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/)
-   -   Problem with tet-tet mesh merging (ICEM) (http://www.cfd-online.com/Forums/ansys-meshing/83001-problem-tet-tet-mesh-merging-icem.html)

srr December 10, 2010 17:37

Problem with tet-tet mesh merging (ICEM)
 
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

jeevankumarb December 13, 2010 07:09

what problem you are getting. is it multiple edges?

PSYMN December 13, 2010 13:28

Guidelines and rules
 
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.

srr December 22, 2010 23:26

2 Attachment(s)
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

PSYMN December 23, 2010 15:27

Single edge check...
 
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 December 23, 2010 15:31

Multiple....????
 
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...

srr December 26, 2010 12:13

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.


All times are GMT -4. The time now is 23:44.