[bastil]

Hello all,

I am quite confuesed about OpenFOAM philosophy of handling "sub-meshes". It offers CellZones and regions and for me it is not obvious why both is required. From my point of view one of them would be sufficiant. The current status in v1906 is as follows:

For Porosity, a CellZone is required, on the other hand side for heat transfer regions are required ...

For exporting meshed, foamToVTK can handle regions (and seems also cell Zones) but foamMeshToFluent handles neither nor.

Questions from my side:
Would not do one of CellZones or regions? This will also easen development as many tools do not need to support both?
Is there a way to preserve CellZones and/or regions in Fluent export?

Thanks.

[simrego]

Hi!


Cell zone is a group of cells. For example porosity is just add some source terms to the "marked" (the cells in the cellZone) cells.


While region is a completely different mesh. You can solve different equations in different regions, and you can couple them. So when you are using multiple regions, it is like if you are using different solvers which are coupled. This gives you a lot of freedom. Different turbulence models in every region, different radiation models, different equations, etc.. (in commercial solvers it is mostly impossible)


On the other hand. Let's assume you have a giant cht simulation. You have one giant mesh, which is mostly solid cells. So let's create the fields. You must fill the solid cells with garbage data for the flow variables. There is a commercial solver which does something similar, and you can imagine that waste of memory. But there may be other pros and cons (Honestly I don't know the drawbacks, and I think there are not so much)


I think this whole region thing is came in a later point of the development and if you check the source code for the discretizations, BC handling, etc, that was the easiest way while it is still brilliant and makes the solver really flexible. (This is my personal opinion)



Feel free to ask if something is not clear.

[hjasak]

May I please add a further wrinkle. There is a difference between a cell SET and a cell ZONE, which is important. As a person who designed and implemented the dynamic mesh in FOAM, it is fair to comment.



The idea of a cell ZONE is that it represents a piece of space in which you can eg. specify a heat source in a thermal simulation. Obviously, it is a part of a mesh because I can eg. solve the heat transfer equation on the whole mesh, but only have a volumetric source on a piece of it.


If I renumber the mesh (reorder cells), do a parallel decomposition, run topological changes such as adaptive refinement or layering, the piece of space will remain the same. In all cases, the actuall cell IDs (cell numbers) will change, but the SPACE will remain the same.


In a cell SET, as a part of mesh generation, I collect and manipulate cells only by their IDs. I can do old STAR tricks of moving between cell, face, point, boundary sets and play with their connectivity. If I happen to renumber the mesh after I created a cell set, the cell IDs remain the same but the piece of space would change.


I also have the option of converting a set into a zone; I can have point, face, cell sets/zones at will. There are also further issues of backward lookup, eg. which zone does this cell belong to?, but this is a different story.


Hope thishelps,


Hrv