bubblefoam totally failed on unstructured mesh.
 

Sorry, but yes, I have to concede that bubblefoam totally cant run on an unstructured mesh.
I even dont need to attach my case.
Just generate any simple cyclinder with an inlet,wall,outlet with an unstructured mesh. and run bubblefoam or twophaseeulerfoam.


bang!!......blowing up!


anyway,Thats is not my expected,I want a plausible suggestion how to prevent blowing up.

If you want people to solve a problem for you, you should provide much much more details.

So you DO have to upload your case, because nobody is going to take the effort of making a mesh and running a simulation just to see what you mean.

If you show that you have put some effort into thinking about the issue and trying to solve it and share this information, then somebody might be willing (and be able) to help you.

Hi Michiel:

Thank you very much for my consideration. actually I have done lots of works about bubblefoam, even all of them are extremely simple ones.




http://www.cfd-online.com/Forums/ope...tml#post396032
in this thread I tried use structured mesh on bubblefoam but failed, so I have to use unstructured mesh.then....

http://www.cfd-online.com/Forums/ope...behaviour.html
in this thread I have tried unstructured mesh on twoPhaseEulerFoam,or bubblefoam,it cant get convergence.

untill now I dont know if bubblefoam can handle unstructured mesh...

I cant upload my case because the fluent.msh is large.... but I can upload a image.
its a very simple case. if anyone can generate a mesh then just put it in mycase folder,the fluentMeshToFoam fluent.msh, setFields . bubbleFoam..
you will see the result.


everytime I receive an Email, I would be more closer to my success...thats exciting.

Thats quite weird, is there anyone tried an unstructured mesh on bubblefoam?

nobody is here?...

get a dropbox account and put the mesh there.

why do you have different inlet velocities for the phases?

Thank you for reminding me the dropbox Niklas. I upload my case on hotfire. you can chekc it out there.
https://hotfile.com/dl/184355810/d49...p.html?lang=en
https://hotfile.com/dl/184356440/5e7...p.html?lang=en


you can run it directly as of I have set the alpha field and generated the mesh.:

twoPhaseEulerFoam


U1 is the gas velocity , U2 is the liquid velocity, there is only air get in the column,so U2 inlet is zero.

If you can give me any assistance I would be very appreciated.

doesnt work. hotfile is terrible.
cant download and now it says im downloading and I can only download 1 at a time.

here is a link on dropbox~

https://www.dropbox.com/s/1v6n8cf39n...structured.zip
https://www.dropbox.com/s/mguy6w6gm9...structured.zip

Looks like only FOAM developers can tackle this problem?...

the main problem is the mesh-quality at the interface. I would try to remake the mesh, slightly finer and also to add some outer corrections instead of running in piso mode.

I dont know if that is sufficient, but its impossible to get it working with that mesh.

Thank you very very much. although this problem has not been handled.I would be very thankful for your assistance.

um...maybe twophaseeulerfoam in next edition of OpenFOAM would be better on dealing with this mesh problem.? But I dont have much time to wait.....

add this to controlDict and watch what happens to the velocities

Dear Niklas,
yeah, thats help, somthing wired about velocity fields. but finally,I dont know how to run bubblefoam or twophaseeulerfoam on that mesh. is this regarding to the model itself? if its ture. that is far beyond my ability.

Use the "upwind" scheme for the divergence term of U1 and U2, and use the "uncorrected" option for Laplacians and snGrad. Also, fix the maximum time step to a much lower value than 1s, to avoid too strong fluctuations in the time-step.

I attach the files I used, and it ran up to 0.18s, then I stopped.

P.S. There is no reason to use an unstructured mesh with such a simple geometry :-)

Oh my GOD! Thank you so very much Prof. alberto. I have been waiting for your reply. coz I know you can handle this question. I will try this . and update this thread if its necessary.

Well~Prof.Alberto, I have tried, but the result looks...unsatisfactory.the image has been attached.If you have time,could you do me a favor check this thing out again please? Thank you.
BTW,I really admire what you have done in CFD research.

You should improve your mesh resolution if you want to obtain reliable results.

P.S. Alberto works just fine, no need of titles ;-)

Okay! I will remesh and try it, and update the result! Thanks alberto~

May I know why you are trying to use a tetrahedral mesh?

Because I want to simulate the velocity field in a stirred tank which has two or more complex impeller and other things. the liquid is xanthan gum. and the air was injected. ofcourse I want to use hex mesh. but its too hard the create it. the image has been attached.
Wish someday I can fly to IOWA..haha
I will try to make a fine tet mesh and update later,now its very late in my country~but if you are interested in my research just ask me I will give you a detailed reply~

For your type of flow you will need to consider non-Newtonian flow models too, which are not available in twoPhaseEulerFoam.

..............I just thought it could be set just like interFoam..:(:(:( oh, I am facing a real problem.

I think I should post it here, sorry.


More details see here,http://www.cfd-online.com/Forums/ope...tml#post399837

Um....looks like this problem still exists.

Its been a long while.

But until in FOAM　2.2.0, twoPhaseEulerFoam and bubbleFoam still cannot solve tet mesh.

Hi guys,

A little success.Regards to twoPhaseEulerFoam. I spent several days learning snappyhexmesh, and this solver can deal with this mesh.

Hi, sharonyue!

I am also facing the same problem with this thread,
I also tried to use snappyHexMesh to generate a more or less okay mesh for a stirred tank, but it turned out there were always prism elements.
So, I am wondering did you manage to get rid of prisms in your case?
If so, how did you make it?

Many thanks!

Regards,

I am not sure what solver you are using and in what version of OpenFOAM, but twoPhaseEulerFoam has been deeply modified in recent releases.

I would suggest you use OpenFOAM 4.x (Foundation), and take a look at reactingTwoPhaseEulerFoam, which has been much more robust in my experience.

Successfully using tet meshes is a question of choosing the appropriate schemes, so it would be useful to see what you are using in fvSchemes / fvSolution. If they come from the tutorials, it may not be ideal.

I hope this helps.

Hi Alberto,

Very happy to have your help here.
You just helped me a lot in learning OpenQBMM a while ago, I am Dang.....
As you know, I need to develop a two-phase flow solver based on OpenQBMM,
Now I am struggling on that...
I solved the above problem by creating pure Hex mesh for Rushton turbine using blockMesh.
and also changed some settings in fvSchemes/fvSolution after searching around in this platform.
But I still have two difficulties:
1. I will mainly use multiple pitch blade turbines, which are far more difficult to generate Hex mesh by blockMesh. I noticed your group have done wonderful job on this recently by using Pointwise (9th International Conference on Multiphase Flow). In a presentation by Xiaofei Hu, your mesh is so impressive, could you please shed some lights as regard to how to add/mesh zero-thickness blades/walls in pointwise?

2. I also tested multiphaseEulerFoam in a gas-liquid stirred tank, but failed to inject gas from a sparger by using the attached "fvOptions" file. This file is okay for twoPhaseEulerFoam. Do you have some suggestions on this?

By the way, I used both FOAM.3.0.1 and 2.4.

Many thanks in advance!

Best regards,

Yes, I remember. :)
I am working on a similar problem (bubble columns) with a student of mine, but the code isn't public yet.

A zero-thickness surface in Pointwise is simply a face (domain) in a 3D block, so you need to create the domain for each blade, mesh it, and typically project/extrude or connect to another face to build the 3D block.

We have worked on very large-scale industrial reactors, with complex stirrers, which were too tedious to be meshed in a CAD-like environment. We obtained excellent results, comparable to those in Pointwise, with snappyHexMesh, once we figured the settings out, and properly defined the STL (if you use SolidWorks, feel free to maximize the export quality).

I have not used fvOptions to simulate the sparger. In our case, we mesh the actual sparger because it is big enough to alter the flow.

Our cases were mostly done with reactingTwoPhaseEulerFoam/reactingMultiphaseEulerFoam in OpenFOAM-dev, which is currently in OpenFOAM 4.0. My post-doc definitely knows these technicalities better than me, but I am quite sure she didn't use 3.0 much.

Regards,

Hi Alberto,

Thanks for your kind reply.
I have tried hard to get rid of prisms by using snappyHexMesh, but still be bothered by them. Do you have some suggestions on this? According to your experiences, which parameters in snappyHexMeshare are crucial to your success?
Is it possible because of you use a large scale tank?
While I work on a lab-scale tank with ~ 0.3 m in diameter (I used Salome to generate STL file).

BTW, I played with twoPhaseEulerFoam these days, but have no clear idea about
"maxFullyDispersedAlpha" and "maxPartlyDispersedAlpha" under "blending" in "phaseProperties". Could you explained them?

Thanks!


Best,

We make the STL separating the following parts in different STL files:

• Tank
• Each impeller
• Parts of the shaft between impellers
• Shaft in the top of the reactor (from outside the rotating zone to the top of the tank)

This allows to specify different refinement levels. We also use the implicit feature detection, which seems to better conform the mesh to the surface in all of our cases. I would recommend you create a fine-enough blockMesh box, to start from a decent mesh resolution, rather than a very coarse one.

We just submitted a paper where we used snappyHexMesh with a tank whose diameter is smaller than yours, and we obtained a good mesh.

Blending is used to stabilize the solution when there is phase inversion. This is achieved by blending the contribution of the phases to the momentum exchange term. The thresholds you refer to are parameters of the blending function you choose to use for the force model. I would stick to the defaults, if you simulate gas-liquid systems, since they have been tested for those.

Hi Alberto,
Thanks very much for your kind reply.
The information is helpful!

Best regards,

[/QUOTE]
Hi, Alberto,

I think it's better to open a new thread to disccuss the reactingMultiphaseEulerFoam issues.
So, I opened a new thread at the following link:

http://www.cfd-online.com/Forums/ope...tml#post615294

Hope you could take a look. :)

Best regards,