
[Sponsors] 
December 31, 2013, 11:51 

#21 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
1. Nope, I don't know analytical solution
2. i tried to run simplest case. When I get results for laminar, I will add turbulence. 3. blockMesh has only oneway mesh grading and I tried to do simplest case, consisting of only one block. Any way I believe i have small enough mesh, at least to get qualitatively results Bruno, thank you for your help! And have a happy New Year! Last edited by wyldckat; December 31, 2013 at 12:21. Reason: merged posts, which were 7 minutes apart ;) 

December 31, 2013, 14:42 

#22 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Hi Sergey,
Then I suggest that you step back a bit and change this case to a 2D or pseudo2D case (instead of "empty" patches, you can use "symmetry" patches on both sides), which makes it easier for you to increase/control the mesh refinement. The "plane wall 2D" case can work as a good start for this: http://openfoamwiki.net/index.php/Ge...__planeWall2D I say this because laminar simulations usually mean that you do not have a wall model that allows for a good estimation of how the turbulence flow behaves near the wall, e.g.: http://www.cfdonline.com/Wiki/Near...komega_models And you're welcome and have a happy new year as well! Best regards, Bruno
__________________


January 2, 2014, 14:26 

#23 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Hi Bruno!
I did a step back  returned back to air instead of water. And results look much better  at least they look like I expect from my intuition. The air at the inlet is cold and it is gradually heating while it is travelling through the fin. The fin itself looses more heat at the inlet, where the air is colder and looses less heat at the end where air is already warm and gradient is smaller. So it looks to me that I still have a problem with my material definition. Do you know if i have to change anything else apart from thermophysicalProperties and rho limits in fluidFomain/fvSolution in order to replace air with water? I think there is inconsistency between fixed density which I'm trying to use in my thermophysical model and compressible solver chtMultiRegionSimpleFoam. But looks like there must be a way to adapt the solver to run with constant density thermophysicalModel. Alternatively there might be a compressible model for water. Last edited by skuznet; January 3, 2014 at 11:53. Reason: update 

January 5, 2014, 11:19 

#24 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Hi Sergey,
OK, took me a while longer than I wanted to, but here goes the steps I suggest you try for the water case:
 edit: I was in a hurry and didn't properly post the images. I've updated them now and added a 3rd image.
The strange low temperature corners are due to a meshing issue that refineWallLayer does, when there is a patch with 90 degree corners, as shown in the second attached image. To avoid this, the Upatch would have to be split into 3 patches and each one refined once at a time. As for air vs water, the problem is as I've been trying to tell you: mesh and turbulence models are extremely important for this case! edit: And without turbulence models, the weight of responsibility falls all onto the mesh configuration. edit: As for speed: keep in mind that turbulence models were created precisely because it was not possible at that time to have meshes with several million cells. So consider turning it back on. Best regards, Bruno
__________________
Last edited by wyldckat; January 5, 2014 at 13:47. Reason: see the 3 "edit:" 

January 6, 2014, 11:17 

#25 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Bruno, thank you so much!
I will try it now. edit: Bruno, I tried to add turbulence and refinement. Adding turbulence didn't change anything, I have the same result: heat doesn't flow inside fluid region. Only boundaries are heated. (fimTurb.tar.gz) After adding refinement(with turbulence on) I can see refined mesh (looks great by the way!). But when I run it, the error appears: (fimTurbRefine.tar.gz) Code:
Time = 110 Solving for fluid region fluidDomain DILUPBiCG: Solving for Ux, Initial residual = 0.01734456, Final residual = 0.0003057888, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.01461149, Final residual = 0.0004831919, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.02473262, Final residual = 0.0004058105, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.002213193, Final residual = 5.1249e05, No Iterations 2 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /home/sergkuznet//OpenFOAM/OpenFOAM2.2.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double) const) const in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so" #5 in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam" #6 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #7 in "/home/sergkuznet/OpenFOAM/OpenFOAM2.2.x/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam" It looks like there is some problem with case setup. Last edited by skuznet; January 8, 2014 at 01:11. 

January 8, 2014, 11:42 

#26 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Hi Bruno!
chtMultiRegionSimpleFoam is based on buyantSimpleFoam. Why it uses different way of prescribing material properties  thermophysicalProperties instead of transportProperties? Is it possible to use transportProperties instead of thermophysicalProperties for the fluid region in chtMultiRegionSimpleFoam? Thank you! Sergey 

January 10, 2014, 15:03 

#27  
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Hi Sergey,
I won't be able to answer to post #25 any time soon Quote:
... Wait, wait... the tutorial "heatTransfer/buoyantSimpleFoam/hotRoom" also uses "constant/thermophysicalProperties". But the tutorial "heatTransfer/buoyantBoussinesqSimpleFoam/hotRoom" uses "constant/transportProperties". Therefore, you might be confusing buoyantSimpleFoam with buoyantBoussinesqSimpleFoam. Quoting from here: http://www.openfoam.org/features/standardsolvers.php Quote:
And honestly, I strongly suggest that you do more experiments with the "plane wall 2D" case and compare with the analytical solution, in order to ascertain if your guesses of what the heat transfer should look like, versus what you are currently getting Best regards, Bruno
__________________
Last edited by wyldckat; January 11, 2014 at 18:50. Reason: typo: it's "won't", not "wont" 

January 18, 2014, 12:56 

#28 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Hi Sergey,
I took a quick look at the cases and although you added the turbulence fields, you did not modify the file "constant/fluidDomain/RASProperties" As for the crash: the refinement I suggested was just a quick hack. The way that the corner cells are refined isn't very good, because it leads to the creation of some big shaped cells on the corners, which leads to distorting the flow. I don't have time to prove this, but as I've said before: it's best to first prove if things are working in the "plane wall 2D" case and comparing to the analytical solution, since that will give you a good insurance that things are being performed correctly or not. To understand better what I mean, have a look at this blog post: http://www.symscape.com/blog/cfdtip...ctivenewyear Best regards, Bruno
__________________


February 11, 2014, 10:18 
adding heat source to plane wall 2d case

#29 
New Member
sarvagy
Join Date: Jun 2013
Location: iit kanpur
Posts: 2
Rep Power: 0 
hello everyone,
i am new to solving heat transfer problems. i have to solve a problem of heat transfer in an electrical appliance , i want to use chtmultiregionfoam solver for it. my problem contains a heat source in the form of a resistance (heat = (i^2)*R joules/sec). for start I am looking at planewall2d case but i am not getting how to add a heat source term to planewall2d case. suppose for instance i want to add a heat source inside the wall at some location emitting q joules/sec of heat, how can i do this? is this possible? 

February 16, 2014, 14:57 

#30 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Greetings flash,
Sorry, I don't have time to create an example for this, but here are some directions:
Bruno
__________________


February 17, 2014, 02:12 

#31  
Member
Kumudu
Join Date: Oct 2013
Posts: 63
Rep Power: 11 
Quote:
Can you please share the file, if you add a heat source into any region as suggested by Bruno. I am really interested about it. Best regards, Kumudu 

February 17, 2014, 15:54 
2d case cht in curved channel

#32 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Hi Bruno!
I made a 2d case based on planeWall2D as you suggested. I just replaced top and bottom fluid with solid regions and solid wall with curved fluid channel. The bottom solid wall is heated to 500, the left and right solid wall are insulated, top solid wall has temperature 300. Velocity: Code:
U { internalField uniform (0.01 0 0); boundaryField { leftLet { type fixedValue; value uniform ( 0.1 0 0 ); } rightLet { type inletOutlet; inletValue uniform ( 0 0 0 ); value uniform ( 0.1 0 0 ); } "fluid_to_.*" { type fixedValue; value uniform (0 0 0); } } } Case runs well with velocity used in initial 2D case. However, the temperature profile doesn't have visible gradient, while I can see a significant variation in temperature on the boundaries of the fluid domain, therefore I would expect a significant gradient in the fluid volume as well. Sergey 

February 17, 2014, 16:19 
2d case cht in curved channel, slow flow

#33 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
I run then the same case, but with much slower flow:
Code:
U { internalField uniform (0.000001 0 0); boundaryField { leftLet { type fixedValue; value uniform ( 0.000001 0 0 ); } rightLet { type inletOutlet; inletValue uniform ( 0 0 0 ); value uniform ( 0.000001 0 0 ); } "fluid_to_.*" { type fixedValue; value uniform (0 0 0); } } Now I can see the nice gradient in temperature and velocity profile looks ok. However, pressure p_rgh doesn't change along the channel. And convergence is terrible: after Time=6822 number of iteration when solving for p_rgh increases and quickly becomes 1000 at every time step until the end. It seems that there is some problem with the solver. Code:
Time = 6822 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001313931, Final residual = 2.132327e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001355683, Final residual = 4.181906e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005424874, Final residual = 4.204827e05, No Iterations 1 Min/max T:302.2691 420.4573 GAMG: Solving for p_rgh, Initial residual = 0.001650452, Final residual = 1.622542e05, No Iterations 8 time step continuity errors : sum local = 2.284558e06, global = 1.620525e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628774, Final residual = 5.548561e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.1269 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001810846, Final residual = 4.49337e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0039 ExecutionTime = 104.75 s ClockTime = 105 s Time = 6823 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001314214, Final residual = 2.124361e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.00135596, Final residual = 4.152029e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005414751, Final residual = 4.192929e05, No Iterations 1 Min/max T:302.2697 420.4691 GAMG: Solving for p_rgh, Initial residual = 0.001648069, Final residual = 1.635356e05, No Iterations 9 time step continuity errors : sum local = 2.284934e06, global = 2.314783e09, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628817, Final residual = 5.548153e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.1477 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001810249, Final residual = 4.491468e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0054 ExecutionTime = 104.76 s ClockTime = 105 s Time = 6824 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001314334, Final residual = 2.116328e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001356137, Final residual = 4.122275e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.00054046, Final residual = 4.181034e05, No Iterations 1 Min/max T:302.2704 420.4808 GAMG: Solving for p_rgh, Initial residual = 0.001647746, Final residual = 1.631238e05, No Iterations 7 time step continuity errors : sum local = 2.310106e06, global = 1.07486e07, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628859, Final residual = 5.547744e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.1685 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001809652, Final residual = 4.489557e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.007 ExecutionTime = 104.78 s ClockTime = 105 s Time = 6825 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001314608, Final residual = 2.108353e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001356435, Final residual = 4.092932e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005394478, Final residual = 4.169154e05, No Iterations 1 Min/max T:302.271 420.4925 GAMG: Solving for p_rgh, Initial residual = 0.001646285, Final residual = 1.643818e05, No Iterations 45 time step continuity errors : sum local = 2.265405e06, global = 1.951309e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628902, Final residual = 5.547334e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.1893 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001809056, Final residual = 4.487734e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0086 ExecutionTime = 104.82 s ClockTime = 105 s Time = 6826 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001314799, Final residual = 2.100056e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001356629, Final residual = 4.063486e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005384321, Final residual = 4.157303e05, No Iterations 1 Min/max T:302.2717 420.5043 GAMG: Solving for p_rgh, Initial residual = 0.001647895, Final residual = 1.638582e05, No Iterations 13 time step continuity errors : sum local = 2.279589e06, global = 9.92179e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628944, Final residual = 5.546926e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.2101 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.000180846, Final residual = 4.485833e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0101 ExecutionTime = 104.84 s ClockTime = 105 s Time = 6827 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001314852, Final residual = 2.091747e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001356806, Final residual = 4.03387e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005374233, Final residual = 4.145507e05, No Iterations 1 Min/max T:302.2724 420.516 GAMG: Solving for p_rgh, Initial residual = 0.00164667, Final residual = 1.64259e05, No Iterations 29 time step continuity errors : sum local = 2.28877e06, global = 1.620525e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001628987, Final residual = 5.546517e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.2309 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001807866, Final residual = 4.48402e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0117 ExecutionTime = 104.86 s ClockTime = 105 s Time = 6828 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001315069, Final residual = 2.083812e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001357013, Final residual = 4.004651e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005364104, Final residual = 4.133708e05, No Iterations 1 Min/max T:302.273 420.5277 GAMG: Solving for p_rgh, Initial residual = 0.001645483, Final residual = 1.638643e05, No Iterations 21 time step continuity errors : sum local = 2.275193e06, global = 1.984058e09, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629029, Final residual = 5.546107e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.2517 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001807272, Final residual = 4.482179e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0133 ExecutionTime = 104.89 s ClockTime = 105 s Time = 6829 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001315206, Final residual = 2.075661e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001357208, Final residual = 3.975553e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005354014, Final residual = 4.121945e05, No Iterations 1 Min/max T:302.2737 420.5395 GAMG: Solving for p_rgh, Initial residual = 0.001645484, Final residual = 1.639848e05, No Iterations 27 time step continuity errors : sum local = 2.262239e06, global = 2.546556e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629071, Final residual = 5.545699e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.2725 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001806678, Final residual = 4.480382e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0148 ExecutionTime = 104.91 s ClockTime = 105 s Time = 6830 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001315388, Final residual = 2.067708e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001357459, Final residual = 3.946405e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005343923, Final residual = 4.110215e05, No Iterations 1 Min/max T:302.2743 420.5512 GAMG: Solving for p_rgh, Initial residual = 0.001644187, Final residual = 1.642512e05, No Iterations 240 time step continuity errors : sum local = 2.313747e06, global = 2.21583e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629113, Final residual = 5.54529e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.2932 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001806086, Final residual = 4.47858e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0164 ExecutionTime = 105.05 s ClockTime = 105 s Time = 6831 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.00131555, Final residual = 2.059634e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001357683, Final residual = 3.918141e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005333868, Final residual = 4.098513e05, No Iterations 1 Min/max T:302.275 420.5629 GAMG: Solving for p_rgh, Initial residual = 0.001643011, Final residual = 1.641557e05, No Iterations 487 time step continuity errors : sum local = 2.249288e06, global = 3.505659e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629155, Final residual = 5.544879e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.314 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001805493, Final residual = 4.476839e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0179 ExecutionTime = 105.3 s ClockTime = 105 s Time = 6832 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001315776, Final residual = 2.051749e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001357895, Final residual = 3.889592e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005323786, Final residual = 4.086815e05, No Iterations 1 Min/max T:302.2756 420.5746 GAMG: Solving for p_rgh, Initial residual = 0.001642862, Final residual = 1.641485e05, No Iterations 420 time step continuity errors : sum local = 2.221193e06, global = 3.770298e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629197, Final residual = 5.544468e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.3347 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.0001804901, Final residual = 4.475049e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0195 ExecutionTime = 105.53 s ClockTime = 105 s Time = 6833 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.001316075, Final residual = 2.044031e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.001358198, Final residual = 3.860973e06, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.0005313752, Final residual = 4.075142e05, No Iterations 1 Min/max T:302.2763 420.5863 GAMG: Solving for p_rgh, Initial residual = 0.001641225, Final residual = 1.711035e05, No Iterations 1000 time step continuity errors : sum local = 2.332723e06, global = 1.356003e08, cumulative = 7027.477 Min/max rho:1000 1000 Solving for solid region bottomSolid DICPCG: Solving for h, Initial residual = 0.0001629239, Final residual = 5.544055e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 381.3555 max(T) [0 0 0 1 0 0 0] 500 Solving for solid region topSolid DICPCG: Solving for h, Initial residual = 0.000180431, Final residual = 4.473332e07, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 308.0211 ExecutionTime = 106.05 s ClockTime = 106 s 

March 4, 2014, 14:15 

#34 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Hi Sergey,
I believe I've referred to comparing to analytical data a few times before, but it seems to have been for nothing. So this time I've done some online researching to give you some more basis.
If I'm not mistaken, the basic expression is this: Code:
(T(t)  T_inf)/(T_0  T_inf) = exp(b*t) where b= (h*A)/(rho*V*Cp) The idea here is that "t" is the time of exposure to the heat source, which in this case, is basically the time a certain streamline of fluid is near the wall. For example, at 0.01 m/s, it means that in 1 second the fluid travels 0.01 metre. Therefore, that's one point of measurement. I'm too tired now to do more graphs and math, but basically this gets you started on how to prove whether the solution gotten with the "chtMultiRegion*Foam" solvers is correct or not. Best regards, Bruno
__________________


March 7, 2014, 11:39 

#35 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Bruno:
Thank you so much for such a detailed reply! I will try to use this information for my case. 

March 20, 2014, 10:56 
chtmultregionfoam crashed

#36 
New Member
zhichao
Join Date: Jun 2012
Posts: 3
Rep Power: 12 
Dear Sergey and Bruno,
I've been tried to modified Sergey's example (fin2,at 19#) to chtMultiRegionFoam for a transient situation simulation for several days. Unfortunately,the program crashed after several time steps.Could you give me some help?I've upload my package. Thanks so much for your kind help. Code:
/**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.1.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 2.1.1221db2718bbb Exec : chtMultiRegionFoam Date : Mar 20 2014 Time : 22:20:08 Host : "localhost.localdomain" PID : 18099 Case : /home/zhichao/OpenFOAM/OpenFOAM2.1.1/run/heatTransfer/MSRRegonFoam/fin2 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Allowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region fluidDomain for time = 0 Create solid mesh for region solidDomain for time = 0 *** Reading fluid mesh thermophysical properties for region fluidDomain Adding to thermoFluid Selecting thermodynamics package hRhoThermo<pureMixture<constTransport<specieThermo<hConstThermo<incompressible>>>>> Adding to rhoFluid Adding to kappaFluid 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 to KFluid Adding to dpdtFluid *** Reading solid mesh thermophysical properties for region solidDomain Adding to thermos Constructed constSolidThermo with rho : rho [1 3 0 0 0 0 0] 8000 Cp : Cp [0 2 2 1 0 0 0] 450 K : K [1 1 3 1 0 0 0] 80 Hf : Hf [0 2 2 0 0 0 0] 1 emissivity : emissivity [0 0 0 0 0 0 0] 1 kappa : kappa [0 1 0 0 0 0 0] 0 sigmaS : sigmaS [0 1 0 0 0 0 0] 0 Region: fluidDomain Courant Number mean: 0.16666667 max: 0.16666667 Region: solidDomain Diffusion Number mean: 8.4931402e05 max: 0.00011111111 deltaT = 0.17985612 Region: fluidDomain Courant Number mean: 0.29976019 max: 0.29976019 Region: solidDomain Diffusion Number mean: 0.00015275432 max: 0.00019984013 deltaT = 0.17985612 Time = 0.179856 Solving for fluid region fluidDomain diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.8044614e08, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 2.3612832e09, No Iterations 2 DILUPBiCG: Solving for Uz, Initial residual = 0.99999996, Final residual = 1.5631079e08, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 0.99999994, Final residual = 8.7134678e10, No Iterations 2 Min/max T:299.99994 300 GAMG: Solving for p_rgh, Initial residual = 1, Final residual = 0.0042877256, No Iterations 8 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (fluidDomain): sum local = 0.0030054054, global = 4.8786781e07, cumulative = 4.8786781e07 GAMG: Solving for p_rgh, Initial residual = 0.94468661, Final residual = 102.55324, No Iterations 1000 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (fluidDomain): sum local = 17.56586, global = 2.0763789e05, cumulative = 2.1251657e05 Solving for solid region solidDomain DICPCG: Solving for T, Initial residual = 1, Final residual = 1.1180367e08, No Iterations 2 DICPCG: Solving for T, Initial residual = 3.0395743e09, Final residual = 3.0395743e09, No Iterations 0 Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 350 ExecutionTime = 15.03 s ClockTime = 15 s Region: fluidDomain Courant Number mean: 287.02986 max: 543.83794 Region: solidDomain Diffusion Number mean: 0.00015275432 max: 0.00019984013 deltaT = 9.9214854e05 Time = 0.179955 Solving for fluid region fluidDomain diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.0074809029, Final residual = 8.5987093e08, No Iterations 2 DILUPBiCG: Solving for Uy, Initial residual = 0.003465942, Final residual = 4.2461954e09, No Iterations 3 DILUPBiCG: Solving for Uz, Initial residual = 0.0029413719, Final residual = 4.0638087e08, No Iterations 2 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 3.7695281e08, No Iterations 3 Min/max T:300 20075.046 GAMG: Solving for p_rgh, Initial residual = 0.99999669, Final residual = 1.9534598e+115, No Iterations 1000 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (fluidDomain): sum local = 1.1630494e+15, global = 1, cumulative = 1.0000213 #0 Foam::error::printStack(Foam::Ostream&) in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 at sigaction.c:0 #3 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<double>&, Foam::Field<double> const&) const in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #8 in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam" #9 __libc_start_main in "/lib64/libc.so.6" #10 in "/home/zhichao/OpenFOAM/OpenFOAM2.1.1/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam" Last edited by wyldckat; March 23, 2014 at 17:26. Reason: Added [CODE][/CODE] 

March 23, 2014, 17:29 

#37  
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 126 
Quote:


March 23, 2014, 23:45 

#38 
Member
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 11 
Hi Zhichao!
Please find attached my latest attempt to do conjugate heat transfer in OpenFOAM. It is a transient case and uses STL geometry and snappyhexmesh utility. It runs ok, but I'm not sure if the results are correct. The velocity and pressure distributions seems ok, but temperature distribution doesn't look correct to me. It seems that heat doesn't flow well enough into the fluid region. Please let me know if you have any ideas about it or if you see any mistakes in me case. Sergey 

March 24, 2014, 04:07 
chtMultiRegionFoam problem

#39  
New Member
zhichao
Join Date: Jun 2012
Posts: 3
Rep Power: 12 
Quote:
Thanks a lot for you reply and kind help. which version of OF did you use?Since the project you've attached crashed on the step surfaceFeatureExtract. Best Regards Zhichao 

March 24, 2014, 07:15 
multiregionFoam

#40  
New Member
zhichao
Join Date: Jun 2012
Posts: 3
Rep Power: 12 
Quote:
Thanks a lot for you reply and help. In my opinion,the problem should be in the OF version and deltT setup. I've succeed the modificaion of multiRegionLiquidHeater to my application, although the result should not be completely correct.Later I will post my project and the construction tutorial from Gambit to chtmultiRegionFoam. Thanks to Mojtaba's tutorial and sergey's and you posts here. BTW,That's an interesting process to learn multiregion simulation on OF,it takes me around 3 weeks upto now. Best Regards zhichao 

Tags 
cht, solidfluid interface 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Conjugate Heat Transfer: Wall Heat Flux at Coupled Walls?  MaxHeat  FLUENT  4  September 14, 2017 11:44 
openfoam for heat transfer  kirankarki  OpenFOAM Running, Solving & CFD  29  February 12, 2015 19:46 
Conjugate Heat transfer in CFX  ksp1717  CFX  11  December 10, 2010 23:07 
Conjugate Heat Transfer of Motorized EGR  enr_venkat  CFX  1  October 12, 2010 19:17 
best mesh generator for conjugate heat transfer?  phsieh2005  Main CFD Forum  1  June 1, 2007 18:35 