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,