[cfdhelp]

Hello,

I would like to ask you about an OpenFOAM tutorial which was download from the Chalmers and which is concerned for conjugate heat transfer.
There are some problems with the velocity magnitude distribution in the fluid domain.
The case is divided into a square solid and fluid domain. In the fluid domain
is at the inlet set velocity 1m/s for cooling of the solid domain. But after a the end of the iterations, the resulted velocity magnitude a few times exceeded the fluid velocity magnitude... It can be seen in the pictures in the appendix. " Maybe it looks like some type of the wave. "
I don't know what is wrong.
I and another will be grateful for any comments.
The 2D task is fully automated and solution will not take more than ~5 min.
web:http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/
Name of the tutorial:
Conjugate heat transfer in OpenFOAM Slides, Report, Files
The tutorial is in the appendix with the pictures of pressure and velocity.
For simulation, the OpenFOAM - http://bluecfd.github.io/Core/Downloads/ was used.
blueCFD Core 2016-1, OpenFOAM 4 ... version by https://cfd.direct/

Regards,
Ivan

[Bloerb]

If these are the original files from the chalmers report, it looks like a bad comparison to me. It looks like he uses 0.1 m/s as the inlet velocity in one calculation and 1 m/s in the other. Also the starting values are different. Then there is the issue that the thermophysical properties, solvers and schemes are slightly different, the relaxation factors for temperature shouldn't be 0.7 as the temperature will take forever to converge, etc... This is comparing apples to oranges. I am actually to lazy to calculate all the values like density, kappa etc to see if these are identical between the versions.

I have used both solvers in the past, coupled fe40 and of40 and in my comparisons the temperature distribution was identical.

In the files you attached (which is also wrong in the chalmers report) it is the pressure boundary condition. You should set the pressure (p_rgh / dynamic pressure) to fixedValue at the outlet and not at the inlet (fixedMean).

[Tobi]

Hi all,

finally this is exactly the same problem than we have in the 2DPlan tutorial on the wikipage (https://openfoamwiki.net/index.php/G..._-_planeWall2D). Bruno and I were already trying to resolve the problem. Here, in that case it is the same that the pressure BC makes trouble. I investigated a bit but I think, we need some special BC treatment here. In previous FOAM versions we did not use the »p_rgh« pressure and therefore setting up the pressure field was easy.

However, I made a test now and changed the pressure BC to the right hand side. The results seems physically but I don't know if it is correct.

[cfdhelp]

Hi all,

thank you for your answers. The problem was "solved" by the recommendations. The contours looks better but I am not sure the 100%.
I will try to put the corrected case in the appendix as soon as possible.

Regards,
Ivan

[Tobi]

Hi,

you can do so. I also changed the tutorial case I mentioned in the openfoamwiki (planeWall2D). The fixedMean BC seems okay and the results that we get are similar to the one we had previously. However, a validation would be great. In addition it is now very important to unset the gravity in that cases, otherwise you start to get instabilities. To get the results much faster than in the tutorial, there are some options of tweaking. The tweaked case will be published on my website soon.

I am happy that my suggestions helped. Good luck.

[cfdhelp]

Hello all,

I would like to ask in some continuity way if the GAMG for pressure works
properly ?


Regards,
Ivan