:
Quote:
Quote:
Code:
//"0/cellZone_2/T" ".*_to_.*" { type compressible::turbulentTemperatureRadCoupledMixed; value uniform 300; Tnbr T; kappa fluidThermo; QrNbr none; Qr none kappaName none; } Kind of strange and suspicious, isn't it? Then how can I exclude some boundaries from RTE when I don't want them to take part in radiation exchange? Is it ever possible? Quote:
Code:
//"constant/cellZone_1/radiationProperties", "constant/cellZone_3/radiationProperties" radiation off; radiationModel opaqueSolid; absorptionEmissionModel none; constantAbsorptionEmissionCoeffs { absorptivity absorptivity [ 0 1 0 0 0 0 0 ] 0.0; //opaque emissivity emissivity [ 0 1 0 0 0 0 0 ] 0.0; E E [ 1 1 3 0 0 0 0 ] 0; } scatterModel none; sootModel none; Quote:
Quote:
Solver output shows no sign of progress in solution. It is obviously converged: Code:
Time = 998 Solving for fluid region cellZone_2 DILUPBiCG: Solving for h, Initial residual = 9.552542e08, Final residual = 9.552542e08, No Iterations 0 Min/max T:1738.045 1851.023 Solving for solid region cellZone_1 DICPCG: Solving for h, Initial residual = 9.899032e07, Final residual = 9.899032e07, No Iterations 0 Min/max T:300 1789.063 Solving for solid region cellZone_3 DICPCG: Solving for h, Initial residual = 9.094747e07, Final residual = 9.094747e07, No Iterations 0 Min/max T:1816.936 2000 ExecutionTime = 66.05 s ClockTime = 78 s Time = 999 Solving for fluid region cellZone_2 DILUPBiCG: Solving for h, Initial residual = 9.552542e08, Final residual = 9.552542e08, No Iterations 0 LU Back substitute C matrix.. Min/max T:1738.045 1851.023 Solving for solid region cellZone_1 DICPCG: Solving for h, Initial residual = 9.899032e07, Final residual = 9.899032e07, No Iterations 0 Min/max T:300 1789.063 Solving for solid region cellZone_3 DICPCG: Solving for h, Initial residual = 9.094747e07, Final residual = 9.094747e07, No Iterations 0 Min/max T:1816.936 2000 ExecutionTime = 66.2 s ClockTime = 78 s Time = 1000 Solving for fluid region cellZone_2 DILUPBiCG: Solving for h, Initial residual = 9.552542e08, Final residual = 9.552542e08, No Iterations 0 Min/max T:1738.045 1851.023 Solving for solid region cellZone_1 DICPCG: Solving for h, Initial residual = 9.899032e07, Final residual = 9.899032e07, No Iterations 0 Min/max T:300 1789.063 Solving for solid region cellZone_3 DICPCG: Solving for h, Initial residual = 9.094747e07, Final residual = 9.094747e07, No Iterations 0 Min/max T:1816.936 2000 ExecutionTime = 66.23 s ClockTime = 78 s Quote:
I have to ask my question from the post #1 again. Can you (or anyone else) tell me why thermal conductivity (kappa) depends on density (rho) in the case of a fluid region? Shouldn’t the relation “Pr=mu*Cp/kappa” always hold? Code:
//“constant/cellZone_2/thermophysicalProperties” thermoType { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState rhoConst; //<perfectGas>; specie specie; energy sensibleEnthalpy; } pRef 100000; mixture { specie { nMoles 1; molWeight 28.9; } thermodynamics { Cp 1000; Hf 0; } transport { mu 1.8e05; Pr 0.0018; // "Pr=mu*Cp/kappa" } equationOfState { rho 1e02; } } It is easy to see that as density increases the temperature distribution in the central region gets more and more level, uniform as if thermal conductivity increased too. Obviously, there are 2 limit boundaries the plot line can stick to: 1) density is 0 (then we get the correct solution depicted by a dashed red line in the picture), 2) density is infinite (the solution is totally incorrect and corresponds to the case of infinite thermal conductivity). It looks like we have something like this: “kappa = f *(mu*Cp/Pr)“, where f is a function of density. It goes to 1 when density goes to 0 and it goes to infinity when density goes to infinity. Can anybody confirm my assumption? My a little bit updated case can be downloaded here: http://s000.tinyupload.com/?file_id=31692654334161942508 

November 27, 2015, 18:16 

#4  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 17 
Hi Zeppo,
First of all, I apologize for my very late response, I've been busy lately. I will try to respond quickly to your questions... Quote:
Quote:
I don't think this is so strange nor suspicious, radiation is taken into account in your calculations for the fluid region but something "weird" is happening at the boundaries when you set Qr/QrNbr to "none", that is to say, something "not very physical, but mathematically possible" occurs. Btw, the dotted blue line, corresponding to the proprietary software, represents the central region as a fluid or as a solid? And what about the segmented red line? If you want some boundaries not to take part in the radiation exchange in the ViewFactors method you can exclude them in the ViewFactorsDict file. However, I never did it and I have no clue if it can lead to unphysical results... Maybe you could try it and find it out! Quote:
Naaaah... Just kidding! I know it is quite confusing, mainly because of the units, everyone knows that emissivity in a surface is a dimensionless factor. However, in a solid region here is where you can store the value of the emissivity. Another confusing point in this file is the definition of an opaque solid, there it says that as the solid is opaque its absorptivity has a value of 0!!! Someone was drunk when writing this file because what defines the opacity of a surface is its transmitance not its absorptivity! Anyway, I hope that someday someone will change the format file for solid regions so that people don't get confused! Quote:
Quote:
Let's see if someone else more skilled and clever than us can find the solution of this problem... So far my little contribution for today. I hope it can help you a bit on your multiRegionRadiative adventure! And again, I'm sorry for my late response! 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! 

November 29, 2015, 15:43 

#5  
Senior Member
Sergei
Join Date: Dec 2009
Posts: 232
Rep Power: 16 
Quote:
Code:
//“constant/cellZone_1/radiationProperties”, “constant/cellZone_3/radiationProperties” radiation off; radiationModel opaqueSolid; Code:
// "0/cellZone_2/Qr" ".*" { type greyDiffusiveRadiationViewFactor; value uniform 0; emissivityMode lookup; Qro uniform 0; emissivity uniform 1; } Quote:
Quote:
Code:
// "constant/cellZone_2/viewFactorsDict" ".*_to_.*" { nFacesInCoarsestLevel 0; featureAngle 0; } maxDynListLength 100000000; Code:
// "log.viewFactorsGen.cellZone_2" Total number of coarse faces: 2760 View factor patches included in the calculation : 2(0 1) Calculating view factors... Writing view factor matrix... F00: 2.042893e08 F01: 1.00178 F10: 0.2369856 F11: 0.5562016 On the other hand the least number of coarse faces I can get is 4. So you can't exclude a patch from radiation exchange as you say. Or maybe I am going the wrong way and I can do so in any other way? Code:
// "constant/cellZone_2/viewFactorsDict" ".*_to_.*" { nFacesInCoarsestLevel 0; featureAngle 1000000; } Code:
// "log.viewFactorsGen.cellZone_2" Total number of coarse faces: 4 View factor patches included in the calculation : 2(0 1) Calculating view factors... Writing view factor matrix... F00: 0 F01: 0.8841754 F10: 0 F11: 1.059796 Quote:
Quote:
All in all I don't want to give up and will continue my "experiments" with the solver. 

December 13, 2015, 15:26 

#6  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 17 
Hi Zeppo,
Again, I apologise for my late response! Quote:
Quote:
Quote:
Code:
writeViewFactorMatrix true; // Write agglomeration as a volScalarField with calculated boundary values writeFacesAgglomeration true; writePatchViewFactors false; Quote:
Quote:
Quote:
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! 

December 14, 2015, 05:51 

#7 
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 270
Rep Power: 13 
Hello, Zeppo,
I would just correct you about kappa and rho effect. Your solutions are NOT converged at all. In thermal stationary simulation, convergence check should be done with some probes, not with residual at 1e6. In your convergence plot, you see a flat line at 1e7 after 700 iter, and if you look at the log, you have "No Iteration 0". This mean you don NOT calculate T Field anymore ... What you should do is: set Tolerance to a far lower value 1e12,, or add "minIter 1;" in you FvSolution File, for the h solver. Thermal simulation have usually a convergence at very low residual value. regards, olivier 

January 13, 2016, 05:19 

#8  
New Member
Join Date: Mar 2015
Location: Earth yet
Posts: 25
Rep Power: 6 
Quote:
Since it is an incompressible solver all the equations are divided by rho, even the viscosity value to be used should be cinematic rather than dynamic. I don't recall the energy equation in this solver right now, it could be written in terms of kappa or making Pr appear or whatever... anyway if Pr is divided by rho in the equation, the actual kappa would be obtained from cinematic viscosity rather than dynamic. This leads me to the point: when you tried simulating with different rho values did you vary viscosity accordingly? Does this make any sense or sounds just like BS? ps: in my property file I don't even have the equationOfStaterho part, i just change viscosity values for different densities 

June 22, 2016, 10:10 
Problem with Boundary condition

#9 
New Member
Vishesh
Join Date: Jun 2016
Posts: 10
Rep Power: 5 
Hello All,
I am trying to run a case of chtMultiRegionSimpleFoam based on the multiRegionHeaterRadiation example. My case has 8 solid blocks inside air. The air and blocks are inside a metal cabinet, and also touch the cabinet. The cabinet is in the atmosphere. When i run the case, the temperature diverges and an error comes up. I am not able to diagnose the error. Please help! Time = 1 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0156926, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0130481, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0180424, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.0671467, No Iterations 1 Min/max T:300 7709.26 GAMG: Solving for p_rgh, Initial residual = 0.88219, Final residual = 0.00738372, No Iterations 6 time step continuity errors : sum local = 21.78, global = 18.8129, cumulative = 18.8129 Min/max rho:0.2 1.15862 Solving for fluid region domain2 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0184007, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.0246227, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0227786, No Iterations 1 [3] [3] [3] > FOAM FATAL ERROR: [3] Attempt to cast type compressible::turbulentTemperatureCoupledBaffleMix ed to type compressible::turbulentTemperatureRadCoupledMixed[0] [3] [3] From function refCast<To>(From&) [3] in file /home/kav9kor/OpenFOAM/OpenFOAM3.0.1/src/OpenFOAM/lnInclude/typeInfo.H at line 114. [3] 

June 23, 2016, 10:20 

#10  
New Member
Join Date: Mar 2015
Location: Earth yet
Posts: 25
Rep Power: 6 
Quote:
So, since you're trying to run a case of chtMultiRegionSimpleFoam based on the multiRegionHeaterRadiation example you probably forgot to adapt some part of one case to the other. Check the bc type in T field of /0/domain2 and /system/domain2/changeDictionaryDict (especially after running changeDictionary). Something else you could do is to see if you have the same issues with similar regions, like domains that have more or less the same bc types. Modify constant/regionProperties and put the similar region before your domain2, eg: solids(domain0 domain1 domain3 domain2) assuming 3 is similar to 2. Now the order of solving has been changed: if it runs until domain2 then domain 3 should be correctly set up. So copy and paste files from domain 3 folder to 2 and adapt it back with the correct values for domain 2. It's actually easier to do than to explain ... Hope it helps, Have fun! 

June 23, 2016, 12:26 

#11 
Member
Bruno
Join Date: Jun 2016
Location: Siegen, Germany
Posts: 59
Rep Power: 5 
Hi,
I'm trying to do something based on chtMultiRegionSimpleFoam/planeWall2D. I want to make a solid cylinder suspended in a body of air. To prevent errors I kept as many names as possible, deleting the bottomAir variable from the picture, using topAir as my air volume and wall as my cylinder. splitMeshRegions works okay and split my mesh correctly, but when running chtMultiRegionSimpleFoam I get the following error: Code:
Create time Create fluid mesh for region topAir for time = 0 Create solid mesh for region wall for time = 0 *** Reading fluid mesh thermophysical properties for region topAir Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:? #4 Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) at ??:? #5 Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) at ??:? #6 Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) at ??:? #7 ? at ??:? #8 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #9 ? at ??:? Floating point exception (core dumped) 

June 24, 2016, 01:44 

#12 
New Member
Vishesh
Join Date: Jun 2016
Posts: 10
Rep Power: 5 
Thank you coccone, I checked my boundary conditions and i found the problem. he issue has been resolved.
Hi Bruno, I had the exact same problem and the issue is in boundary conditions only. I believe you are using changeDictionary to write your BC files. In my case, i found that after running changeDict, all the boundaries were not coming in the boundary conditions file due to some error from my side. I would recommend you to compare your changeDict to the boundary conditions files in 0/topAir and other folders and check if any boundaries are not getting BC's. 

June 24, 2016, 01:52 

#13 
New Member
Vishesh
Join Date: Jun 2016
Posts: 10
Rep Power: 5 
Hi,
I am trying to run a case of chtMultiRegionSimpleFoam based on the multiRegionHeaterRadiation example. My case has 8 solid blocks inside air. The air and blocks are inside a metal cabinet, and also touch the cabinet. The cabinet is in the atmosphere. When i run the case, the temperature diverges and an error "Maximum number of iterations exceeded". Looking at the geometry, the spot where the temperature is diverging lies on the cell where 3 Boundary conditions intersect. I am not able to diagnose the error. Please help! Time = 4 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.494337, Final residual = 0.0365276, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.410604, Final residual = 0.00511476, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.533649, Final residual = 0.00156498, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 4.10453e05, No Iterations 1 Min/max T:6.25267e+07 1.94969e+11 GAMG: Solving for p_rgh, Initial residual = 0.677243, Final residual = 0.00620046, No Iterations 556 time step continuity errors : sum local = 8649.74, global = 8438.73, cumulative = 8436.92 Min/max rho:0.663714 0.717282 Solving for fluid region domain2 DILUPBiCG: Solving for Ux, Initial residual = 0.363923, Final residual = 0.0297, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.300749, Final residual = 0.0230535, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.440358, Final residual = 0.0310553, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0544437, Final residual = 0.00419095, No Iterations 1 Min/max T:294.252 349.985 GAMG: Solving for p_rgh, Initial residual = 0.796012, Final residual = 0.00544866, No Iterations 6 time step continuity errors : sum local = 2.17657, global = 8.83195e16, cumulative = 8436.92 Min/max rho:0.470228 1.34124 Time = 5 Solving for fluid region domain0 DILUPBiCG: Solving for Ux, Initial residual = 0.563651, Final residual = 0.00134662, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.554814, Final residual = 0.00039006, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.555083, Final residual = 0.000398982, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.405382, Final residual = 0.00225312, No Iterations 1 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam:erfectGas<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam:er fectGas<Foam::specie> >, Foam::sensibleEnthalpy>] in file /home/kav9kor/OpenFOAM/OpenFOAM3.0.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66. 

June 24, 2016, 11:23 

#14 
Member
Bruno
Join Date: Jun 2016
Location: Siegen, Germany
Posts: 59
Rep Power: 5 
Thanks Vishesh, it indeed had to do with a missing entry for one of my BCs in the ChangeDict. I hit the next problem though (regarding temperatures reaching negative values and then the simulation crashing) but I feel that's more relevant in another topic so I'll post it there.


June 24, 2016, 12:26 

#15 
New Member
Vishesh
Join Date: Jun 2016
Posts: 10
Rep Power: 5 
Hi Bruno,
you are welcome. I am also facing the negative temperature problem. I have figured that it is because velocity is diverging. You ll notice that velocity diverges in the 1st iteration and then temperature diverges. But i havent figured out the solution yet. Please send me the link of the thread where you will post your problem. 

February 6, 2017, 10:55 
chtMultiRegionSimpleFoam

#16 
New Member
Join Date: Sep 2013
Posts: 3
Rep Power: 8 
Hello, I want to simulate a similar case to this one. It is a solid box with a hole in the center containing air. Two faces have fixed temperature wall and others are adiabatics. I tried to download the case of this post but I couldn't. It will help me with my case, I am new with OF and I am a little lost. Thanks a lot!!


May 18, 2017, 19:04 

#17 
Member
alberto
Join Date: Apr 2016
Location: Mexico
Posts: 99
Rep Power: 5 
Hi i want to simulate flow through one pipe, with two obstacles, this obstacles are inmersed like in the figure.
1. I export with .msh 2. splitMeshRegions cellZones overwrite (fluid, porosity, solid) This separate my three domains, but the interior faces of my porosity became into wall. I want the fluid flow through the porous media. how can i fix this? 

Tags 
chtmultiregionsimplefoam, conjugate heat transfer, radiation, temperatureradcoupled, thermal conduction 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Radiation Modeling  Chris89  CFX  20  August 14, 2014 08:51 
Modeling both radiation and convection on surfaces  Ansys Transient Thermal R13  s.mishra  ANSYS  0  March 31, 2012 05:12 
Surface incident radiation  Pipiola  FLUENT  0  August 11, 2009 16:46 
DO Surface incident radiation Problem  Thomas  FLUENT  0  March 18, 2005 04:55 
Info: Short Course On Thermal Design of Electronic Equipment  Arnold Free  Main CFD Forum  0  August 10, 1999 11:18 