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

Problem with tet-tet mesh merging (ICEM)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 10, 2010, 17:37
Default Problem with tet-tet mesh merging (ICEM)
  #1
srr
New Member
 
srr
Join Date: Feb 2010
Posts: 25
Rep Power: 7
srr is on a distinguished road
Hi all,

I am trying to mesh an aerodynamic domain, where one smaller cube is inside of another bigger and which symmetry surfaces are in the same plane (one contents the other). I need a really fine mesh close to the walls of my object (the smaller cube) and coarser far away from it. In order to achieve that, and taking into account that my PC is not good enough to do that in one step, I am trying to do two separate tet meshes. After I got it, I merge them, selecting the common surfaces and frozen the inside mesh. When this is done and I checked the mesh I got some problems in the vertice where the symmetry surfaces are in contact.

I have tried to merge nodes but that doent work. Does anyone have an idea of what can I do?

I apreciate any help you can give me

Thank you
srr is offline   Reply With Quote

Old   December 13, 2010, 07:09
Default
  #2
Member
 
jeevan kumar
Join Date: Mar 2009
Posts: 81
Rep Power: 8
jeevankumarb is on a distinguished road
what problem you are getting. is it multiple edges?
jeevankumarb is offline   Reply With Quote

Old   December 13, 2010, 13:28
Default Guidelines and rules
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Yea, I'm not really understanding what is going wrong either... You could work on your error description or possibly provide an image...

Are you saying your machine is not big enough to mesh the full domain that you need, so you are meshing a sub domain finely and then coarse meshing the surrounding domain and then merging at the interface between the two? This should work, but there are guidelines and rules to follow.

1) Did you set the size on the interface to approximately the smaller size? If it is just 3 or so times bigger, that can be overcome when the merge meshes tool automatically subdivides the larger tetra elements to match up, but that comes at a serious quality penalty. I would suggest meshing the inner domain first, then looking at the sizes on the interface part (you can measure if you didn't actually set a size). Then use that same size on the interface surfaces of the outer domain.

2) Are you following the other rules of merge meshes? There are numerous posts on CFD-Online about this. Rules include that the interface part must be fully used in the interface and must be bounded by a perimeter curves and the mesh on both sides must be projected to those curves...

Another option, depending on your solver, is to not merge the two domains... For instance, CFX supports a non conformal mesh interface very well. It interpolates across. Ask about that in your particular solver forum.
PSYMN is offline   Reply With Quote

Old   December 22, 2010, 23:26
Default
  #4
srr
New Member
 
srr
Join Date: Feb 2010
Posts: 25
Rep Power: 7
srr is on a distinguished road
Hi PSYMN thank you for your response

Yes what I did was mesh the inner domain first and the outer later using the same tet size on the interface surfaces. All the interface is defined when I merge the meshes, even the perimeter curve (anyway I think there is the problem), but I am not sure if I should do something aditional on this curve.

I aldo tried to calculaste with non conformal mesh in FLuent but I got some walls on the vertices. I upload some images showing the problems I found. Sorry about the boxes on the images but those are because of non disclosure agreement, hope you understand.

Thank you in advance

Regards
Attached Images
File Type: jpg non conformal mesh.jpg (48.3 KB, 46 views)
File Type: jpg error in mesh.jpg (62.7 KB, 48 views)
srr is offline   Reply With Quote

Old   December 23, 2010, 15:27
Default Single edge check...
  #5
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It looks like the corner nodes were not merged...

Please go back into the mesh and do a check for single edges. I am guessing you will find 4 on each corner forming a shape like this ^.

These are because you had the curves associated, but not points. You can prevent this next time by making sure that you have points so that your tetra mesh will capture them automatically. For hexa mesh, you must also associate the corner vertex with its point...

To fix it in mesh editing, you can just go to Edit Mesh => Merge Nodes and select the pair of nodes that will join the 4 single edges into 2...
PSYMN is offline   Reply With Quote

Old   December 23, 2010, 15:31
Question Multiple....????
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Actually, as I moved on, It occurred to me that your multiple edges might be strange... These are usually for a T connection or something like that in a 3D model. If this is a 3D model and just the symmetry or periodic face of a 3D model, then you probably just need to delete your interface shells before moving on to the solver. No worries.

If this is a 2D model, Is the 2D mesh overlapping in this area? Can you zoom in on a corner where you see these multiple edges and see what is going on...? Turn off the surfaces so the iso-parametric lines don't cause confusion. While in there, see if you can determine which 3 or more elements are sharing those edges... If you can take another zoomed in image, I may have a better idea of where you went wrong...
PSYMN is offline   Reply With Quote

Old   December 26, 2010, 12:13
Default
  #7
srr
New Member
 
srr
Join Date: Feb 2010
Posts: 25
Rep Power: 7
srr is on a distinguished road
Thank you very much Simon for your advice, when I checked the mesh I put the problem in a subset and then I cleared it.
In Fluent the mesh check was ok and I ran a simple simulation (without energy and viscous models) for 50 iteration just to check what happened and it worked perfectly.

Thank you again.
srr 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
ICEM 2D tetra mesh question kawamatt2 ANSYS Meshing & Geometry 18 March 3, 2014 11:56
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
problem when converting mesh (made by ICEM) using fluentMeshToFoam Forrest_Lei OpenFOAM 11 October 16, 2009 06:28
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 02:10.