|
[Sponsors] |
Two-sided Wall Heat Transfer BC - No Separate Solid Mesh and No Heat Transfer Coeff |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 15, 2010, 21:36 |
Two-sided Wall Heat Transfer BC - No Separate Solid Mesh and No Heat Transfer Coeff
|
#1 | |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Dear Foamers and Experts,
I have been trying to perform a CFD for compressible internal flow (using rhoSimpleFoam). However, I have been having difficulty implementing the right BC for modelling heat transfer through a 'two-sided' thin wall. The wall does not have thickness (only surface mesh). However, it needs to model heat transfer from one side to another side (this is similar to having a 'shadow wall' in Fluent), without having a separate solid mesh region. Quote:
Additionally, the ability to compute 2D heat conduction in the thin shell is important. All these will need to be achieved without the need to have a separate solid mesh region, and readily implementable with rhoSimpleFoam and rhoSonicFoam solver. I believe no BC is readily available in OF that is able to do this without the need to have a separate solid mesh. I have attempted to model the above requirements using wallHeatTransfer, groovyBC, and fixedGradient, all to no satisfactory result. Could anyone please advice me if this is readily achievable in OpenFOAM without further development of a new BC? Thank you very much in advanced for your response. Best Regards, Stefano Wahono |
||
September 17, 2010, 02:09 |
|
#2 |
Senior Member
ata kamyabi
Join Date: Aug 2009
Location: Kerman
Posts: 323
Rep Power: 18 |
Hi Stefano
I think you are right. As I know there in no such a BC in OF. Best regards Good luck Ata |
|
November 29, 2010, 03:42 |
thin wall conduction
|
#3 |
New Member
majid
Join Date: Aug 2010
Posts: 6
Rep Power: 16 |
hi
I have a problem with heat conduction through thin wall i have square and in fluent in BC i put thickness and shell conduction for walls and i put heat generation in the square too but after solving, in display contours of temperature i can't see contours of temp in the square and i can't see any thickness that i put for wall.why? could any one help me |
|
November 30, 2010, 19:00 |
|
#4 |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Hi Majas,
I believe you are describing your problem with Fluent. But, unfortunately, this is an OpenFOAM forum. I think you stand better chance to get help if you post in the Fluent forum within the cfd-online.com. Cheers, Stefano
__________________
Stefano Wahono Defence Science and Technology Organisation Propulsion Systems |
|
August 20, 2011, 12:35 |
|
#5 |
Member
ak
Join Date: May 2011
Posts: 64
Rep Power: 15 |
Hi Stefano,
Were you able to implement the Two-sided Wall Heat Transfer BC ?ak |
|
August 21, 2011, 20:33 |
|
#6 |
Member
Stefano Wahono
Join Date: Aug 2010
Location: Melbourne, Australia
Posts: 42
Rep Power: 16 |
Hi ak,
Yes, OpenFOAM 2.0 comes with a two-sided wall BC. Several pre-processing steps are needed to set up this. The following steps solve BOTH the normal heat transfer through the wall and the lateral heat transfer (or shell conduction). Good luck trying. Let me know how you go. Let's say the patch name of your two-sided wall is "wall_duct". Note the following steps work with mesh imported from Fluent format with a "shadow" wall already created in the mesh. The pre-processing: 1. Create a setSet file with the following entries Code:
faceSet fBaffle new patchToFace wall_duct faceSet fBaffleShadow new patchToFace wall_duct-shadow cellSet fBaffleCells new faceToCell fBaffle any cellSet fBaffleShadowCells new faceToCell fBaffleShadow any faceZoneSet fBaffle new setToFaceZone fBaffle faceZoneSet fBaffleShadow new setToFaceZone fBaffleShadow // You need to do above for each of you two-sided wall. Code:
$ setSet -batch setSet Code:
region baffleRegion; faceZones (fBaffle); faceZonesShadow (fBaffleShadow); oneD false; extrudeModel linearNormal; nLayers 10; // Number of layers to solve the Conduction Eqn expansionRatio 1; adaptMesh yes; // apply directMapped to both regions linearNormalCoeffs { thickness 0.005; // virtual wall thickness in m } Code:
$ extrudeToRegionMesh -overwrite in your 0/T file: Code:
wall_duct { type compressible::thermoBaffle1DTemperature<constSolidThermoPhysics>; baffleActivated yes; thickness uniform 0.005; // virtual baffle thickness Qs uniform 0; // Heat flux [W/M2] transportProperties { K 202.4; // heat Conductance } radiativeProperties { sigmaS 0; kappa 0; emissivity 0; } thermoProperties { Hf 0; Cp 871; } densityProperties { rho 2719; } value uniform 300; } wall_duct-shadow { $wall_duct } Add the following in 0/U Code:
fBaffleShadow_top { type fixedValue; value uniform (0 0 0); } "region0_.*" { type fixedValue; value uniform (0 0 0); } Code:
fBaffleShadow_top { type zeroGradient; } "region0_.*" { type zeroGradient; } Code:
fBaffleShadow_top { type compressible::epsilonWallFunction; } "region0_.*" { type compressible::epsilonWallFunction; } Code:
fBaffleShadow_top { type compressible::kqRWallFunction; } "region0_.*" { type compressible::kqRWallFunction; } Code:
fBaffleShadow_top { type alphatWallFunction; value uniform 0; } "region0_.*" { type alphatWallFunction; value uniform 0; } Code:
$ mkdir 0/baffleRegion Make a new directory under the system directory: Code:
$ mkdir system/baffleRegion Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: dev | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dictionaryReplacement { boundary { fBaffleShadow_top { type directMappedWallVariableThickness; // This thickness is used if the baffle is 1D. thickness uniform 0.005; } region0_to_baffleRegion_fBaffle { type directMappedWallVariableThickness; // This thickness is used if the baffle is 1D. thickness uniform 0.005; } symplanes { type symmetryPlane; // (symmetryPlane:2D. wedge:1D) } } T { boundaryField { fBaffleShadow_top { type compressible::turbulentTemperatureCoupledBaffleMixedNew; neighbourFieldName T; K solidThermo; KName none; //value uniform 300; Don't want to spoil the old run } region0_to_baffleRegion_fBaffle { type compressible::turbulentTemperatureCoupledBaffleMixedNew; neighbourFieldName T; K solidThermo; KName none; //value uniform 300; Don't want to spoil the old run } } } } Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: dev | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object changeDictionaryDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dictionaryReplacement { T { boundaryField { fBaffleShadow_top { type compressible::turbulentTemperatureCoupledBaffleMixedNew; neighbourFieldName T; K basicThermo; KName none; //value uniform 300; Don't want to spoil the old run } region0_to_baffleRegion_fBaffle { type compressible::turbulentTemperatureCoupledBaffleMixedNew; neighbourFieldName T; K basicThermo; KName none; //value uniform 300; } } } } Code:
$ changeDictionary -literalRE $ changeDictionary -region baffleRegion -literalRE The system/baffleRegion/fvSchemes look like this: Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: dev | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system/baffleRegion"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default steadyState; } divSchemes { default none; } gradSchemes { default Gauss linear; } laplacianSchemes { default none; laplacian(K,T) Gauss linear corrected; } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: dev | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "system/baffleRegion"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { T { /* solver PCG; preconditioner { preconditioner GAMG; tolerance 1e-05; relTol 0; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 2; nFinestSweeps 2; cacheAgglomeration false; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e-05; relTol 0; maxIter 100; */ solver PCG; preconditioner DIC;//GaussSeidel; smoother DILU; tolerance 1e-06; relTol 0; } } nNonOrthCorr 0; relaxationFactors { T 1; } // ************************************************************************* // Create a new file constant/thermoBaffleProperties Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.0 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object thermoBaffleProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoBaffleModel thermoBaffle2D; active yes; regionName baffleRegion; thermoBaffle2DCoeffs { } noThermoCoeffs { } // ************************************************************************* // Create a new file inside this new subdirectory constant/baffleRegion/solidThermophysicalProperties Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 1.7.x | | \\ / A nd | Web: http://www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; object solidThermophysicalProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType constSolidThermo; constSolidThermoCoeffs { //- thermo properties rho rho [1 -3 0 0 0 0 0] 2719; Cp Cp [0 2 -2 -1 0 0 0] 871; K K [1 1 -3 -1 0 0 0] 202.4; //- radiative properties kappa kappa [0 -1 0 0 0 0 0] 0; sigmaS sigmaS [0 -1 0 0 0 0 0] 0; emissivity emissivity [0 0 0 0 0 0 0] 1; //- chemical properties Hf Hf [0 2 -2 0 0 0 0] 0; } // ************************************************************************* // In this example I use rhoSimpleFoam Copy the entire directory of $FOAM_SOLVERS/compressible/rhoSimpleFoam into a new directory $FOAM_SOLVERS/compressible/rhoSimpleBaffleFoam Add the following line in your $FOAM_SOLVERS/compressible/rhoSimpleBaffleFoam/rhoSimpleBaffleFoam.C Code:
#include "simpleControl.H" #include "thermoBaffleModel.H" Code:
autoPtr<regionModels::thermoBaffleModels::thermoBaffleModel> baffles ( regionModels::thermoBaffleModels::thermoBaffleModel::New(mesh) ); Code:
baffles->evolve(); thermo.correct(); Change the Make/files Code:
rhoSimpleBaffleFoam.C EXE = $(FOAM_APPBIN)/rhoSimpleBaffleFoam Code:
EXE_INC = \ -I$(LIB_SRC)/regionModels/regionModel/lnInclude \ -I$(LIB_SRC)/regionModels/thermoBaffleModels/lnInclude EXE_LIBS = \ -lthermoBaffleModels \ -lregionModels Code:
$ Allwmake I hope that helps! Kind regards, Stefano
__________________
Stefano Wahono Defence Science and Technology Organisation Propulsion Systems |
|
August 23, 2011, 12:03 |
|
#7 |
Member
ak
Join Date: May 2011
Posts: 64
Rep Power: 15 |
Hi Stefano,
Thanks so much for the detailed reply! This should be very useful! Currently I am using OF 1.7.1 but will be upgrading to the newer version, and will post once I have results. Thanks again, ak |
|
March 26, 2014, 06:12 |
|
#8 |
New Member
Karla Mora Ulate
Join Date: Jan 2014
Posts: 5
Rep Power: 12 |
Hi,
I am following a similar process but when I use extrudeToRegionMesh -overwrite I got the following error: --> FOAM FATAL ERROR: Zone walls is not consistently all internal or all boundary faces. Face 107868 at (-4 0.1 -3.9) is the first occurrence. From function checkZoneInside(..) in file extrudeToRegionMesh.C at line 439. FOAM exiting Do you have an idea about how can I solve this? Regards, Karla |
|
February 26, 2015, 04:30 |
two sided wall in openfoam
|
#9 |
Member
Naresh Yathuru
Join Date: Feb 2015
Posts: 66
Rep Power: 11 |
Hi karla mora
I m new to openfoam. I m using openfoam 2.3 i would like to know if u could able to solve the error and procceed further. Its a very interesting topic to simulate two sided walls in openfoam . could you please share your experience and challenges u faced. it would be a real contribution. Thank you. regards, Naresh |
|
May 22, 2017, 16:27 |
Two Sided Wall Heat Transfer for Incompressible Flow
|
#10 |
New Member
Brian Schwartz
Join Date: Jul 2016
Location: Lancaster,Pa
Posts: 1
Rep Power: 0 |
I was initially excited when I stumbled upon this post, however I don't think this solution works for my case. I am trying to implement a baffle into a meshed region, and have the baffle affect the flow (act as a wall) but then not affect heat transfer between fluids; I am also using incompressible flow.
Basically, I have added heat transfer to pimpleFoam and I want to track heat transfer across the baffle assuming it is of near zero thickness (no conduction thermal resistance). I successfully added a baffle into the fluid, and have the baffle redirecting flow. However, I had to make the temperature BC zeroGradient for the simulation to run, so it isn't calculating heat transfer across the baffle. I experimented with mapping the baffle master to slave, but didn't really get anywhere with that. Does anyone know of a way in which to do this? |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|