chtIcoMultiRegionFoam - Incompressible version of chtMultiRegionFoam.
 

Hi all,

I have been working with some modified chtMultiRegion codes for some time.. This version is the same I have send to Hrvoje Jasak for inclusion on the next version OpenFOAM-1.6-ext
To complie just enter the folder and type "wmake".

The solver was tested without turbulence, I will add an test case to this thread as soon as I have time to setup an easy to understand..

Please, keep the references in the source-code.. If you like to reference this solver you can:

CANESIN, F. C. : chtIcoMultiRegionFoam, incompressible multi-region fully segregated conjugated heat transfer - http://www.canesin.com/software

I hope to see good use of the code, I'm working in an fully coupled version and in some addons and a test case for my undergraduate thesis .. but don't hope for it so soon.

Best regards,
Fábio C. Canesin

Hi Fabio,

I have been working on the exact same thing.

It is on the shelf for now but beginning next year I will do some work with my solver.

Probably I will start with validating against work done by Tiselj (Conjugate heat transfer in channel flow) since I will do fully turbulent DNS.

What are you working on?

Regards,

Steven

Hi Steven,

I have been working with geometric optimization for active magnetic regenerators .. it is an setup for magnetic cooling.

Does it works for unstructured meshes?
 

Hi Fábio,

I've using chtMultiReginFoam, from 1.6.x, for some weeks. Apparently there is an issue with unstructured meshes, or I'm missing something . If you set up a case with uniform temperatures, spurious velocities arises.

Have you tried using unstructured meshes?

Best regards,

Pablo

Hi Pablo,

I have not.. but, I know that in my solver will not have this issue, because it is a fully segregated approach, it solves velocity and them uses it to transport temperature..

The case in chtMultiRegionFoam cam be from the Boussinesq aproximation, where the temperature field is diverging the pressure.. or maybe some wrong boundary condition..

Best regards,
Fábio C. Canesin

Hi, Canesin,

I will try to see if I can modify the tutorial case in OF-1.7.x to run with your chtIcoMultiRegionFoam solver. Any suggestion before I start?

What is the reason of developing the chtIcoMultiRegionFoam over chtMultiRegionFoam (which uses compressible solver for fluid I believe)?

Pei

Yes, you can setup the case where the fluid has a configuration as like pimpleFoam and the solid as like the solid in chtMultiRegionFoam

Besides using an compressible solver in chtMultiRegionFoam it can be used to simulate water, as is done in the new tutorial in 1.7.x, but it is like as little mess, you have to define and compressible::incompressible thermophysic property O.o.... Also it uses Boussinesq aproximation for natural(free) convection.. In that solver I propose there is no effects from the temperature in the fluid, like in forced convection.

Hi, Fábio,

Is there any reason why K is required for the fluid region? What value should I use for K if fluid is water?

Thanks!

Pei

K is the thermal conductivity of the fluid.. It is needed for the temperature coupling with the solid region, to compute the heat flux..

A tipical value for water is 0.6 W/m*k

Best regards,

Fábio C. Canesin

Hi, Fábio,

Thanks for the explanation.

This is more involved that what I originally expected. I basically used the fluid properties from buoyantBoussinesqPimpleFoam case and also made some changes to the fvSchemes and fvSolution. But, I am getting strange error messages. I will have to look into your code in more detail.

Pei
--------------------
Solving for fluid region bottomAir
DILUPBiCG: Solving for T, Initial residual = 1, Final residual = 4.8181319e-05, No Iterations 1
max(T) [0 0 0 1 0 0 0] 304.7137


--> FOAM FATAL ERROR:

request for uniformDimensionedVectorField g from objectRegistry bottomAir failed
available objects of type uniformDimensionedVectorField are

0
(
)


From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/phsieh/OpenFOAM/OpenFOAM-1.7.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 139.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 Foam::UniformDimensionedField<Foam::Vector<double> > const& Foam::objectRegistry::lookupObject<Foam::UniformDi mensionedField<Foam::Vector<double> > >(Foam::word const&) const in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#3 Foam::buoyantPressureFvPatchScalarField::updateCoe ffs() in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoef fs() in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#5 Foam::adjustPhi(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&) in "/home/phsieh/OpenFOAM/OpenFOAM-1.7.x/lib/linux64GccDPOpt/libfiniteVolume.so"
#6
in "/home/phsieh/OpenFOAM/phsieh-1.7.x/applications/bin/linux64GccDPOpt/chtIcoMultiRegionFoam"
#7 __libc_start_main in "/lib64/libc.so.6"
#8
at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116
Aborted
phsieh@rutgers:~/OpenFOAM/phsieh-1.7.x/run/snappyIcoMultiRegionHeater>

Hi, Fábio,

Sorry to bother you again. I am wondering which fluid solver your chtIcoMultiRegionFoam was based on? PimpleFoam? buoyantBoyssinesqPimpleFoam?

At a quick glance, I did not find the location in the code that g is given.

Also, I compiled your chtIcoMultiRegionFoam on OpenFOAM-1.7.x. I am wondering if this makes any difference. However, compilation was successful.

Are you planning to write any paper or thesis on your work? Maybe I can read your thesis/paper to figure it out?

Pei

The fluid is based in pimpleFoam .. ... this is not the solver for my work, this is a first generation, as the final version needs the not-released block-matrix solver for do pressure coupling and become fully implicit ..

It should not as for g in the solver .. in the controlDict you have changed the solver ??? O.o ..

If you can hold until the weekend I can setup a very basic case for it, and you can them use it to make your case work.. sorry, but I'm doing 53hours/week..

Best regards,

Fábio C. Canesin

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.

So, this solver does not handle natural convection? Is there any reason why you did not pick buoyantBousinessqPimpleFoam as fluid solver?

Pei

Yes it does not handle natural convection.. it was developed for forced convection cases and small channels cooling.. consistence and easy to expand, that where the reasons.

Dear Fábio, sorry for the late reply. It was a hard week. The problem I had seems to be related with the pressure definitios previous to 1.7 version.

You can see the release notes for OF http://www.openfoam.com/archive/1.7....ease-notes.php
So, I'll start using the standard new cht version. I've been very busy last week.

Regards

Pablo

Hi Fabio,
and thanks for sharing your solver! Incompressible & forced convection & unstructured mesh: this is what I was looking for! Have you made any tests with the turbulence on? I need it in my case. Can you tell me something about that?
Regards

mad

I have not done many tests in the turbulence settings.. But it is "FOAM way" of doing turbulence.. If you look at the source code you will see that turbulence is added as an term in the equations using turbulent prandtl and nu ..

You should be able to use any turbulence model from OpenFOAM, but it will be tied with your study case.

Sorry but I cannot understand... This is what usually applies to turbulence, isn't it?
One more question, open to everybody: is there anyone that has a steady state version of this incompressible multiregion cht solver?
Thank you

mad

Hi all,

does somebody have a simple tutorial for this solver?

I have been trying to create a case myself but it keeps generating errors, I guess I am making a mistake somewhere in setting up the case.

It would be great if one of you guys could share a simple case you have performed with this solver.

Thanks in advance.

Kind regards,

Steven

Yes, it is what applies to turbulence...

I do not have a steady state version because my problem do not have steady state solution.

But, you could use larger times steps.. Run fist the potentialFoam to have good fluids fields... tham use something like GAMG to make it more tolerant to instabilities.

Hi all,

I have set up my mesh as follows:

And the initial condition as:

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

Changed the initial condition for T to:

Now it seems to be working, is this also what you guys use?

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

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.

Hi Pei,

What change did you make to resolve ?
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 :D)

Hi all
Your solver is very usefull. Have you a test case? To see necessary dict? Also a simple case.

Thanks

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::printStack(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::DimensionedField<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

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,

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::printStack(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::operator<< <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::objectRegistry::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"

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

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

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:
nothing actually runs...

Any hints where it can come from?
(I don't join my case but if necessary I will)

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

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

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

Ok, I'm going to work following your suggestions.
Have a good workshop!

Steady state version?
 

Hello,
nicolasB, Mirco, have you succeeded in creating a steady state version of chtIcoMultiRegionFoam?

mad

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