CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Programming & Development

chtIcoMultiRegionFoam - Incompressible version of chtMultiRegionFoam.

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree5Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 26, 2011, 04:03
Default
  #21
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 6
stevenvanharen is on a distinguished road
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);
    }
And the initial condition as:

Code:
Fluid_to_Solid
    {
        type            compressible::turbulentTemperatureCoupledBaffle;
        value           uniform 300;
        neighbourFieldName T;
        K               K;
    }
Is this correct? I have a feeling the error I get is coming from how I set this interface up.

Any help will be appreciated.

Regards,

Steven
stevenvanharen is offline   Reply With Quote

Old   January 26, 2011, 06:07
Default
  #22
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 6
stevenvanharen is on a distinguished road
Changed the initial condition for T to:

Code:
Fluid_to_Solid
    {
      type  solidWallMixedTemperatureCoupled;     
        value           uniform 300;
        neighbourFieldName T;
        K               K;
    }
Now it seems to be working, is this also what you guys use?
stevenvanharen is offline   Reply With Quote

Old   January 26, 2011, 10:11
Default
  #23
Member
 
Fábio César Canesin
Join Date: Mar 2010
Location: Florianópolis
Posts: 67
Rep Power: 6
Canesin is on a distinguished road
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
Canesin is offline   Reply With Quote

Old   January 26, 2011, 10:30
Default
  #24
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 6
stevenvanharen is on a distinguished road
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.
stevenvanharen is offline   Reply With Quote

Old   March 17, 2011, 07:55
Default
  #25
Member
 
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 5
sixwp is on a distinguished road
Quote:
Originally Posted by phsieh2005 View Post
Hi, Fábio,

I made some more changes. Now the case is running. This is the same case in the OF-1.7.x/snappyMultiRegionHeater. I will check if the results are reasonable when the run completes.
Pei
Hi Pei,

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
sixwp is offline   Reply With Quote

Old   March 17, 2011, 09:23
Default
  #26
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 6
Daniele111 is on a distinguished road
Hi all
Your solver is very usefull. Have you a test case? To see necessary dict? Also a simple case.

Thanks
Daniele111 is offline   Reply With Quote

Old   March 24, 2011, 14:18
Default
  #27
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 6
Daniele111 is on a distinguished road
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:rintStack(Foam::Ostream&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#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:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, char const*) in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam"
#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
Daniele111 is offline   Reply With Quote

Old   March 24, 2011, 14:27
Default
  #28
Member
 
Sabin Ceuca
Join Date: Mar 2010
Location: Munich
Posts: 42
Rep Power: 6
sabin.ceuca is on a distinguished road
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,
sabin.ceuca is offline   Reply With Quote

Old   March 24, 2011, 14:50
Default
  #29
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 6
Daniele111 is on a distinguished road
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:rintStack(Foam::Ostream&) in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Foam::Ostream& Foam:perator<< <Foam::error>(Foam::Ostream&, Foam::errorManip<Foam::error>) in "/home/acconcia/OpenFOAM/acconcia-1.6.x/applications/bin/linuxGccDPOpt/chtIcoMultiRegionFoam"
#3 Foam::UniformDimensionedField<Foam::Vector<double> > const& Foam:bjectRegistry::lookupObject<Foam::UniformDi mensionedField<Foam::Vector<double> > >(Foam::word const&) const in "/home/acconcia/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so"
#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"
Daniele111 is offline   Reply With Quote

Old   March 26, 2011, 17:08
Default
  #30
Senior Member
 
Daniele
Join Date: Feb 2010
Posts: 134
Rep Power: 6
Daniele111 is on a distinguished road
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
Daniele111 is offline   Reply With Quote

Old   April 4, 2011, 10:05
Default
  #31
Member
 
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 5
sixwp is on a distinguished road
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
sixwp is offline   Reply With Quote

Old   April 15, 2011, 08:58
Default
  #32
Member
 
Samuel ARNAUD
Join Date: Feb 2011
Location: Grenoble, FRANCE
Posts: 39
Rep Power: 5
sixwp is on a distinguished road
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
nothing actually runs...

Any hints where it can come from?
(I don't join my case but if necessary I will)
__________________
Sam
sixwp is offline   Reply With Quote

Old   May 30, 2011, 19:02
Default
  #33
New Member
 
Jean El-Hajal
Join Date: Jun 2010
Location: Ulm
Posts: 16
Rep Power: 6
Jean El-Hajal is on a distinguished road
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
Jean El-Hajal is offline   Reply With Quote

Old   May 31, 2011, 06:58
Default
  #34
Member
 
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 5
NicolasB is on a distinguished road
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.
NicolasB is offline   Reply With Quote

Old   June 1, 2011, 15:59
Default
  #35
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 7
mirko is on a distinguished road
Quote:
Originally Posted by NicolasB View Post
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.
Hi Nicolas,

I recently generated a few elementary test cases with this solver. I include them in the attaced file.

I welcome suggestions, corrections, ...

Mirko
Attached Files
File Type: gz chtIcoHeatExchanger.tar.gz (68.9 KB, 149 views)
PonchO and brucechen1115 like this.
mirko is offline   Reply With Quote

Old   June 8, 2011, 04:58
Default
  #36
Member
 
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 5
NicolasB is on a distinguished road
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
NicolasB is offline   Reply With Quote

Old   June 8, 2011, 09:40
Default
  #37
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 7
mirko is on a distinguished road
Quote:
Originally Posted by NicolasB View Post
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
Hi Nicolas,

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
mirko is offline   Reply With Quote

Old   June 8, 2011, 10:07
Default
  #38
Member
 
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 5
NicolasB is on a distinguished road
Ok, I'm going to work following your suggestions.
Have a good workshop!
NicolasB is offline   Reply With Quote

Old   July 11, 2011, 05:42
Default Steady state version?
  #39
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 11
maddalena is on a distinguished road
Hello,
nicolasB, Mirco, have you succeeded in creating a steady state version of chtIcoMultiRegionFoam?

mad
maddalena is offline   Reply With Quote

Old   July 11, 2011, 09:42
Default
  #40
Member
 
Nicolas
Join Date: Apr 2011
Location: Biarritz / France
Posts: 33
Rep Power: 5
NicolasB is on a distinguished road
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
Attached Files
File Type: gz chtIcoMulti.tar.gz (9.9 KB, 112 views)
NicolasB is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFOAM on cluster: version GLIBCXX_3.4.9 and GLIBCXX_3.4.11 not found ovie OpenFOAM 9 October 15, 2012 02:59
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
Problem with paraFoam on a linux-64 bit bunni OpenFOAM Paraview & paraFoam 4 April 14, 2010 21:55
paraFoam reader for OpenFOAM 1.6 smart OpenFOAM Installation 13 November 16, 2009 22:41


All times are GMT -4. The time now is 13:16.