My first study: stratification

[Elektrix]

Hello all,

I was successful with my first study and I want to show here what I did. Perhaps somebody could review this and give me some hints about what is wrong and what is ok.

The study is about stratification of water in a storage tank. I hav made a geometry in salome that include a pipe that goes horizontally into a storage tank. The geometry is attached here. The pipe has a diameter of 100mm. I have built only the part of the tank I thought would be important. Only half of the geometry is actually built and I use the symmetry boundary condition in code saturne. The water in the tank has a temperature of 40°C. The water coming through the pipe is at 60°C. I want to see how the warm water flows into the tank.

The geometry is meshed with the mesh module of salome. The mesh is tetrahedral without viscous layer and has around 194000 cells. A view of a part of the mesh is also attached here.

Now to code saturne: I use version 4.4.1 debian package.
The mesh check says about mesh quality:

Code: Select all

  Criterion 3: Least-Squares Gradient Quality:
    Number of bad cells detected: 41 -->   0 %

I decided to ignore this (also because I don't know how to correct this).
I checked steady flow. The turbulence model is Rij-epsilon SSG. I first tried with k-epsilon Linear Production but had errors in the listing telling me that the mesh was too fine. I don't know a lot about the different turbulence models and took the tip from one of the best practice guides. I don't know if this model is the right one but I didn't get errors.
I have no radiative transfers and no conjugate heat transfer (perectly insulated tank).
For the Fluid properties I took the equations for water from a tutorial.
The boundary conditions are:
- Inlet where the water comes in with a speed of 0.03m/s and 60°C Temperature
- Wall with standard settings
- Outlet with standard settings that I don't understand (prescribed flux = 0)
I have set the timestep to 0.5 seconds. A complete calculation run with 400 steps takes around one hour what is statisfying to me with a Intel I5 processor with four cores.

Postprocessing is done with paravis showing the temperature in the symmetry plane, see attached.

The result looks reasonable to me although I cannot really judge it as I'm not a fluid physics specialist. So if somebody could give me some info about what is wrong or right or what could be done better this would help me a lot.

Very best regards

Elektrix

[Martin FERRAND]

Hello,
I will try to answer to some of your interrogations.

Concerning the warning about least square gradient, it is not a big deal (the criterion is not universal). What I would suggest for tetras is to use the least square gradient over extended neighbourhood by the way.

Concerning the warning about the mesh refinement, you can check the Y+ value on the boundary postprocessing mesh. For high Reynolds number turbulence models (such as k eps and Rij SSG), Y+ should be greater than 20-30 so that the model is valid in the wall vicinity. So if the criterion is violated in areas out of interest, no worries.

Concerning the outlet, this condition is on the transported scalar (in your case the temperature) if the flow, for a reason or an other, wants to enter in the domaine. 0 flux is thus consistent with what you want to do.

The results looks indeed realistic. The best to validate your case is to look to cases similar to your one with experimental values available (there exist many experiment for buoyant jets, try to find one with the same reduced Froude number).
If you perform such a case, it is also of interest for us.

Best Regards
Martin

[Elektrix]

Hello Martin,

thank you very much for all the information! This will help me a lot. And, as a beginner it is good to see that I'm already on the "right track" and not doing totally wrong.

Very best regards

Elektrix