[eliasmontoya]

I would really appreciate if somebody could help me with this one.

I am trying to simulate the flow around a modified mk-66 (Hydra 70) Rocket. The rocket is basically an axis-symetrical body with 3 curved fins. I have not been able t generate a mesh for the whole rocket, but I was able to mesh one third of it (of a 120 degree slice), which is repeated two more times.

Trying to obtain valid results, I defined PERIODIC boundary conditions in the planes with which I splitted the rocket. Then I set the condition as "Rotational periodic"

The mesh is generated and I think the boundary conditions are fine. I wanted to check in the simplest case I could think of (10 m/s flow, Spalart-Allmaras, etc) before switching to compressible flow and sending the job to a supercomputer, but no mather what I try to change, I always get an "Error: divergence detected in AMG solver: xxxxxxxxxx"

Thank you in advance for any help...

[PawnPace]

Hi,

Can you use a 2D mesh (I am assuming that your geometry and BCs as well as ICs are also axi-symmetric) for some crude estimates.

If you have already done this then I'm not sure about your problem.

Regards,

PawnPace

[delfel]

Hi Elias,

I've gotten that error before with the 3d rotationally periodic BCs and never figured out exactly what the problem was. If I recall right, I've seen it either when I initialize a solution on the grid or with the first iteration. I believe I got rid of the error eventually by going back to gambit and checking that the faces were linked properly (including the direction as defined by the nodes) and making sure that all the duplicate faces and edges have been cleaned up, then re-exporting the mesh.

Hope that helps,
Sean

[eliasmontoya]

PawnPace, Thank you for you reply.

I don´t know if I can actually use a 2D axis-symmetric mesh, given that the rocket is not completely axis-symmetric because of the fins. You can see the image of the rocket in my first post, if you think it is possible to use a 2D axis symmetric mesh I would really aappreciate if you told me.

Thank you again for your help.

[eliasmontoya]

delfel,

Thank you for your answer. I have already checked the mesh, and I am sure that the faces are linked properly and in the right direction. I get the error when I try to iterate, before getting the results of the first iteration. I only meshed one third of the rocket, is it right or should I mesh the whole rocket even if I am using periodic BC?

Thank you for your answer

[delfel]

Hi Elias,

You should be fine modeling only 1/3 of the geometry and using rotationally periodic BCs. I'm sure i've gotten the same error before -- i'll see if i can figure out how i fixed it.

Cheers,
-sean

[eliasmontoya]

Hi Sean,

Thanks again for your replies, I have been trying to solve my problem but still get the same result before the first iteration. I have tried using different solver options and viscous models, but still get the same AMG solver error.

If you remember how you solved it I would really appreciate your help.

Thank you again

[delfel]

Hi again Elias,

Can you tell me what your inlet and outlet BCs are? I'm wondering if it isn't a problem with the periodic BCs but with the inlet and outlet conditions - especially if you're are intending to run it as a compressible problem eventually but are currently trying to run it as incompressible.

I would also recommend running the case as laminar at first and then adding the turbulence model later. You could also try initializing the solution to something more realistic (i'm guessing you're starting at zero).

Final thought -- if you really want to see if it's a problem with the periodic BCs, change them to wall boundaries in gambit and re-export the mesh and see what happens. If you still have the same divergence troubles, then it's likely not the periodic boundaries causing it.

-sean

[eliasmontoya]

Hi Sean,

My control volume is 1/3 of a cylinder, obviously parallel to the rocket's body. Right now my BCs are Velocity inlet for both the "top" of the cylinder and the lateral rounded face, and periodic for the faces with which I divided the cylinder in 3. The "Bottom" face is a pressure outlet. Right now I am working with incompressible laminar flow, and still doesn't work when I use periodic faces. However I did what you suggested me of changing them to wall faces and then they did work, so the problem is obviously with the periodic BC.

The only weird thing that I see when reading the mesh is that there is a "shadow" zone for the periodic faces, which fluent skips because it is not referenced by the grid. Maybe this has something to do with my problem.

I tried everything from the beginning, and even meshed the volume again with a better mesh, but still the same result.

thanks again

Elias

Thanks again

[eliasmontoya]

Hi Sean,

I already found out the problem. It was that I had not defined the axis of rotation properly, but now that I have changed it I am at least getting iterations and everything looks good.

Thank you again for your help,

Cheers,

Elias

[delfel]

Great! Congrats and good luck,

-sean