Multizone issues (on my project)
 

Greetings:
I am currently doing a Ph D on Chemical Engineering, working with fluidized bed granulation. At the moment I am trying to simulate the airflow inside the complete system. The system is a pilot scale fluidized bed we have in our institution. This is the starting point on what i will do after i can run multiple simulations with a more complex system.

I am able to use Ansys Meshing software, or if needed, the meshing software for openfoam
The system I am trying to simulate is similar to the one present in the paper:
https://www.researchgate.net/publica..._bed_equipment
If you read the paper, they made use of Gambit Software to produce the grid, and the number of elements is between 200k-240k. They used a unstructured mesh (hexa-tetra)

My system:
http://s24.postimg.org/yt3ammvsh/Geom.jpg
Zoom to the grid area: (52 smalls cylinders)
http://s24.postimg.org/vxq7frrsh/grid.jpg


What I want to achieve:
I am trying to make use of the multi-zone method on the ansys meshing to use hexaedrical mesh on the pipes, the extension, the grid, and if I can in the cone. In the plenum I will use a prims and tetra because of how the flow move.
My issues:
If I work with only one body, when I check sweepeable areas on Ansys meshing I can’t select anything. I can’t generate mesh even choosing source and target face on the geometry selection on multizone
If I work with more than one body, using slice, I end with too many contact regions, and this generate in fluent a lots of messages about issues with interface areas.
When I use cut-cell as assembly method, I see convergence issues with the coupled solver at fluent. I get the lowest number of elements for the grid, but even making a finer mesh I don’t get good convergence.
Most of the tutorials I found about multiple bodys or multiple parts are for mechanics and not for fluid dynamics.
I am asking advice about:
Should I work with multi-body? (To use multi-zone more easy), if so, any advice on how to do it right will be appreciated
If I work with multiple body, how I can share the mesh topology, without losing the areas that are sweepables

Boundary conditions:
Boundary condition at the pipe inlet: Average velocity or pressure (I have experimental data on both)
Boundary condition at the extension outlet: Pressure (again, I have experimental data, but I can choose to work with 0 at the outlet pressure)
I have Match number over 0.3 on the distribution grid in some cases, so I am using Ideal gas or SRK to obtain air density. Is the only area where this happens


If needed i can upload the geometry.

Thanks in advance, and sorry for the way I write in English,
Best regards
Carlos

First off, your English is great. Don't sweat about it.

I'm just going to throw some basic things out there, not sure how much you have used Meshing:

I would advice you to have multiple volumes gathered in one group in DesignModeler. This way you wouldn't have to worry about the interfaces because they are taken care of automatically. Secondly, you could use Multizone with hexa only option instead of sweeping if you're facing adversity from the shape of the system. This should help you getting more hexahedral cells in your system.

Personally, I haven't been able to use the cut cell method effectively on anything remotely complex. That might -of course- be due to my own skills and amount of effort invested in studying the method.

Hope you get further with your case, best of luck!

Divergence, thanks for the reply
Working with parts reduced a lot the need to check and remake the connections and the issues with the empty surface areas.
I still get some of this messages:
Note: zone-surface: cannot create surface from sliding interface zone.
Creating empty surface.

But at least i can use Multizone.

Now I have a mesh with this values:
Minimum Orthogonal Quality = 3.59060e-01
Maximum Ortho Skew = 6.40940e-01
Maximum Aspect Ratio = 3.34314e+01

I think those values are really good compared with I was getting (Skew close to 0.95, Orthogonal close to 0.05 and aspect ratio more than 300)
At the moment I am not using inflation (The beauty of multi-zone is that one can use the “inflate this method” option)

Sadly, the first mesh I generated is a monster of 840k elements (with my current laptop my limit is 2.7m) but at least is a step in the right direction. At the moment I am making the mesh and geometry on my laptop and the simulation on the pc at work.
In the 3rd image the number of elements is 540k. A lot less element than the 840k. I will keep working on it to find the best meshing possible

This is a pic:
http://s14.postimg.org/rxez8g125/mesh1.jpg
I am using share topology but it doesnt share it. Between this 2 parts, idk why.

http://s14.postimg.org/l4emc6a8t/mesh2.jpg

http://s14.postimg.org/mxhj0hvfh/mesh3.jpg

I found to that the face-split feature is really useful, so later i will post some pics of what i am doing with this.

If anyone had the issue of:

Note: zone-surface: cannot create surface from sliding interface zone.
Creating empty surface.

And know any way to resolve it, thanks in advance

Glad to hear you're making progress!

Couple of questions:

-Do you need the interfaces for something for example in your calculations?
-Are each and every volume in a single group? Are there more than one active group?

The meshes of the extension and the cone volumes don't seem to be matching, which is what they should do if they are in one group. That whole "sliding-interface" trouble be washed away if the grouping would be working as desired.

Thanks again for the reply Divergence,
About the questions:
1.- I don’t need interfaces. I was working with 4 parts not grouped so ansys meshing and fluent keep generating them. In my final system (a pilot scale fluidized bed granulator) there will be one interface at the bottom of the cone to avoid the solid phase moving downwards. But now I only care about the airflow and working with the simplest system
2.- As I said before, I was working with 4 parts and I didn’t realize the system wasn’t matching the topology of the different body’s until I saw the image I upload. That was a mistake I fixed later. I couldn’t upload the new images because I can use fluent in my workplace only.

This is the mesh now, without any inflation and with mesh matching:
http://s14.postimg.org/blpbnbgi5/mesh4.jpg

I really dont know why i cant make this kind of mesh working with only 1 body.

I will add inflation later to get better wall results, but for the test I am doing at the moment, this way to generate the mesh is ok.

I am reading the fluent theory guide and I can’t find what is the recommended range of y+ to use with Realizable K epsilon turbulence model working with Menter- Lechner wall treatment. Most of the information say it is a y+ insensitive method, but on the other hand it say that a y+ close to 1 is recommended. For the y+ i am getting i can use standar wall functions in most of the system (except on the grid) but i will refine the mesh later so probably i will need to change to another wall treatmen aproach

It seems that my replies and post need administrator approve so if I don’t reply fast is because of that or that I am not in my workplace pc

Best regards
Carlos

Do the following before you export the mesh:
1. In Ansys meshing make sure that all the parts are declared as solid.
2. If interfaces are created automatically, delete them.
3. Select all the parts and make a 'name selection' e.g. fluidRegion.

These should help resolve the interface issue.

Typo
In Ansys meshing make sure that all the parts are declared as fluid.

Vasava, thanks for the reply.


I guess that with point 2:
2. If interfaces are created automatically, delete them.

you mean to delete the contact regions that are automatically created on Ansys Meshing when one load the geometry.
The option 1 are 3 are usefull to reduce the boundary conditions that fluent generate later

If i do that i end with non matching faces on the connections between the diferents bodys. Maybe i am doing something wrong.

Still with the way i worked before i removed the issue of the interface and i have matching faces.

Again thanks for the reply

Best regards
Carlos

do "named selection" for all the faces which you require
delete all the interfaces which it has created automatically.
make sure you have done named selection of both faces of interfaces separately.

You can introduce 'matching' but then you have to use same type of meshes (tetra or hexa) for all the bodies.