Learning Forum

[Dato]

Dear all,

I'm meshing a under-sea model whose domain extents is approximately 10 km x 6 km x 30 m on average. It's really a large scale fluid domain with irregular seabed and shoreline. Due to high aspect ratio of domain, the model is literally like a sheet. 

All structured mesh of hexahedron is considered. I have been working on repairing the negative element for quite a long time by checking determinant 2x2x2. I have applied Y-block and adjust the edge parameter (lower spacing near the irregular surface on the right side) to eliminate the negative element. And finally the top view of the blocks and the generated mesh are shown below. 

The total element is 1.4 million. The value of determinant 2x2x2 is good. However, the minimum orthogonality is below 8e-3 which is unacceptable, I think, for FLUENT. The mesh is used and a preliminary steady single phase inviscid flow has diverged with increasing continuity residual. 

The location of worse orthogonality element is near the irregular distorted surface on the right side as shown below. 

 

I thought that the divergence is mainly caused by the poor orthogonality of mesh and  tried several ways to improve the orthogonality but failed. I have try "smooth mesh globally" and "smooth hexahedral mesh-Orthogonal" function in Edit mesh panel to perform post processing of the mesh, the quality become even worse and negative element occurred. 

 

Are there any ways I can do to improve the orthogonality in ICEM?

Any suggestions would be greatly appreciated. 

 

Best regards

LEE

 

 

 

[Rob]

I suspect the issue is linked to the very flat (high aspect ratio) cells that you have scattered through the domain. Trying to create a block structured mesh here isn't necessarily the best solution, and you may find a pave mesh to be better. High aspect ratio can trigger the ortho skew, and if there's a very sudden jump in cell size at a block boundary you'll also have problems. 

[Dato]

Yes, most mesh with high ortho skew have high aspect ratio too in my case. I have tried improving the orthogonality and it finally has increased from 0.0081 to 0.0586 at the cost of cell counts increased by 64%. The convergency has slightly improved in inviscid single phase flow. But I think maybe it's not satisfying enough for an engineering problem that the the ratio of net mass flow rate of inlet and outlet is around 2.65%. 

I'm not exactly understand the meaning of the "pave mesh". Do you means a hybrid mesh strategy should be used? Using unstructured mesh near the shoreline region and finally append the structured and unstructured mesh file in Fluent? I haved thought about this solution. If so, ICEM and Fluent meshing are reqiured and interface may be applied, I think. I have tried using Fluent meshing but it seems that hexahedral mesh with extremely high aspect ratio (~1000) in the bulk domain is not realizable in order to reduce the cell counts as much as possible.  

 

Sincerely thanks for your helpful advice.

[Rob]

I'd not use ICEM CFD for anything other than turbo applications, even then I'd use Fluent Meshing or make a colleague do it. For river/tidal flows I'd use an unstructured mesh and sweep "down" if I needed a CFD level solution. For flooding type scenarios I'd talk to specialists, and not use CFD: I'd save that for smaller scale simulations around bridge piers and the like. 

[Dato]

Thanks. Maybe it's necessary to turn to technical consultant.