CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] ICEM MRF Interface - Penetrating Elements (http://www.cfd-online.com/Forums/ansys-meshing/106714-icem-mrf-interface-penetrating-elements.html)

survADe September 6, 2012 03:48

ICEM MRF Interface - Penetrating Elements
 
4 Attachment(s)
Hello ICEM users,


I need to generate a Mesh with two domains for a MRF simulation. Overall it is one cylinder filled with one fluid, whilst the outer wall is ROTATING. I cannot tell you all the details so you have to believe that an interface is necessary even though this simple case can be solved without. As there is a stationary and rotating domain it is splitted in two cylinders. The outer one is the domain with the rotating wall and it is linked via an interface to the stationary inner domain. This leads to three interface surfaces dividing the two domains. It is a very basic configuration so I don’t think I need to add geometry. However If interested I will post it.


I checked the Geometry with Blocking topology and everything is ok (all red lines). Material points are set for each domain.


After doing Tetra/Prism Meshing with ICEM 13 (Volume Meshing with Tetra Mixed and Octree Method) I get a beautiful mesh, with no mesh errors. So far I am very happy. In order to generate a MRF simulation in Fluent I need for each interface side a surface. I did this by using >Edit-Mesh/Split Mesh/Split Internal Wall (Create Volume Cells is unchecked!). Three additional parts are generated ending with “…Back”. Now If I do Mesh Check I get “Penetrating Elements” along the interface. So far all attempts to repair the surface mesh with ICEM result in merging the second interface surface (interface…_back) with the former interface, i.e I cannot perform MRF in Fluent.:mad:


I also used the un-splitted mesh in Fluent and did the job in Fluent by using >mesh/modify-zones/slit-face-zones but then I get degenerated contact points and also the mesh check in Fluent fails.


I guess there is a simple solution for this problem - how to do this in a top-down approach and not necessarily need to mesh the two parts separately. Hope there are some clever guys out there who might know the answer:).

survADe September 10, 2012 03:41

Somebody who has idea??? Maybe it is quite simple I am stuck at this point

survADe October 10, 2012 09:11

I uploaded the icem files for the problem

https://www.dropbox.com/sh/e7tp9j1t7inx71w/_DPUUkLTui

maybe this helps

Regards

Far October 10, 2012 10:43

create the two concentric regions and mesh them seperatly in ICEM and export mesh. Open these meshes in Fluent and create interface there.

survADe October 13, 2012 11:27

1 Attachment(s)
Thanks Far for the reply. The separate meshing works fine! I get no errors from icem at the concentric region.

When I read it into Fluent13 the coupled walls are automatically slitted and shadow walls are generated. Normally you can than choose from the boco type 'interface' but here it is not possible (see Figure).

Is there something wrong with the way I tried?

Regards.

Far October 13, 2012 12:21

Quote:

Originally Posted by survADe (Post 386427)
Thanks Far for the reply. The separate meshing works fine! I get no errors from icem at the concentric region.

When I read it into Fluent13 the coupled walls are automatically slitted and shadow walls are generated. Normally you can than choose from the boco type 'interface' but here it is not possible (see Figure).

Is there something wrong with the way I tried?

Regards.


So two separate meshes works fine? Right?

The method you are working doesn't seem right to me. Someone else may share their experience as well.

survADe October 13, 2012 12:52

1 Attachment(s)
Dear Far,

yes the meshing in icem works.
1.) I meshed the inner concentric volume
2.) I meshed the outer one with "Use exisiting mesh parts" checked and also once with not checked (then ICEM asks me to merge the two meshes)

I fixed the problem now!

Take the mesh from ICEM into Fluent and the walls will be automatically splitted (->shadow walls). By this you will see the same reduced BOCO options as I sketched in the previous post. Go to /mesh/modify-zones/slit-face-zone in Fluent and type in the ID of one of the interface walls. Now you are able to choose Interface.

Thanks for the help Far!

Far October 13, 2012 13:57

good info and post. Can you make it blog on cfd-online? to help the future queries?

survADe October 14, 2012 03:50

sure no problem. Done

Regards

sk692 February 4, 2015 03:26

Problem with interfaces
 
Hi survAde

I am facing the same problem with interfaces. I am working on a centrifugal pump.
I meshed it in ICEM and exported the mesh to fluent.
I did the interfacing in fluent as you indicated in your post and also tried another 2-3 ways but the results are all wrong.

Can you help me out with the problem. See if I am missing something.

You can find my problem here.

thank you


All times are GMT -4. The time now is 23:38.