CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ANSYS Meshing] Multizone issues (on my project)

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 5, 2016, 13:13
Default Multizone issues (on my project)
  #1
New Member
 
C. Renaudo
Join Date: Feb 2016
Posts: 5
Rep Power: 2
crenaudo is on a distinguished road
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:

Zoom to the grid area: (52 smalls cylinders)



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 canít select anything. I canít 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 donít 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
crenaudo is offline   Reply With Quote

Old   April 7, 2016, 06:20
Default
  #2
New Member
 
Join Date: Mar 2014
Posts: 16
Rep Power: 4
divergence is on a distinguished road
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 is offline   Reply With Quote

Old   April 7, 2016, 10:29
Default
  #3
New Member
 
C. Renaudo
Join Date: Feb 2016
Posts: 5
Rep Power: 2
crenaudo is on a distinguished road
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 ďinflate this methodĒ 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:

I am using share topology but it doesnt share it. Between this 2 parts, idk why.





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
crenaudo is offline   Reply With Quote

Old   April 8, 2016, 06:22
Default
  #4
New Member
 
Join Date: Mar 2014
Posts: 16
Rep Power: 4
divergence is on a distinguished road
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.
divergence is offline   Reply With Quote

Old   April 8, 2016, 08:19
Default
  #5
New Member
 
C. Renaudo
Join Date: Feb 2016
Posts: 5
Rep Power: 2
crenaudo is on a distinguished road
Thanks again for the reply Divergence,
About the questions:
1.- I donít 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 didnít realize the system wasnít matching the topology of the different bodyís until I saw the image I upload. That was a mistake I fixed later. I couldnít 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:


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 canít 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 donít reply fast is because of that or that I am not in my workplace pc

Best regards
Carlos
crenaudo is offline   Reply With Quote

Old   April 12, 2016, 03:06
Default
  #6
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
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.

Last edited by vasava; April 12, 2016 at 03:11. Reason: Typo
vasava is offline   Reply With Quote

Old   April 12, 2016, 09:39
Default
  #7
New Member
 
C. Renaudo
Join Date: Feb 2016
Posts: 5
Rep Power: 2
crenaudo is on a distinguished road
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
crenaudo is offline   Reply With Quote

Old   April 12, 2016, 23:00
Default
  #8
Senior Member
 
Join Date: Apr 2014
Location: Not Sure
Posts: 506
Rep Power: 6
Kapi is on a distinguished road
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.
Kapi is offline   Reply With Quote

Old   April 13, 2016, 02:59
Default
  #9
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 682
Rep Power: 15
vasava will become famous soon enough
Quote:
Originally Posted by crenaudo View Post
Vasava, thanks for the reply.
If i do that i end with non matching faces on the connections between the diferents bodys. Maybe i am doing something wrong.
Carlos
You can introduce 'matching' but then you have to use same type of meshes (tetra or hexa) for all the bodies.
vasava is offline   Reply With Quote

Reply

Tags
geometry, mesh, multizone

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFOAM v3.0+ ?? SBusch OpenFOAM 21 October 15, 2016 12:52
CoCoons Project - Community-driven Documentation on OpenFOAMģ Technology holger_marschall OpenFOAM Announcements from Other Sources 3 December 13, 2013 10:14
The FOAM Documentation Project - SHUT-DOWN holger_marschall OpenFOAM 242 March 7, 2013 13:30
"Sharing Violation on path...*wbpj" project gone MainzerKaiser ANSYS 0 February 23, 2012 05:59
CFD project idea John Cleveland Main CFD Forum 4 March 8, 2005 13:55


All times are GMT -4. The time now is 12:59.