Hugh cell jump in Tetra mesh
 

Dear All,

i am doing tetra meshing of a full aircraft configration.
When i generate Tetra mesh from the surface mesh, there is a hugh cell jump in the the genetared terta mesh, as seen in the image. i used delaunay method for generating tetra mesh. The surface mesh is good and has no errors.

please can anyone tell me why this jump accurs in the terta mesh and what can be the solution to fix this problem.

Thank you in advance

Tetra Tumor
 

This is a "Tetra Tumor".

It sometimes happens with the Delaunay Tetra algorithm. I have found that adjustments to the surface mesh can prevent it (it is some how a result of what happens at the surface (mostly large size transition) mixing badly with the back ground grid and how the filling proceeds). I can't tell you precisely how to fix it, usually any change will help, but sometimes the change just moves the problem somewhere else, especially if it is still a large mesh with large surface gradients.

At the moment, the best "Fix" is using the TGlib option.

I would suggest just redoing the volume mesh, but this time turn on the TGlib option under the Global Mesh Setup for Delaunay...

Attachment 3597

In this case, I am using Delaunay with TGlib and the AF (Advancing Front) refinement function.

Thank you Simon Pereira

but i am using ansys 11 and 10 and i dont think so the tglib option is available in this version. but i will try out the other suggestion on volume mesh transition from the surface mesh.

is this has to do anythin with the memory scaling factor or the memory requirements in the windows os.

Thank you once again

Nope,

The memory scaling factor is because this chunk of code is fortran and does not support dynamic memory allocation. Instead, it looks at the number of surface elements and "reserves" memory based on a simple calculation. If it runs out, it doubles the memory and tries again. After 3 attempts, it fails and gives you a message.

Memory is cheap, so I usually just set this memory scaling factor to 3 or something like that so that the first attempt is less likely to fail and waste my time.

This defect has more to do with insertion errors while the algorithm is running.

At ANSYS 11.0, we had just bought Fluent (the April before that release) and had put in a rough hookup. If you turn on beta options you will find "TGRID" is one of the options. It is rough in that it doesn't accept density boxes or keep prisms and it may have some issues with high aspect ratio quads, but at least it won't have this problem.

Another option is to use the remesh subset option under "edit mesh (tab) => Repair Mesh => Remesh". You would first select your large elements for a subset, then "modify" that subset to add a few layers including volume elements. When the outside of the element subset looks like the right mesh size, go and "remesh" with tetra and use the "subset" selection tool. Sorry if it is not easy to understand what I mean...