LES within a RANS domain ?
 

Hello all,

I have a two questions :)

-Is it possible to perform LES within a RANS domain only for a small particular region ? If so how, I have tried mapping with unsatisfactory results, is there any other method(s)

-Is there any tutorial for stationary GGI ? all the examples I am finding are for turbo machinery components

Regards,

Hasan K.J

Hi,

1) DES could be an option (openfoam does have some DES SGS models) which switches from a RANS to a LES based on the resolution of your mesh. You could try refining your mesh fine enough in the region where you want your SGS modeling and thereby performing an LES in that region alone.

2) You could use mapFields to map the solutions of a RANS case and then run your LES. If you dont want to use mapFields, use the time directory of your last time step of the RANS solution and rename it to 0. This will become your 0 folder for your LES case with all the field data and then you could run LES.

About your question 2, I am ignorant about it.Sorry.

I hope this helps.

Thanks (Nandri) Thangam,

I am quite aware of the MapFields function in openFOAM, My actual question is that if we could simulate LES within RANS domain simultaneously like as the RANS simulation is running ?
- How familiar are you with MapFields Function because I have question about it here
http://www.cfd-online.com/Forums/ope...-openfoam.html

Regards,
Hasan K.J

Greetings to all!

@Hasan:
Can you be more specifically as to what exactly you want this simulation to do?

In other words:

1. Why can't you run 2 separate simulations, where one is using RANS and the other is using LES?
2. Doesn't DES or DDES work for your case? Namely to have LES and RANS simulated in the same domain, but only some cells use LES and others use RANS?

Best regards,
Bruno

Hey Bruno,

well i tried doing what you have mentioned a initial RANS case and mapping data to a subdomain for a LES case and hat troubles with boundary conditions after MapFields and i have been partly unsuccessful.

I want to try GGI but not entirely sure if it applicable for two stationary cases ?

- the doubt arouse when i saw some papers where they mentioned that LES was simulated for flow only from midspan of the airfoil to one chord length behind the airfoil. I dunno how they have performed this.

- to explain it more clearly the entire domain of just an airfoil simulated for RANS but only a smaller denser sub-section from mid of the airfoil to one chord length behind the airfoil is used for LES

- haven't had the time to look into DES, I have submission on second week of JAN and because the RANS domain i am using is quite large for DES, i need to refine the mesh already with coarse i have 11 million cells no time for further modifications to mesh

- i dont understand what you mean by "Namely to have LES and RANS simulated in the same domain, but only some cells use LES and others use RANS?"

Thanks for your time,
Regards,
Hasan K.J

GGI? Why do you think you need to use a "General Grid Interface"? Do you mean that you want to have two meshes to transfer flow between each other, without having to stitch the meshes into a single mesh?


Regarding DES and DDES:

• http://www.openfoam.org/docs/user/st...-libraries.php
  
  Quote:

  SpalartAllmarasDDES - Spalart-Allmaras delayed detached eddy simulation (DDES) model SpalartAllmarasIDDES - Spalart-Allmaras improved DDES (IDDES) model

• http://www.openfoam.org/features/LES.php
• http://www.openfoam.org/features/turbulence.php
  
  Quote:

  Detached eddy simulation (DES): Hybrid method that treats near-wall regions with a RAS approach and the bulk flow with an LES approach. DES models are found in the list of LES models.

A couple of posts that might come in handy for you:

• http://www.cfd-online.com/Forums/ope...tml#post424797 post #10
• http://www.cfd-online.com/Forums/ope...tml#post424652 post #2

Beyond this, perhaps you need to first address the issue of ensuring a good mesh, as implied in this post: http://www.cfd-online.com/Forums/ope...tml#post467771 post #37


Ooooh, wait... I think I'm starting to understand... you want to be able to have the big domain region running with RAS (RANS) and to use LES only near the blade, is that it? I think that, at least in theory, you don't need to do that. You simply use a coarse mesh wherever you don't need much turbulence resolution and use a finer mesh where you want more resolution; and use only LES for the whole domain. Then one of the LES turbulence models should be able to give you the level of control you want, concerning how it behaves in the coarse mesh region.

Hey Bruno,

ya what i meant was transferring data between the two without stitching the mesh that would be awesome !!! - how should i go about it any suggestions ?

Since stitching could cause more problems, than I already have in hand

- another issue with DES is .. My project title itself something to do with LES so can't back on that.. too late now.. lol

"Ooooh, wait... I think I'm starting to understand... you want to be able to have the big domain region running with RAS (RANS) and to use LES only near the blade, is that it? "
- thats exactly IT

"I think that, at least in theory, you don't need to do that. You simply use a coarse mesh wherever you don't need much turbulence resolution and use a finer mesh where you want more resolution; and use only LES for the whole domain. Then one of the LES turbulence models should be able to give you the level of control you want, concerning how it behaves in the coarse mesh region."

- This could be possible if the Stitching the mesh is possible or transferring data between 2 geometries and LES gives awful results in coarse mesh from my experience and my coarse mesh is not that coarse it has 11 million cells

- I have reasonable data to make a good thesis
- but not being able to replicate the wake flow is a stress
- so stitching the mesh and running one LES should do and run a Full LES

- if stitching is possible can i have my hexahedral cells ? after stitching ?

Thanks,
Hasan K.J

Hi Hasan,

Yes, it's possible to do so. But it doesn't always work very well, specially if the two meshes aren't compatible enough. Here is a very nice thread on this topic, including some situations where things don't go as expected: http://www.cfd-online.com/Forums/ope...mesh-used.html

Yes, they will remain hexahedral. The detail is that stitching can require cutting up the faces in the interface, in order to be able to connect the cells between each mesh. Which can be a source of problems, since faces with very small areas can lead to very big simulation difficulties :(

I've done this with OpenFOAM 2.1 and/or 2.2, where I simply merged the meshes with mergeMeshes and defined the patches between the two meshes to be "cyclicAMI", using either createPatch or changeDictionary... I can't remember which one it was.

Ah, OK OK. Then DES/DDES/IDDES might not be what you're looking for.

I'm not an expert on this topic, namely LES... nor RANS, nor CFD for that matter :rolleyes: I just know some basics and act somewhat as an interactive library here in the forum :)
But AFAIK, stitching or merging the mesh only solves the mesh resolution issue. And that issue can be easily solved if you mesh it all at once, while defining a proper mesh refinement near the blade.

Then it all comes down to using the correct LES model, from the list given here: http://www.openfoam.org/features/LES.php
Based on the summary description of the LES models above, it seems to me that the following could possibly be suitable for such a meshing domain with so many refinement levels:

• kOmegaSSTSAS
• Smagorinsky2
• dynSmagorinsky
• mixedSmagorinsky
• dynMixedSmagorinsky
• locDynOneEqEddy

Look for more information about these directly in the source code or via the Doxygen code documentation: http://www.openfoam.org/docs/cpp/
Google (or any other online search engine) might help as well.

As I indicated above, stitching is only a meshing strategy. This can come in handy if you cannot mesh everything in the mesher all at once; but meshing all from the same mesh (as snappyHexMesh does it) or all at once, usually makes it easier to do get a good mesh.


From what I know, what you are looking for is a LES model that is able to handle the two kinds of meshes: coarse and fine meshes. In theory, all of them can do this, it's just that some do it better than others.
As for the wake... you'll have to balance the mesh resolution farther after the end of the blade, but you won't need to do so before the blade.

Best regards,
Bruno

Hey Bruno,
thanks for the advice, it has really helped me a lot.

- I am cheating a little bit by creating the Tunnel mesh in ICEM and using snappyHex only for the Blade :p and this would be my mesh 1
- Mesh 2 is the C-Grid i created with Salome


I will try and do a merge mesh, can you have a glance at my snappyhexDict ? i have attached with this post

the mesh is fine but after i do the snappy hex, my blade has moved every so slightly this would cause a problem when I am trying to merge the mesh with the other one made from salome right..?

Thanks,
Hasan K.J

Hi Hasan,

In "snappyHexMeshDict", the "refinementBox" is not being used anywhere.

As for mesh 1 vs mesh 2... if I'm not mistaken, Salome generates only tetrahedral cells, correct? If this is the case, merging or stitching the meshes might not go very well.
And do try to avoid overlapping the meshes, because that will lead to non-physical results.

Wait, why do you need to use ICEM to create the tunnel? Is the tunnel very complex or is it just a simple geometry?


C-Grid... I think lakeat has something for that for OpenFOAM... here you go: http://www.cfd-online.com/Forums/ope...generator.html

Best regards,
Bruno

Hey Bruno,

You have mistaken, salome is a efficient software it can create a lot of cell types.

- I have used Salome for Creating a structured C-Grid with full Hexahedral cell.

- Tunnel is a complicated geometry, and i strictly wanted hexahedral, so with ICEM a full hexahedral mesh i created, the slightly cheated by using snappyHex to put the Blade right in the middle of the full 3D hexahedral mesh.

- I remember putting refinement box around the blade :/ have i not ?

now - i want to merge the snappyhex mesh with the salome mesh.

Thanks,
Hasan K.J

I've never use Salome, only seen in brief descriptions, so I don't know specifically the full capabilities it has got. But it's very good to know how powerful it really is!

In the "snappyHexMeshDict", you only defined the refinement box in the geometry section, but didn't define what resolution should be used for it.

Hey Bruno,
My ADD is worst than i thought… I will correct it
but other than that what do you think, ? is this snappy hex good enough

what could i do about the warning from snappy saying it has moved the blade every so slightly?



refinementRegions
{
refinementBox
{
mode inside;
levels ((1E15 5));
}
}

Thanks,
Hasan K.J

The "snappyHexMeshDict" looks good enough to me.

And I have not seen the message you are referring to, so I don't know what exactly has happened :(