Convergence Problem to Simulate Natural Convection (Buoyancy Driven Flow) Simulation

[Mita Sarkar]

Hello,
 
I am trying to simulate natural convection inside a cavity (buoyancy
driven flow) with radiation effect. The solution is not converging.
Could anyone please let me know how to look at the residuals during
calculations?  I am simulating this problem using steady state
algorithm. I guess if I reduce the relaxation coefficient, it will help
to converge. If that is the case, what value of relaxation coefficient
would be optimum?
I tried to simulate the same problem using standard algorithm, i.e.
unsteady algorithm with a constant and uniform time-step but it did not
help, this is also diverging. Any tricks to tackle this problem? Any
help would be very much appreciated.
 
Thanks
Mita 

[Jean Deschodt]

Hi,
could you attach your settings file? Do you have user sources?
My first advise is to use a unsteady algorithm and particularly "variable time step, constant in space".  Then, for buoyancy driven flow, you have to be very careful with the time step: in the GUI, in the Time Step heading, I advise you to check the button "control of the thermal time step" (I don't remember the exact label, but the keyword is IPTLRO). This button is enable if you use an unsteady algorithm, you have a thermal scalar, and gravity is not null.

[Mita Sarkar]

Hello Jean,
 
My case file is attached here. I have usphyv subroutine to define density variation law. Following your suggestion, I use unsteady algorithm and particularly use time step option as "variable in time and uniform in space" and I also checckk the button "time step limitation with the local thermal time step" but the solution did not converge. I have attached the listing file for two cases: (1) unsteady algorithm with a constant and uniform time step which diverge the solution and (2) unsteady algorithm with time step option as "variable in time and uniform in space". 

[Alexandre Douce]

Hi Mita,
I'd like to reproduced your computation. Do you think, you could attached your mesh too? If it is too big, could you described it or upload it in an external site for file sharing like sendspace for example?

[Mita Sarkar]

Hello Alexandre,
 
The mesh file is attached here. Please let me know if you get any better solution.

Thanks

Mita

[Mita Sarkar]

Hello Alexandre,
 
Is there any updates on this convergence issue. I could not resolve this yet and waiting for your response.
 
Thanks

Mita 

[Alexandre Douce]

Hi Mita,

I think that the trouble with your convergence is due to the mesh: you use a  full tetrahedron mesh, and for a 2D computation it is not appropriate. In the thickness of the mesh you should have a single prism or hexahedron.

In the attached file, you will find a example of a mesh made of hexahedrons, with a parameters file. This set up fails with your mesh 2dcavity1.msh , but works with the attached one (but I try quickly :) ).

More generally, here are some tips for buoyancy driven flow:
- density: check the validity of the law for the density and check the variation of the density in the listing, particularly at the initialization step
- time step: use the unsteady algorithm "variable in time and uniform in space" with the option "Time step limitation with local thermal time step" (see user guide for more explanations, keyword IPTLRO)
- turbulence modeling: check the Grashof number of the situation. For a vertical plate, the flow transitions to turbulent around a Grashof number between 10 8 and 10 9 .   The v2f could be useful  for cases around these critical values. For a well established turbulence, I prefer to use a RSM.
- thermal radiation transfer modeling: do a first set up without radiative transfer. Then iff the computation works, add to the set up the radiative transfer. It is more easy to avoid mistake like this.

[Mita Sarkar]

Hello Alexandre,
 
Thanks a lot for your help! I downloaded the attached file but I could not run it on my machine, it is giving me error at pre-processing stage. Somehow Saturne could not support MED format which is unusual. I could not figure out why it can not support it. The listpre file is attached here. Could you tell me what is wrong with my version of Saturne (Code_Saturne-2.0-rc1), why it can not support MED format? Another thing I noticed on the attached case file, you simulated as constant density but in buoyancy driven flow, density is not constant. If I use density as constant, it is running fine with my mesh file itself. Did you try your mesh file (cavity_hex_2d.med) with variable density and turbulence model also? i think I am facing problem to simulate variable density. I will try to make hex mesh as you suggested and try to run it though I don't understand why it is not running with tet mesh!
 
Once again thank you!
 
Mita

[Yvan Fournier]

Hello,

It would seem that you did not configure/compile Code_Saturne with MED file support (which is optional). This may be due either to not defining the correct "--with-med=<med_prefix_path>" configure options for the Preprocessor and the FVM library, giving a wrong path, or not having MED or its developpement header files installed on your machine.

You probably need to reinstall Code_Saturne with MED support. Depending on the architecture you are running on, MED may be available through your package manager (Debian, Ubuntu for example), or you may need to download it at: http://files.opencascade.com/Salome/Salome5.1.3/med-fichier_2.3.6.tar.gz (it also requires HDF5, available at: http://www.hdfgroup.org).

Best regards,

[Alexandre Douce]

Hello Mita,

the attached mesh is an example. If you could not use the med format, just redo a convenient mesh with gmsh, or add the support of the med library as said by Yvan. Nevertheless, I confirm that I use a variable density with the formula rho = 1.293 * (273.15 / TempK) so I have simulated a buoyancy driven flow. With your mesh, if you use a constant density, no flow occurs (velocity is null) that why the computation does not crash.

I do not use a turbulence model, because in my little test, the flow is not turbulent.