CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

Boundary type for interface boundaries

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 7, 2012, 07:37
Default Boundary type for interface boundaries
  #1
New Member
 
Rachit Prasad
Join Date: Jun 2011
Location: Blacksburg, Virginia
Posts: 29
Rep Power: 6
Rachit is on a distinguished road
Hi everyone!

I have been creating a mesh which is two regions. In both the regions, the meshing method is different. When I create an interface from two boundaries from the two separate region, then what should be the boundary type for these boundaries? As in, all that should happen here is information exchange, why have a boundary type here?

Thanks in advance!

Regards,
Rachit
Rachit is offline   Reply With Quote

Old   February 7, 2012, 07:46
Default
  #2
Member
 
Join Date: Feb 2011
Location: DE-PB
Posts: 56
Rep Power: 6
willimanili is on a distinguished road
If i understand you right you have two regions with one mesh continuum for each, right?! (two mesh continua!)
I'm sry but it isnt possible to create an interface between two regions with different mesh continua.
Use one mesh continuum for both regions, then you can create an interface between them. The boundary type for the boundaries which you would like to connect by the interface is just important for the areas where no interface will be created and depends on the behavior of your simulation model.
willimanili is offline   Reply With Quote

Old   February 7, 2012, 08:28
Default
  #3
New Member
 
Rachit Prasad
Join Date: Jun 2011
Location: Blacksburg, Virginia
Posts: 29
Rep Power: 6
Rachit is on a distinguished road
Okkk...I wasn't aware of that...thanks!

But then how should I accomplish my goal? I have been told to create a highly refined structured C-mesh around an airfoil (I will use trimmer for that) followed by a tetrahedral mesh in the background. How should I create such a hybrid mesh? I have been told not to use prism layers as prism layers option produces an O-mesh around the airfoil and hence the quality of mesh is not good at the trailing edge.

Any ideas?
Rachit is offline   Reply With Quote

Old   February 7, 2012, 09:49
Default
  #4
Member
 
Join Date: Feb 2011
Location: DE-PB
Posts: 56
Rep Power: 6
willimanili is on a distinguished road
From the user guide, Chapter Volume Meshing (V6.06.017):


".... For multi-region cases, a conformal mesh at the interface
one of region and the next is currently possible for the tetrahedral and
polyhedral mesh types as part of the meshing process. This option is
currently not supported for the trimmed cell mesher.
Different mesh types can also be used for different mesh regions if desired
by using a different mesh continuum for each region. A conformal mesh
interface at inter-region boundaries is not supported in this case.
...."

So it is impossible to generate such a trimmer hybrid mesh in ccm+.

In your case i would use poly mesh plus well solved prism layer boundary. Also i would refine the mesh with volumetric control at the trailing edge and the area downstream the airfoil.
willimanili is offline   Reply With Quote

Old   February 7, 2012, 10:31
Default
  #5
New Member
 
Rachit Prasad
Join Date: Jun 2011
Location: Blacksburg, Virginia
Posts: 29
Rep Power: 6
Rachit is on a distinguished road
Thanks for your insight!

Could you just clarify what you mean by "well solved" prism layer boundary?

I have tried by increasing the mesh density in the wake region using volumetric control (see picture), but it didn't give me the result I was looking for. I have been meaning to capture the vortex shedding pattern from the airfoil under low Reynolds no flow. But the vortex seems to dissipate out after formation. Is it because of faulty mesh? Or am I going wrong in some other aspect?

Thanks in advance!

Regards,
Rachit
Attached Images
File Type: jpg mesh 2.jpg (91.9 KB, 39 views)
Rachit is offline   Reply With Quote

Old   February 7, 2012, 11:09
Default
  #6
Member
 
Join Date: Feb 2011
Location: DE-PB
Posts: 56
Rep Power: 6
willimanili is on a distinguished road
"Well solved" means that you have as much layers as you need to resolve your boundary layer flow gradients in the way you need. In your case the mesh seems to be ok on the first view.

Are you using steady or unsteady solver?! Which turbulence model do you use?!

I give my best to answer specific questions, i am sry that i cant give you an detailed explanation how to set up your simulation. But there are a lot of informations in the user guide, books, forums, websites e.g. which will help you. Just spend some time on it.
willimanili is offline   Reply With Quote

Old   February 18, 2012, 07:56
Default
  #7
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
You should use either a trimmed mesh or a poly mesh. Tetras don't work very well with ccm+.
Also have a look on the aspect ration of the near wall cells (first prism layer), it seems to be a very flat cell. Maybe you have to refine a little bit at the surface of your airfoil.

And assuming you can create a structured C-mesh (ccm+ doesn't support that with standard meshing models, maybe the airfoil wizard will do), you CAN create hybrid mesh. So willimanili's answe ist just wrong. You can create an interface between arbitrary meshes. What you can't do is creating a CONFORMAL interface.
Without a conformal interface, your solution will smear a little at the interface, but it shouldn't have too much impact on the solution when the interface is far enough from the region of interest.
abdul099 is offline   Reply With Quote

Old   February 22, 2012, 05:30
Default
  #8
New Member
 
clement
Join Date: May 2011
Location: München
Posts: 12
Rep Power: 6
Clementhuon is on a distinguished road
Quote:
Originally Posted by willimanili View Post
I'm sry but it isnt possible to create an interface between two regions with different mesh continua.
Use one mesh continuum for both regions, then you can create an interface between them. The boundary type for the boundaries which you would like to connect by the interface is just important for the areas where no interface will be created and depends on the behavior of your simulation model.
Hi willimanili,

I don't understand your explanation. I'm actually studying a wheel with brake system with a rotation velocity. The inner part of my brake disk (the cooling channel) is set as another region and a MRF rotation is applied on it.

The both regions are meshed with two different mesh continua (one trimmed for the wheel and one poly for the cooling channel) and both region a coupled with an interface. And that works fine !!!

One part of the interface is meshed as poly and the otherone with trimmer, the intersection Tolerance is 0.05 and a get 100% surface intersection for both part of the interface. The only thing you really have to care is to disable the boundary layer on this interface.

I really think this is possible to do this kind of mesh (i'm actually doing it) !

Bye
Clementhuon is offline   Reply With Quote

Old   February 22, 2012, 06:32
Default
  #9
Member
 
Join Date: Feb 2011
Location: DE-PB
Posts: 56
Rep Power: 6
willimanili is on a distinguished road
Yes it will work, but it isnt a conformal interface, like abdul has already mentioned.

Quote:
Without a conformal interface, your solution will smear a little at the interface, but it shouldn't have too much impact on the solution when the interface is far enough from the region of interest.
willimanili is offline   Reply With Quote

Old   February 24, 2012, 07:28
Default
  #10
Member
 
Oliver Lauer
Join Date: Mar 2009
Location: Coburg
Posts: 57
Rep Power: 8
olauer is on a distinguished road
Quote:
Originally Posted by Rachit View Post
Hi everyone!

I have been creating a mesh which is two regions. In both the regions, the meshing method is different. When I create an interface from two boundaries from the two separate region, then what should be the boundary type for these boundaries? As in, all that should happen here is information exchange, why have a boundary type here?
The answer to this initial question is: wall boundary, especially if it should be connected 100%.

Quote:
Originally Posted by willimanili View Post
If i understand you right you have two regions with one mesh continuum for each, right?! (two mesh continua!)
I'm sry but it isnt possible to create an interface between two regions with different mesh continua.
Use one mesh continuum for both regions, then you can create an interface between them. The boundary type for the boundaries which you would like to connect by the interface is just important for the areas where no interface will be created and depends on the behavior of your simulation model.
The first part of this answer is definitely wrong, an interface can be created, but it is not conformal, as already mentioned (so what, some additional faces are created for the cells). The second part is correct and helpful.
olauer is offline   Reply With Quote

Reply

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
turbulent jet simulation antonio_ing OpenFOAM Running, Solving & CFD 5 September 16, 2010 02:31
pipe flow with heat transfer Fabian OpenFOAM 2 December 12, 2009 05:53
Concentric tube heat exchanger (Air-Water) Young CFX 5 October 6, 2008 23:17
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50
Please help with flow around car modelling! Tudor Miron CFX 17 March 19, 2004 20:23


All times are GMT -4. The time now is 00:25.