CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   chtIcoMultiRegionFoam - Incompressible version of chtMultiRegionFoam. (http://www.cfd-online.com/Forums/openfoam-programming-development/81746-chticomultiregionfoam-incompressible-version-chtmultiregionfoam.html)

Canesin November 5, 2010 08:25

chtIcoMultiRegionFoam - Incompressible version of chtMultiRegionFoam.
 
1 Attachment(s)
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

stevenvanharen November 5, 2010 10:39

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

Canesin November 5, 2010 14:43

Hi Steven,

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

pcaron November 5, 2010 17:24

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

Canesin November 5, 2010 20:27

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

phsieh2005 November 7, 2010 16:30

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

Canesin November 8, 2010 05:26

Quote:

Originally Posted by phsieh2005 (Post 282547)
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?

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

Quote:

Originally Posted by phsieh2005 (Post 282547)
What is the reason of developing the chtIcoMultiRegionFoam over chtMultiRegionFoam (which uses compressible solver for fluid I believe)?

Pei

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.

phsieh2005 November 8, 2010 13:40

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

Canesin November 8, 2010 16:56

Quote:

Originally Posted by phsieh2005 (Post 282646)
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?

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

phsieh2005 November 8, 2010 21:08

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>

phsieh2005 November 8, 2010 21:52

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

Canesin November 10, 2010 09:43

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

phsieh2005 November 10, 2010 10:34

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

Canesin November 11, 2010 17:55

Quote:

Originally Posted by phsieh2005 (Post 282920)
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.

pcaron November 13, 2010 16:05

Quote:

Originally Posted by Canesin (Post 282400)
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

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
Quote:

Modifications to multiphase and buoyant solvers
...
Multiphase and buoyant flow solvers now solve for p_rgh=p-rho g\cdot x, rather than the static pressure p. This change is to avoid deficiencies in the handling of the pressure force / buoyant force balance on non-orthogonal and distorted meshes.
...
So, I'll start using the standard new cht version. I've been very busy last week.

Regards

Pablo

maddalena January 14, 2011 03:38

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

Canesin January 14, 2011 13:15

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.

maddalena January 17, 2011 04:26

Quote:

Originally Posted by Canesin (Post 290471)
I have not done many tests in the turbulence settings.. But it is "FOAM way" of doing turbulence.. [...] 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

stevenvanharen January 25, 2011 09:54

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

Canesin January 25, 2011 11:37

Quote:

Originally Posted by maddalena (Post 290685)
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

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.


All times are GMT -4. The time now is 22:53.