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] Delete wall between two regions (http://www.cfd-online.com/Forums/ansys-meshing/123813-delete-wall-between-two-regions.html)

cscalo September 21, 2013 19:35

Delete wall between two regions
 
Hello ICEM crowd,

I need to create a hexa mesh with two different adjacent regions, say FLUID0 and FLUID1. I can do this easily by creating a "Part" for each region. ICEM CFD thinks that these two parts are two different materials. This wouldn't be a problem if only ICEM didn't create a wall in between them.

I read on this forum that is possible to setup the hexa mesh (in Global Mesh Parameters.. or something like that) so that it doesn't do this. I'm not sure how to do this.

I basically need one mesh with regions of it that have different labels ("FLUID0" and "FLUID1"). I need these labels in my solver in these specific regions to activate certain functionalities.

I would appreciate your help on this! Thanks!

diamondx September 22, 2013 21:24

keep that wall and make it "interior" when setting the boundary condition in the output tab

cscalo September 22, 2013 22:13

Hi Diamondx - thanks for your reply. Unfortunately it didn't work. My solver tells me that some faces "are not associated" with the internal wall. Is there something deeper and non-Fluent dependent that I can do? Something in Global Mesh Setup for example? I simply want to leave the labels to the volume with no physical surface dividing them.

Thanks!

Far September 22, 2013 23:29

Quote:

Originally Posted by cscalo (Post 452922)
Hello ICEM crowd,

I need to create a hexa mesh with two different adjacent regions, say FLUID0 and FLUID1. I can do this easily by creating a "Part" for each region. ICEM CFD thinks that these two parts are two different materials. This wouldn't be a problem if only ICEM didn't create a wall in between them.

I read on this forum that is possible to setup the hexa mesh (in Global Mesh Parameters.. or something like that) so that it doesn't do this. I'm not sure how to do this.

I basically need one mesh with regions of it that have different labels ("FLUID0" and "FLUID1"). I need these labels in my solver in these specific regions to activate certain functionalities.

I would appreciate your help on this! Thanks!

HEXA or TETRA ?

cscalo September 22, 2013 23:33

Hi Far - My mesh is purely HEXA... I think it was you (in some post I read) who said that you can do this at the Global Mesh Setup level.. thanks for your help.

Far September 23, 2013 01:22

Are you associating face to part for the interface?

Far September 23, 2013 01:34

Quote:

Originally Posted by diamondx (Post 453027)
keep that wall and make it "interior" when setting the boundary condition in the output tab

Yes exactly. Still you will see the boundary condition (interface or whatever name you choose) in fluent (as int_interface) but now it interiour. Means it will pass the flow as usual.

cscalo September 23, 2013 01:37

yes.. I create a surface in between the two regions and that surface is added to a "PART" called, say, SHARED_WALL. This (surface) part is a boundary in between the two regions which have different labels (or part names). I would like this boundary to disappear before my mesh gets to the solver. If I define it as an internal face I feel like that would work for Fluent but for an in-house solver I think I need that wall to be removed before (at the connectivity level).

I will retry as you say -- labeling that surface as an "internal_surface" -- and see if I can have my solver accept it if that's the only way I can do such a thing with ICEM.

Thanks!

Far September 23, 2013 01:49

I am not sure about the in-house solver. For this, Simon is the most appropriate person to answer or you can contact ANSYS support.

PSYMN September 23, 2013 14:36

Yes, of course there is an automatic way to turn that off that doesn't require creating any geometry, etc... The fact that ICEM CFD Hexa defaults to project a face between two materials to the nearest surface is meant as a convenience, not to cause trouble. ;^)

If you have two blocking materials, say FLUID1 and FLUID2, and you don't want to have default face to surface projection between blocks of these two materials (usually because you want these in different materials for selection or other "non-physics" reasons);
  • Blocking tab>Blocking Associations>Associate Face to Surface...
  • You will find a bunch of methods in there. One of them is "Shared Wall".
  • Switch the radio button to "Shared Wall" and Select all the volume parts that you wish to allow adjacent without surface projection between. The command is iterative, so cancel (or accept without selecting) after the ones you want disappear from the options.
  • Switch the Radio Button for "Shared surface elements" to "None", so that no surface projection will be the default between these materials.
  • Apply

Let us know if that is what you were looking for... Of course, this just changes the default. If you want to associate a face between these blocks to a surface, you can always do that manually.


All times are GMT -4. The time now is 02:29.