|
[Sponsors] |
June 6, 2018, 06:31 |
turbulentTemperatureCoupledBaffleMixed
|
#1 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
I'm running a chtMultiRegionSimpleFoam with a tetrahedral mesh made in Salome. The model consists of a small number of connected solids surrounded with air.
One solid has a volume heat generation defined as a scalarSemiImplicitSource in fvOptions. Solids and fluids are connected using compressive::turbulentTemperatureCoupledBaffleMixe d patch and the solver runs but it looks like the patches try to hold the temperature I set as initial guess. Obviously this never converges and temperatures on the boundary don't rise as expected. How do I set BC for connected patches without setting a fixed temperature? |
|
June 6, 2018, 09:57 |
|
#2 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
Here are the results from one timestep. Heat source is in the "coil" region. "Air" surrounds the whole assembly and cooler is a big aluminium piece that should disperse heat into surrounding air.
Code:
Time = 266 Solving for fluid region air DILUPBiCGStab: Solving for Ux, Initial residual = 0.00595372, Final residual = 0.0002666618, No Iterations 1 DILUPBiCGStab: Solving for Uy, Initial residual = 0.005627012, Final residual = 0.0002532324, No Iterations 1 DILUPBiCGStab: Solving for Uz, Initial residual = 0.006628133, Final residual = 0.0002960641, No Iterations 1 DILUPBiCGStab: Solving for h, Initial residual = 0.002119841, Final residual = 9.896488e-005, No Iterations 1 Min/max T:300 342.3529 GAMG: Solving for p_rgh, Initial residual = 0.03928421, Final residual = 0.0002773877, No Iterations 3 time step continuity errors : sum local = 0.0006090867, global = 5.509568e-012, cumulative = -2.228852e-010 Min/max rho:1.016304 1.159781 Solving for solid region cooler DICPCG: Solving for h, Initial residual = 0.001841032, Final residual = 2.965676e-005, No Iterations 2 Min/max T:300 300.1434 Solving for solid region coil DICPCG: Solving for h, Initial residual = 0.001263771, Final residual = 3.696184e-005, No Iterations 2 Min/max T:300.0023 359.0179 ExecutionTime = 2512.975 s ClockTime = 2513 s |
|
June 6, 2018, 10:17 |
|
#3 |
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 21 |
Well this isn't enough information to help. Are you certain, that your thermal conductivity in thermoPhysicalProperties is correctly defined. Maybe you are just solving something which i inherently slow to heat up. Or your temperature difference is minimal because of a high flow rate. Or you are drastically relaxing the temperature solution....All I can do here is speculate
|
|
June 6, 2018, 11:13 |
|
#4 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
I'll share the whole case. I again regret naming stuff in my language, let me translate here for you. I simplified the description in the above post, there's four solids instead of two, but the rest is the same, including the results.
I got approximate thermophysical values for mentioned materials. It's a test case and I'll do more research later when this runs OK. I can't attach a mesh, I can only give you a screenshot. I experimented with various mesh densities from 100 000 points to 10 million, same results in every case. I also tried different boundary conditions for U but as expected, it doesn't affect heat transfer between solids. I appreciate any advice you can give me. Thanks! |
|
June 17, 2018, 09:41 |
|
#5 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
I think I figured it out.
First, meshing. My STL files were assembled from different patches made in SALOME so their normals weren't all pointing in the same direction. There's a utility for cases like this: surfaceOrient. I also had a separate STL file for surrounding 'air' which snappy couldn't snap to. I just removed that from meshing so now background mesh made in blockMesh is what my 'air.stl' used to be. I use topoSet to create a separate zone from background mesh then run splitMeshRegions. Here's my topoSetDict: Code:
FoamFile { version 2.0; format ascii; class dictionary; object topoSetDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // actions ( { name air; type cellSet; action new; source zoneToCell; sourceInfo { name ".*"; } } { name air; type cellSet; action invert; } ); In the end, I found a template that will be used in foamSetupCHT utility in the next release (6?). Though it's not in the current release one can still use all schemes and other settings, including boundary conditions: https://github.com/OpenFOAM/OpenFOAM...singleFluidCHT |
|
November 11, 2020, 12:02 |
|
#6 | |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
Quote:
Hi i have a similar problem. For my case, a very simple case of solid cooling by air, i am not able to see any change in the outlet temperature of air and it always remains around initial value. No matter how much i increase the value of heat flux in fvOptions, there is no change in outlet temperature or the maximum temperature of the solid. It seems to me that the solver is not reading fvOptions at all, even if i enter absurd values in fvOptions, it runs and the outlet temperature and solid temperature just remains the same as the initial value. I have tried many things but nothing helped. Thanks in advance for any suggestions Regards |
||
November 11, 2020, 12:13 |
|
#7 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
can you share your case?
are your fvOptions in constant/<region> or in global constant folder? |
|
November 11, 2020, 12:32 |
|
#8 | |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
Quote:
I have tried all the possible locations of fvOptions. Here is the case https://drive.google.com/file/d/1Hcs...ew?usp=sharing I have used blockmesh toposet and splitmeshregions to set up the mesh. Thanks a lot again cheers |
||
November 11, 2020, 12:50 |
|
#9 |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
it seems to me that there is no problem with the case, its just its taking too long to converge and to settle down, i guess i need to meddle with the relaxation factors etc !!! anyways, i will really appreciate your input !!
thanks |
|
November 11, 2020, 16:30 |
|
#10 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
To speed up convergence on solids somewhat, try forcing more iterations on those regions. Set nNonOrthogonalCorrectors to a higher-than-needed value. For instance, system/heatsink/fvSolution:
Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 5 | | \\ / A nd | Web: www.OpenFOAM.org | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "h.*" { solver PCG; preconditioner DIC; tolerance 1e-08; relTol 0.001; } } SIMPLE { nNonOrthogonalCorrectors 20; } relaxationFactors { equations { h 1.0; } } // ************************************************************************* // |
|
November 12, 2020, 06:20 |
|
#11 | |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
Quote:
thanks a lot , i will do that!! can i request you to have a look at my case, just for your input. thanks !!! |
||
November 12, 2020, 07:01 |
|
#12 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
Sure, but you'll have to share it with me
|
|
November 12, 2020, 07:04 |
|
#13 |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
||
November 12, 2020, 08:06 |
|
#14 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
Ah, sorry, I never noticed that link.
I took a look, here are some comments:
Here's the system/diode/fvOptions file: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v2006 | | \\ / A nd | Website: www.openfoam.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object fvOptions; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // heatsource_diode { type scalarSemiImplicitSource; active true; scalarSemiImplicitSourceCoeffs { selectionMode all; // all, cellSet, cellZone, points volumeMode absolute; // absolute; injectionRateSuSp { h (500000 0); } } } Hope this helps. |
|
November 12, 2020, 08:37 |
|
#15 | |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
Quote:
Hello Thanks a lot for the reply. I will change the blockMesh Yes you are right, after trying for all possible locations, i feel FvOptions in system/region works but i am not sure. I am not able to see any change in the temperature of air outlet and solid (No matter how big is the value of the heat flux lol). I must be doing something completely wrong, i do not know what for the moment. Yes i am trying with a steady solver. But no difference. anyways i will let you know if i succeed . thanks a lot |
||
November 12, 2020, 08:44 |
|
#16 |
Senior Member
Nejc
Join Date: Feb 2017
Location: Slovenia
Posts: 196
Rep Power: 9 |
It works for me, see your updated case in attachment. I stripped mesh files.
Another advice, create a sort of Allrun script so you (or whoever helps you) don't have to manually execute the whole procedure. |
|
November 12, 2020, 09:15 |
|
#17 | |
Member
Bineet Mehra
Join Date: Aug 2013
Posts: 61
Rep Power: 13 |
Quote:
cheers |
||
|
|