|
[Sponsors] |
chtIcoMultiRegionFoam - Incompressible version of chtMultiRegionFoam. |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#21 |
Senior Member
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 16 ![]() |
Hi all,
I have set up my mesh as follows: Code:
Fluid_to_Solid { type directMappedWall; nFaces 50; startFace 825; sampleMode nearestPatchFace; sampleRegion Solid; samplePatch Solid_to_Fluid; offset (0 0 0); } Code:
Fluid_to_Solid { type compressible::turbulentTemperatureCoupledBaffle; value uniform 300; neighbourFieldName T; K K; } Any help will be appreciated. Regards, Steven |
|
![]() |
![]() |
![]() |
![]() |
#22 |
Senior Member
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 16 ![]() |
Changed the initial condition for T to:
Code:
Fluid_to_Solid { type solidWallMixedTemperatureCoupled; value uniform 300; neighbourFieldName T; K K; } |
|
![]() |
![]() |
![]() |
![]() |
#23 |
Member
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 16 ![]() |
compressible::turbulentTemperatureCoupledBaffle;
This turbulent BC is not used in the solver.. if you look at the code it use other turbulent library... The solver was developed for laminar cases, turbulence was added for public release, but no correct treatment of the conjugated heat transfer is present in OpenFOAM turbulence libraries, so using the one that you used (the mixedtemperaturecoupled) is the right way to do coupling, also having an fine mesh around the solid surfaces helps a lot in increasing the quality of the simulation |
|
![]() |
![]() |
![]() |
![]() |
#24 |
Senior Member
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 16 ![]() |
Thanks for you reply. Now I am sure about the coupling.
I am going to do DNS so I am not bothered with turbulence modelling or wall functions. Thanks again for sharing your work. |
|
![]() |
![]() |
![]() |
![]() |
#25 | |
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 15 ![]() |
Quote:
What change did you make to resolve Code:
--> FOAM FATAL ERROR: request for uniformDimensionedVectorField g from objectRegistry bottomAir failed available objects of type uniformDimensionedVectorField are 0 ( ) Is there something to do with the code (hopefully not...) or is it located in the directories? Thanks Have a nice day/evening/night (depending on where you are ![]()
__________________
Sam |
||
![]() |
![]() |
![]() |
![]() |
#26 |
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 16 ![]() |
Hi all
Your solver is very usefull. Have you a test case? To see necessary dict? Also a simple case. Thanks |
|
![]() |
![]() |
![]() |
![]() |
#27 |
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 16 ![]() |
Hi
In my test case I have this error: Create time Create fluid mesh for region Fluido for time = 0 Create solid mesh for region Solido for time = 0 *** Reading fluid mesh thermophysical properties for region Fluido Adding to KFluid Adding to TFluid Adding to pFluid Adding to UFluid Adding to phiFluid Adding to thermoFluid Selecting incompressible transport model Newtonian Adding to turbulence Selecting turbulence model type laminar *** Reading solid mesh thermophysical properties for region Solido Adding to rhos Adding to cps Adding to Ks Adding to Ts Region: Fluido Courant Number mean: 0 max: 2.00134 Region: Solido Diffusion Number mean: 1.528169e-05 max: 3.332232e-05 deltaT = 0.2498326 Region: Fluido Courant Number mean: 0 max: 5 Region: Solido Diffusion Number mean: 3.817864e-05 max: 8.325001e-05 deltaT = 0.2498326 Time = 0.249833 Solving for fluid region Fluido --> FOAM FATAL ERROR: incompatible dimensions for operation [U[0 1 -2 0 0 0 0] ] == [-grad(p)[1 -2 -2 0 0 0 0] ] From function checkMethod(const fvMatrix<Type>&, const GeometricField<Type, fvPatchField, volMesh>&) in file /home/acconcia/OpenFOAM/OpenFOAM-1.6.x/src/finiteVolume/lnInclude/fvMatrix.C at line 1219. FOAM aborting #0 Foam::error: ![]() #1 Foam::error::abort() in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so" #2 void Foam::checkMethod<Foam::Vector<double> >(Foam::fvMatrix<Foam::Vector<double> > const&, Foam: ![]() #3 in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" #4 in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" #5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #6 in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" How can I solve it? Thanks |
|
![]() |
![]() |
![]() |
![]() |
#28 |
Member
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 16 ![]() |
Ciao Daniele,
you have to check your pEqn.H because it looks like you have added a new term that does not have the right dimension! You have something with kg/m that is not coherent with the dimensions of the momentum eq. Hope it helps, |
|
![]() |
![]() |
![]() |
![]() |
#29 |
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 16 ![]() |
Yes my previus post is wrong my error is this sorry
![]() Create time Create fluid mesh for region Fluido for time = 0 Create solid mesh for region Solido for time = 0 *** Reading fluid mesh thermophysical properties for region Fluido Adding to KFluid Adding to TFluid Adding to pFluid Adding to UFluid Adding to phiFluid Adding to thermoFluid Selecting incompressible transport model Newtonian Adding to turbulence Selecting turbulence model type laminar *** Reading solid mesh thermophysical properties for region Solido Adding to rhos Adding to cps Adding to Ks Adding to Ts Region: Fluido Courant Number mean: 0 max: 2.00134 Region: Solido Diffusion Number mean: 1.528169e-05 max: 3.332232e-05 deltaT = 0.2498326 Region: Fluido Courant Number mean: 0 max: 5 Region: Solido Diffusion Number mean: 3.817864e-05 max: 8.325001e-05 deltaT = 0.2498326 Time = 0.249833 Solving for fluid region Fluido DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 4.067041e-06, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 3.773002e-06, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 5.093329e-07, No Iterations 1 DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 3.398608e-07, No Iterations 1 max(T) [0 0 0 1 0 0 0] 955.9357 --> FOAM FATAL ERROR: request for uniformDimensionedVectorField g from objectRegistry Fluido failed available objects of type uniformDimensionedVectorField are 0 ( ) From function objectRegistry::lookupObject<Type>(const word&) const in file /home/acconcia/OpenFOAM/OpenFOAM-1.6.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 140. FOAM aborting #0 Foam::error: ![]() #1 Foam::error::abort() in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Foam::Ostream& Foam: ![]() #3 Foam::UniformDimensionedField<Foam::Vector<double> > const& Foam: ![]() #4 Foam::buoyantPressureFvPatchScalarField::updateCoe ffs() in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so" #5 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricFi eld<double, Foam::fvPatchField, Foam::volMesh>&, Foam::dimensionSet const&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libincompressibleRASModels.so" #6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacianUncorrected(Foam::GeometricFi eld<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so" #7 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so" #8 Foam::fv::laplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so" #9 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" #10 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" #11 in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" #12 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #13 in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam" |
|
![]() |
![]() |
![]() |
![]() |
#30 |
Senior Member
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 16 ![]() |
Hi
How can I resolve this problem: FOAM FATAL ERROR request for uniformDimensionedVectorField g from objectRegistry Fluido failed available objects of type uniformDimensionedVectorField are ????????????????? Thanks |
|
![]() |
![]() |
![]() |
![]() |
#31 |
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 15 ![]() |
Hi Daniele,
I had exactly the same problem (with icoFoam but anyway, still). I just managed to solve it. In my case, the BC were the problems. For, p I had buoyantPressure BC for a wall and it wasn't fitted for icoFoam (with a zeroGradient, it's fine). I will suggest to have a look at your BC, carefully! Hope that can help you
__________________
Sam |
|
![]() |
![]() |
![]() |
![]() |
#32 |
Member
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 15 ![]() |
Me again!
Has anyone created a tutorial or have a running case with chtIcoMultiRegionFoam? Something must be wrong with the case I try to run. All I've got is: Code:
Region: v_fluid Courant Number mean: 0 max: 925.786412 Region: v_solid Diffusion Number mean: 0.00805877817 max: 0.0110466663 Region: domain0 Diffusion Number mean: 0.00807993205 max: 0.0110468266 Region: domain2 Diffusion Number mean: 0.00807993206 max: 0.0110468266 Time = 666 ExecutionTime = 1.84 s ClockTime = 2 s Region: v_fluid Courant Number mean: 0 max: 925.786412 Region: v_solid Diffusion Number mean: 0.00805877817 max: 0.0110466663 Region: domain0 Diffusion Number mean: 0.00807993205 max: 0.0110468266 Region: domain2 Diffusion Number mean: 0.00807993206 max: 0.0110468266 Time = 667 ExecutionTime = 1.84 s ClockTime = 2 s Any hints where it can come from? (I don't join my case but if necessary I will)
__________________
Sam |
|
![]() |
![]() |
![]() |
![]() |
#33 |
New Member
Jean El-Hajal
Join Date: Jun 2010
Location: Ulm
Posts: 16
Rep Power: 16 ![]() |
Hi,
(already wrote it in an another post but maybe someone is also interested here) I had a problem with chtIcoMultiRegionFoam compilation with 1.7.x In the file: chtIcoMultiRegionFoam/derivedFvPatchFields/solidWallMixedTemperatureCoupled/solidWallMixedTemperatureCoupledFvPatchScalarField .C just add #include "mapDistribute.H" like this: #include "solidWallMixedTemperatureCoupledFvPatchScalar Fiel d.H" #include "addToRunTimeSelectionTable.H" #include "fvPatchFieldMapper.H" #include "volFields.H" #include "directMappedPatchBase.H" #include "mapDistribute.H" #include "regionProperties.H" maybe could help someone. Jean |
|
![]() |
![]() |
![]() |
![]() |
#34 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 ![]() |
Hi,
Thank you for sharing this solver. Unfortunately, I'm not able to set up my case using it: I've copied the chtMultiRegionFoam tutorial and changed the mesh and the BCs. But it seems I've missed something. Has anybody got a simple running case, so that I'll see how to do? Best regards, Nicolas. |
|
![]() |
![]() |
![]() |
![]() |
#35 | |
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 17 ![]() |
Quote:
I recently generated a few elementary test cases with this solver. I include them in the attaced file. I welcome suggestions, corrections, ... Mirko |
||
![]() |
![]() |
![]() |
![]() |
#36 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 ![]() |
Hi Mirko,
thank you very much for these cases. I still have to work on this solver since I'm not able to set up a steadyState case including 1 fluid and 2 solids. But maybe it's quite normal see that the two cases with fluids you shared are transient. Am I mistaking? And once again, thanks for the work. Nicolas |
|
![]() |
![]() |
![]() |
![]() |
#37 | |
Senior Member
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 17 ![]() |
Quote:
I set-up the fluid/fluid to model a heat exchanger. I have not tried setting up a steady-state case. That is something I need to get familiar with. I would suggest that you make sure you know how to solve steady state case of a pure incompressible solver (i.e., single region problem), before trying it with this one. As for fluid/solid, I should have included that too. It should not be difficult. The same temperature conditions should apply, just decleare one of the regions as solid, and assign appropriate properties. Do it first as transient, and then try steady state. I'm traveling next 2.5 weeks, so I will not be able to work on this. On the other hand, I will attend the OF workshop at Penn State, so hopefully I learn useful stuff for multi-region solvers :-) Mirko |
||
![]() |
![]() |
![]() |
![]() |
#38 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 ![]() |
Ok, I'm going to work following your suggestions.
Have a good workshop! |
|
![]() |
![]() |
![]() |
![]() |
#39 |
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 23 ![]() |
Hello,
nicolasB, Mirco, have you succeeded in creating a steady state version of chtIcoMultiRegionFoam? mad |
|
![]() |
![]() |
![]() |
![]() |
#40 |
Member
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 15 ![]() |
Hi,
I've set up a case with both a solid and a fluid. It seems to run correctly in transient, but I've got something weird with the temperature on steady. I join an archive with these cases (just use the "Allrun" scripts). What I don't understand is why we have to run this solver on transient mode for fluids while it works on steady for solids... Regards, Nicolas |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
OpenFOAM on cluster: version GLIBCXX_3.4.9 and GLIBCXX_3.4.11 not found | ovie | OpenFOAM | 10 | April 19, 2021 19:06 |
paraview installation woes | vex | OpenFOAM Installation | 15 | January 30, 2011 08:11 |
bubbleFoam validation case | balkrishna | OpenFOAM Running, Solving & CFD | 24 | August 30, 2010 05:37 |
[OpenFOAM] Problem with paraFoam on a linux-64 bit | bunni | ParaView | 4 | April 14, 2010 21:55 |
paraFoam reader for OpenFOAM 1.6 | smart | OpenFOAM Installation | 13 | November 16, 2009 22:41 |