CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   conjugate heat transfer in OpenFOAM (https://www.cfd-online.com/Forums/openfoam-solving/126652-conjugate-heat-transfer-openfoam.html)

 skuznet November 22, 2013 11:44

conjugate heat transfer in OpenFOAM

Dear FOAMers

I'm new in OpenFoam and would like to model steady state conjugate heat transfer(solid and fluid region) in a heat exchanger which consists of a few vertical metal plates attached to a horizontal plate with fluid flowing in gaps between plates.

My current experience with OpenFoam is restricted by “Lid-driven cavity flow tutorial” and “Stress analysis of a hole” tutorials. I know that there are “chtMultiRegionFoam” and “chtMultiRegionSimpleFoam” cases in /tutorials/heatTransfer/ folder. However, i didn't findt tutorials which would explain these cases and it's hard to understand what is going on in these cases without explanation.

I wonder if there is a step-by-step tutorial similar to “Lid-driven cavity” tutorial explaining conjugate heat transfer.
I also wonder if there are tutorials explaining
- how to create a case containing regions with different properties(fluid and solid), assign regions and boundaries;
- how to use conjugate heat transfer solvers;

My next step will be to model a steady state conjugate heat transfer in a porous material consisting of orthogonally interlaced cylindrical wires and fluid between them. I have a geometry for this case created in Abaqus.

I wonder if there is any way to translate my geometry from Abaqus to Open Foam preserving surfaces and regions definitions. Or what would be appropriate tool consistent with Open FOAM where I can create such geometry and define regions and surfaces?

Thank you!

 wyldckat November 22, 2013 17:30

Greetings skuznet and welcome to the forum!

Have a look into this (unofficial) tutorial: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D - and feel free to add information to it, when you've understood better how things work! :)

As for Abaqus, I have no idea if there is a direct way. You can try looking here in the forum. You can even use Google:
Code:

`site:www.cfd-online.com/Forums/ Abaqus OpenFOAM`
If there is no such direct conversion, have a look into this wiki page and the links therein: http://openfoamwiki.net/index.php/SnappyHexMesh

Best regards,
Bruno

 skuznet November 22, 2013 20:12

Bruno,
Actually I've run already the planeWall2D case. It didn't work. There was an error message in log.chtMultiRegionSipleFOAM

Code:

```/*---------------------------------------------------------------------------*\ | =========                |                                                | | \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          | |  \\    /  O peration    | Version:  2.2.2                                | |  \\  /    A nd          | Web:      www.OpenFOAM.org                      | |    \\/    M anipulation  |                                                | \*---------------------------------------------------------------------------*/ Build  : 2.2.2-9739c53ec43f Exec  : chtMultiRegionSimpleFoam Date  : Nov 22 2013 Time  : 19:54:37 Host  : "scyld.localdomain" PID    : 65269 Case  : /home/skuznetsov/OpenFOAM/RUN/planeWall2D nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time --> FOAM FATAL IO ERROR: keyword regions is undefined in dictionary "/home/skuznetsov/OpenFOAM/RUN/planeWall2D/constant/regionProperties" file: /home/skuznetsov/OpenFOAM/RUN/planeWall2D/constant/regionProperties from line 18 to line 20.     From function dictionary::lookupEntry(const word&, bool, bool) const     in file db/dictionary/dictionary.C at line 402. FOAM exiting```

and I also had error message when was trying to open results with paraview
Code:

```ERROR: In ..\..\..\src\VTK\IO\vtkOpenFOAMReader.cxx, line 7200 vtkOpenFOAMReaderPrivate (058864C8): Error reading line 58 of E:\Dropbox\planeWall2D\constant/bottomAir/polyMesh/boundary: Expected number, string or (, found ; ERROR: In ..\..\..\src\VTK\IO\vtkOpenFOAMReader.cxx, line 7200 vtkOpenFOAMReaderPrivate (058865E0): Error reading line 58 of E:\Dropbox\planeWall2D\constant/topAir/polyMesh/boundary: Expected number, string or (, found ; ERROR: In ..\..\..\src\VTK\IO\vtkOpenFOAMReader.cxx, line 7200 vtkOpenFOAMReaderPrivate (058866F8): Error reading line 47 of E:\Dropbox\planeWall2D\constant/wall/polyMesh/boundary: Expected number, string or (, found ; ERROR: In ..\..\..\src\VTK\Filtering\vtkExecutive.cxx, line 756 vtkCompositeDataPipeline (05BAEC40): Algorithm vtkPOpenFOAMReader(05AD8AA8) returned failure for request: vtkInformation (05B304F0)   Debug: Off   Modified Time: 95148   Reference Count: 1   Registered Events: (none)   Request: REQUEST_INFORMATION   FORWARD_DIRECTION: 0   ALGORITHM_AFTER_FORWARD: 1```

 wyldckat November 23, 2013 08:29

Hi Sergey,

Have a look into the wiki page again: http://openfoamwiki.net/index.php/Ge..._-_planeWall2D - I've added an adapted case for OpenFOAM 2.2.

Best regards,
Bruno

 skuznet November 23, 2013 13:14

Awesome! Thank you Bruno!

 skuznet November 23, 2013 19:38

Bruno,
the case now seems to run well.
But when I'm trying to open it paraview I still can't see anything.
I downloaded all case files on my pc and trying to open it with paraview (i tried versions 3.81, 3.12, 3.98.0).
-I choose .OpenFOAM file to open,
-check Mesh Regions box
-and click Apply
and nothing appears.

I see message
Code:

```ERROR: In ..\..\..\src\VTK\IO\vtkOpenFOAMReader.cxx, line 4498 vtkOpenFOAMReaderPrivate (05944570): Error opening E:\Dropbox\planeWall2D\constant/polyMesh/faces.gz: Can't open. If you are trying to read a parallel decomposed case, set Case Type to Decomposed Case. ERROR: In ..\..\..\src\VTK\Filtering\vtkExecutive.cxx, line 756 vtkCompositeDataPipeline (05CB2EA0): Algorithm vtkPOpenFOAMReader(05B9E960) returned failure for request: vtkInformation (05BE93C8)   Debug: Off   Modified Time: 98373   Reference Count: 1   Registered Events: (none)   Request: REQUEST_DATA   FROM_OUTPUT_PORT: 0   FORWARD_DIRECTION: 0   ALGORITHM_AFTER_FORWARD: 1```
I can get rid off this message by choosing Case Type: Decomposed Case
but still don't see anything.

The time panel is not active, I can't change time and in Color panel I can't choose anything except Solid Color.

If I open the cavity case, then I can see geometry and pressure and velocity distributions.

 wyldckat November 24, 2013 08:58

Hi Sergey,

Please, when posting code and error outputs, please use the "[CODE]" markers, as explained in the second link of my signature. And you can edit your previous posts as well, so please add this marker to them, to make it easier to read the posts.

Regarding your question: the "*.gz" files might not be opened with success with ParaView's internal ".foam" reader. First unzip the files; on Linux, you can run this command:
Code:

`find . -name "*.gz" | xargs gunzip`
Then you can open the case with ParaView's internal reader.

Best regards,
Bruno

 skuznet December 5, 2013 00:49

Bruno, thank you for the help!
I installed ubuntu, openfoan and paraview on my homecomputer and now it works well. I can run case planeWall2d and multiRegionHeatre and can open results.
I think my previous issues with opening results were because I was opening them in Windows and files were not transferred or opened correctly in paraview under windows.

 skuznet December 10, 2013 13:36

Dear Bruno:

Thank you for adapting the planeWall2D.
I was able to run this case and I got some basic understanding how it works.
Based on planeWall2D tutorial I was able to set up and run a simple 3d fin case - there is a fin which is heated from the bottom and the fluid flow removes the heat from the fin. I was able to run it with air and it looks ok.

However, when I try to put water instead of air by replacing themoPhysicalProperties with file from

HTML Code:

`/chtMultiRegionFoam/multiRegionLiquidHeater/constant/bottomWater/thermophysicalProperties`
:
Code:

```\*---------------------------------------------------------------------------*/ FoamFile {     version    2.0;     format      ascii;     class      dictionary;     object      thermophysicalProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType {     type            heRhoThermo;     mixture        pureMixture;     transport      const;     thermo          hConst;     equationOfState rhoConst;     specie          specie;     energy          sensibleEnthalpy; } mixture {     specie     {         nMoles          1;         molWeight      18;     }     equationOfState     {         rho            1000;     }     thermodynamics     {         Cp              4181;         Hf              0;     }     transport     {         mu              959e-6;         Pr              6.62;     } } // ************************************************************************* //```

Something is going wrong. Open FOAM starts solving it but during iterations my temperature (minimal temperature in solid and in fluid domains) is reducing, which should not occur, since I have a heater.
At the end temperature in fluid domain becomes even negative, and OpenFOAM crashes.

Can you please tell me if I have to change anything else in my case when I replaced my thermophysicalProperties file with water? I guess the problem might be because thermophysicalProperties for water has different equation of state - rhoConst instead of perfectGas.

Thank you!

 wyldckat December 10, 2013 17:55

Hi Sergey,

A few questions:
1. Which specific multi-region solver are you using?
2. What is the flow speed for each fluid?
3. Have you checked the solid's characteristics? It might be bleeding energy due to very low or high heat transfer factors.
Best regards,
Bruno

 skuznet December 10, 2013 19:53

1. I'm using chtMultiRegionSimpleFoam solver, but the thermophysicalProperties file was taken from the example for chtMultiRegionFoam.

2. I have only one fluid - water, the inlet velocity is 0.1 m/s, while the size of the fin 1x1x3 m.

3. I didn't check the solid. How can I check?

The very first fluid iteration gives also very high temperature 2000, while initial temperature was 300 and temperature of the warmed surface of solid is 350:
Code:

```/*---------------------------------------------------------------------------*\ | =========                |                                                | | \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          | |  \\    /  O peration    | Version:  2.2.x                                | |  \\  /    A nd          | Web:      www.OpenFOAM.org                      | |    \\/    M anipulation  |                                                | \*---------------------------------------------------------------------------*/ Build  : 2.2.x-37940e0cd1ae Exec  : /home/sergkuznet/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam Date  : Dec 11 2013 Time  : 16:43:49 Host  : "ubuntu" PID    : 8592 Case  : /home/sergkuznet/OpenFOAM/run/fin2R_initial nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied 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 {     type            heRhoThermo;     mixture        pureMixture;     transport      const;     thermo          hConst;     equationOfState rhoConst;     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 Radiation model not active: radiationProperties not found Selecting radiationModel none     Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region solidDomain     Adding to thermos Selecting thermodynamics package {     type            heSolidThermo;     mixture        pureMixture;     transport      constIso;     thermo          hConst;     equationOfState rhoConst;     specie          specie;     energy          sensibleEnthalpy; }     Adding to radiations Radiation model not active: radiationProperties not found Selecting radiationModel none     Adding fvOptions No finite volume options present Time = 1 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.041964, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0001767454, No Iterations 2 DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0003058668, No Iterations 2 DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.02843725, No Iterations 1 Min/max T:299.9999 2035.089 GAMG:  Solving for p_rgh, Initial residual = 0.8476081, Final residual = 0.003588793, No Iterations 11 time step continuity errors : sum local = 0.7781759, global = -0.07076251, cumulative = -0.07076251 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.05509895, 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] 350 ExecutionTime = 1.39 s  ClockTime = 1 s Time = 2 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 0.3551669, Final residual = 0.003849144, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 0.05855359, Final residual = 0.001012355, No Iterations 1 DILUPBiCG:  Solving for Uz, Initial residual = 0.02422332, Final residual = 0.0003484752, No Iterations 1 DILUPBiCG:  Solving for h, Initial residual = 0.5433119, Final residual = 0.007134343, No Iterations 1 Min/max T:264.6221 2035.089 GAMG:  Solving for p_rgh, Initial residual = 0.04481994, Final residual = 0.0004256873, No Iterations 18 time step continuity errors : sum local = 3.010856, global = 1.085556, cumulative = 1.014794 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 0.189656, Final residual = 0.014255, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 299.7434 max(T) [0 0 0 1 0 0 0] 350 ExecutionTime = 1.92 s  ClockTime = 2 s Time = 3 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 0.1454075, Final residual = 0.001948315, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 0.09988127, Final residual = 0.001433494, No Iterations 1 DILUPBiCG:  Solving for Uz, Initial residual = 0.0186658, Final residual = 0.0001720673, No Iterations 1 DILUPBiCG:  Solving for h, Initial residual = 0.3185567, Final residual = 0.01199445, No Iterations 1 Min/max T:244.3615 1008.353 GAMG:  Solving for p_rgh, Initial residual = 0.2012721, Final residual = 0.001699132, No Iterations 18 time step continuity errors : sum local = 0.8901295, global = 0.2734903, cumulative = 1.288284 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 0.09596577, Final residual = 0.00727127, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 299.396 max(T) [0 0 0 1 0 0 0] 350 ExecutionTime = 2.44 s  ClockTime = 2 s```

 skuznet December 11, 2013 00:34

Bruno,

I can see some inconsistency in what i'm trying to do:
the chtMultiRegionSimpleFoam in compressible solver, and in thermophysicalProperties which I used the density is constant. Can it be the reason for temperature decrease and OF crash?

 wyldckat December 15, 2013 15:28

Hi Sergey,

Quote:
 Originally Posted by skuznet (Post 465816) 2. I have only one fluid - water, the inlet velocity is 0.1 m/s, while the size of the fin 1x1x3 m.
The fin is quite big. It's easy for it to either cool down too much or warm up too much, depending on the thermodynamic properties defined for it.

Quote:
 Originally Posted by skuznet (Post 465816) 3. I didn't check the solid. How can I check?
Check the file "constant/wall/thermophysicalProperties".

Quote:
 Originally Posted by skuznet (Post 465816) The very first fluid iteration gives also very high temperature 2000, while initial temperature was 300 and temperature of the warmed surface of solid is 350: Code: ```/*---------------------------------------------------------------------------*\ | =========                |                                                | | \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          | |  \\    /  O peration    | Version:  2.2.x                                | |  \\  /    A nd          | Web:      www.OpenFOAM.org                      | |    \\/    M anipulation  |                                                | \*---------------------------------------------------------------------------*/ Build  : 2.2.x-37940e0cd1ae Exec  : /home/sergkuznet/OpenFOAM/OpenFOAM-2.2.x/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam Date  : Dec 11 2013 Time  : 16:43:49 Host  : "ubuntu" PID    : 8592 Case  : /home/sergkuznet/OpenFOAM/run/fin2R_initial nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring run-time modified files using timeStampMaster allowSystemOperations : Disallowing user-supplied 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 {     type            heRhoThermo;     mixture        pureMixture;     transport      const;     thermo          hConst;     equationOfState rhoConst;     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 Radiation model not active: radiationProperties not found Selecting radiationModel none     Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region solidDomain     Adding to thermos Selecting thermodynamics package {     type            heSolidThermo;     mixture        pureMixture;     transport      constIso;     thermo          hConst;     equationOfState rhoConst;     specie          specie;     energy          sensibleEnthalpy; }     Adding to radiations Radiation model not active: radiationProperties not found Selecting radiationModel none     Adding fvOptions No finite volume options present Time = 1 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.041964, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0001767454, No Iterations 2 DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.0003058668, No Iterations 2 DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.02843725, No Iterations 1 Min/max T:299.9999 2035.089 GAMG:  Solving for p_rgh, Initial residual = 0.8476081, Final residual = 0.003588793, No Iterations 11 time step continuity errors : sum local = 0.7781759, global = -0.07076251, cumulative = -0.07076251 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 1, Final residual = 0.05509895, 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] 350 ExecutionTime = 1.39 s  ClockTime = 1 s Time = 2 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 0.3551669, Final residual = 0.003849144, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 0.05855359, Final residual = 0.001012355, No Iterations 1 DILUPBiCG:  Solving for Uz, Initial residual = 0.02422332, Final residual = 0.0003484752, No Iterations 1 DILUPBiCG:  Solving for h, Initial residual = 0.5433119, Final residual = 0.007134343, No Iterations 1 Min/max T:264.6221 2035.089 GAMG:  Solving for p_rgh, Initial residual = 0.04481994, Final residual = 0.0004256873, No Iterations 18 time step continuity errors : sum local = 3.010856, global = 1.085556, cumulative = 1.014794 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 0.189656, Final residual = 0.014255, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 299.7434 max(T) [0 0 0 1 0 0 0] 350 ExecutionTime = 1.92 s  ClockTime = 2 s Time = 3 Solving for fluid region fluidDomain DILUPBiCG:  Solving for Ux, Initial residual = 0.1454075, Final residual = 0.001948315, No Iterations 1 DILUPBiCG:  Solving for Uy, Initial residual = 0.09988127, Final residual = 0.001433494, No Iterations 1 DILUPBiCG:  Solving for Uz, Initial residual = 0.0186658, Final residual = 0.0001720673, No Iterations 1 DILUPBiCG:  Solving for h, Initial residual = 0.3185567, Final residual = 0.01199445, No Iterations 1 Min/max T:244.3615 1008.353 GAMG:  Solving for p_rgh, Initial residual = 0.2012721, Final residual = 0.001699132, No Iterations 18 time step continuity errors : sum local = 0.8901295, global = 0.2734903, cumulative = 1.288284 Min/max rho:2 2 Solving for solid region solidDomain DICPCG:  Solving for h, Initial residual = 0.09596577, Final residual = 0.00727127, No Iterations 1 Min/max T:min(T) [0 0 0 1 0 0 0] 299.396 max(T) [0 0 0 1 0 0 0] 350 ExecutionTime = 2.44 s  ClockTime = 2 s```
Then there is something very wrong with the boundary conditions.

Quote:
 Originally Posted by skuznet (Post 465828) I can see some inconsistency in what i'm trying to do: the chtMultiRegionSimpleFoam in compressible solver, and in thermophysicalProperties which I used the density is constant. Can it be the reason for temperature decrease and OF crash?
:confused: Which specific file are you referring to? Because the file "constant/thermophysicalProperties" is not used by these multi-region solvers!

Best regards,
Bruno

 skuznet December 16, 2013 16:40

1 Attachment(s)
Bruno,

I took the file "constant/solidDomain/thermophysicalProperties" from multiRegionHeater tutorial, and it looks OK to me.

I was reffering to the file "constant/fluidDomain/thermophysicalProperties", which describes my fluid properties.

I can't find out what is wrong with this case. Could you please take a look at it?

Thank you!

 skuznet December 27, 2013 15:35

5 Attachment(s)
Dear Bruno, I've modified file fluidRegion/fvSolutions - changed rhoMin and rhoMax so that constant value of rho prescribed in thermophysicalProperties fits this interval

Code:

```SIMPLE {     momentumPredictor on;     nNonOrthogonalCorrectors 0;     pRefCell        0;     pRefValue      100000;     rhoMin          rhoMin [1 -3 0 0 0] 999;     rhoMax          rhoMax [1 -3 0 0 0] 1001; }```
Now chtMultiRegionSimpleFoam doesn't crash, but results do not look correct.

Temperature distribution in the whole model: Temperature_WholeModel_crop.jpg
Temperature in fluid domain: T_fluid_cut.jpg
Fluid velocity in fluid domain: U_fluid_cut.jpg
Pressure_rgh in fluid domain: p_rgh_fluid_cut.jpg
the case: fin2.tar.gz

The p_rgh distribution is obviously not realistic.
One can see that fluid velocity in the vicinity of top surface changes smoothly from 0 to some value, however in the vicinity of the bottom boundary such a smooth transition doesn't exist, while it should be same because the wall condition is prescribed at the top and there is fluid solid interface at the bottom, which is equivalent to wall condition.

 wyldckat December 29, 2013 16:17

Hi Sergey,

Sorry, I only managed to look at this today. I've had some very busy weeks.

I've done the following modifications:
Code:

```diff -ur fin2_orig/system/fluidDomain/fvSolution fin2/system/fluidDomain/fvSolution --- fin2_orig/system/fluidDomain/fvSolution    2013-11-26 20:37:33.000000000 +0000 +++ fin2/system/fluidDomain/fvSolution    2013-12-29 20:06:05.448515088 +0000 @@ -52,9 +52,9 @@     momentumPredictor on;     nNonOrthogonalCorrectors 0;     pRefCell        0; -    pRefValue      100000; -    rhoMin          rhoMin [1 -3 0 0 0] 0.2; -    rhoMax          rhoMax [1 -3 0 0 0] 2; +    pRefValue      1e5; +    rhoMin          rhoMin [1 -3 0 0 0] 999; +    rhoMax          rhoMax [1 -3 0 0 0] 1001;  }```
If you notice, the only major difference from your latest change is the "pRefValue", where you had "100000", which is 10 times the value I have of "1e5". And "1e5" is the value used in the initial boundary conditions for the pressure fields.

Beyond this, the case is still running on my computer, so I don't if this fixed the problem or not.

edit: Something is still wrong with the pressure, because in the solid region the pressure is still set to 100000 Pa. I've stopped the simulation on my computer and will wait for feedback from your side.

Best regards,
Bruno

 skuznet December 30, 2013 01:09

I did try to run already with
rhoMin rhoMin [1 -3 0 0 0] 999;
rhoMax rhoMax [1 -3 0 0 0] 1001;
and the results do not look correct, they are shown on the previous post (#15).

regarding pressure - 100000 (five zeros) is exactly 1e5 which is athmospheric pressure, so this should be ok,

However, I discovered that in changeDictionaryDict for fluid region i misspelled the inlet patch name for temperature BC:

Code:

```fron             {                 type            fixedValue;                 value          uniform 300;             }```
while should be

Code:

```front             {                 type            fixedValue;                 value          uniform 300;             }```
Not sure I it can be the reason of strange results. Will run it again.

I don't understand the meaning of some BC used in planeWall2D and multiRegionHeater, I just copied them to my case without understanding. So not sure if I'm using them properly.

for example for velocity
Code:

```U     {         internalField  uniform (0 0 0.1);         boundaryField         {             ".*"             {                 type            fixedValue;                 value          uniform (0 0 0);             }             front             {                 type            fixedValue;                 value          uniform ( 0 0 0.1 );             }```
I prescribe fixed velocity at the incled (front) and fixed values (zeros) at the walls. But don't understand the outlet BC (back)

Code:

```          back             {                 type            inletOutlet;                 inletValue      uniform ( 0 0 0 );                 value          uniform ( 0 0 0.1 );             }         }     }```
How does it work?
Similar BC for temperature are used at the outlet.

I also don't understand the BC used at the fluid-solid interface.
For temperature:

Code:

```"fluidDomain_to_.*"             {                 type            compressible::turbulentTemperatureCoupledBaffleMixed;                 neighbourFieldName T;                 kappa          fluidThermo;                 kappaName      none;                 value          uniform 300;             }```
why it contains fixed value 300? It should not be fixed.

 wyldckat December 30, 2013 07:58

Hi Sergey,

Quote:
 Originally Posted by skuznet (Post 468057) regarding pressure - 100000 (five zeros) is exactly 1e5 which is athmospheric pressure, so this should be ok,
Sorry about that. It's really weird, because it looked like 1e6 to me every time I looked at it :(
Wow... now that I think about it, I did have a weird numeric mess in my mind.

Quote:
 Originally Posted by skuznet (Post 468057) I prescribe fixed velocity at the incled (front) and fixed values (zeros) at the walls. But don't understand the outlet BC (back) Code: ```          back             {                 type            inletOutlet;                 inletValue      uniform ( 0 0 0 );                 value          uniform ( 0 0 0.1 );             }         }     }``` How does it work? Similar BC for temperature are used at the outlet.
• The fixed speed set to "0" at the walls is due to the no-slip condition: http://en.wikipedia.org/wiki/No-slip_condition
• The ".*" is a regular expression for selecting all names: http://en.wikipedia.org/wiki/Regular_expression
• The fixed speed at the inlet... well, it's go to be something coming in :)
• As for the "inletOutlet", have a look at the User Guide: http://www.openfoam.org/docs/user/boundaries.php
• Mmm... not much of an explanation there :( Essentially the "inletOutlet" and "outletInlet" boundary conditions allow you to have a valve like condition: when it's meant to flow freely, it does; when the flow is reversed, use this fixed value I'm telling you to use.
• In this particular case, by defining "inletValue uniform ( 0 0 0 )", means that there is no reverse flow allowed. For example, if "zeroGradient" was used and in case for whatever reason there is a vortex building up and going out the outlet, it would lead to having fluid flowing outside and coming back in, through the same patch. With the configured "inletOutlet", this is not allowed.
• The "value" entry for "inletOutlet" is used only as the initial value. After the first iteration, it's always the result of the simulation.

Quote:
 Originally Posted by skuznet (Post 468057) I also don't understand the BC used at the fluid-solid interface. For temperature: Code: ```"fluidDomain_to_.*"             {                 type            compressible::turbulentTemperatureCoupledBaffleMixed;                 neighbourFieldName T;                 kappa          fluidThermo;                 kappaName      none;                 value          uniform 300;             }``` why it contains fixed value 300? It should not be fixed.
In this case, the "value" entry is also only the initial value. It would only be a fixed value if the "type" of the boundary condition was "fixedValue".

Did you go properly study the tutorials in the User Guide? Or did you just go through them as fast as you could? ;)

Best regards,
Bruno

 skuznet December 30, 2013 15:21

1 Attachment(s)
Bruno, thanks for explanation.

In tutorial http://www.openfoam.org/docs/user/boundaries.php
inletOutlet and solid-surface BC are not well detailed, your explanation is better.

I fixed the misspelled patch name and run case again. But result still doesn't look correct, in fact it became even worse - I don't see anymore temperature variation inside fluid domain, only on boundaries.

Can you please explain to me also the pressure BC?

HTML Code:

```p_rgh     {         internalField  uniform 1e5;         boundaryField         {             ".*"             {                 type            fixedFluxPressure;                 value          uniform 1e5;             }             back             {                 type            fixedValue;                 value          uniform 1e5;             }         }     }     p     {         internalField  uniform 1e5;         boundaryField         {             ".*"             {                 type            calculated;                 value          uniform 1e5;             }             back             {                 type            calculated;                 value          uniform 1e5;             }         }     }```

 wyldckat December 30, 2013 16:58

Quoting Tobi:
Quote:
 Originally Posted by Tobi (Post 467108) p = total pressure p_rgh = p - rho *gh (total pressure - hydrodynamic pressure)