Which type of mesh is better for fluid flow and why?
 

Hi,

I normally use block structured hexa mesh for CFD simulations in CFX. Now one can also use automated Tetra mesh for the same.
I have heard that structured hexa mesh is always better for fluid flow simulation.
Is it true? Is tetra mesh less accurate or harder to converge?

Thanks for your inputs..

I answered this exact question a few weeks ago.

In short (I could not be bothered typing the whole thing again):
* hex meshes use less memory
* hex meshes have less artificial dissipation
* hex meshes are far superior for surface tension applications

But things in favour of tet meshes are:
* The additional artificial dissipation from tet meshes has been reduced to a very small amount with the CFX numerics. They have done a good job in making tet meshes pretty much as good as hex meshes.
* If your geometry is complex then doing a quality hex mesh is difficult. A quality tet mesh is far superior than a poor quality hex mesh.

Thanks Glen for your quick reply and clear & precise explanation.
Can you point me to any literature references that can be cited if required to support the use of block structured hexa mesh?

One more thing. Going by the definitions, hexa mesh is structured and tetra mesh is unstructured. As you already explained, hexa mesh needs lesser memory and form that I can conclude that structured meshes take less time to converge due to being more memory efficient.
Then, after generating the block structured hexa mesh in ICEM, why do we convert it to unstructured mesh by right clicking on Pre-mesh?

Is this because of the way CFX solver is coded? Is it the same case for other popular solvers like Fluent and Star CD?

Are these solvers coded for unstructured mesh to be more general ? Doesn`t it make them less efficient as compared to a solver for structured mesh? A solver for structured mesh would be able to exploit the banded matrix structure for a structured mesh and thus will be far more efficient.

Any reasonable CFD textbook will explain why mesh quality is important. The stuff about CFX having similar levels of dissipation between hex and tet meshes is from a tech note issued by CFX - ask tech support for that.

A tet mesh is usually unstructured (but can be structured), and a hex mesh is usually structured (but can be unstructured). Does that clarify things?

A structured mesh is one in which cells are referenced by ijk coordinates. So the cell to the left is i-1, the cell above is j+1 and in front is k-1. An unstructured mesh is one where cells are referenced by a simple ID number, and to work out what its neighbors are you have to go through a neighbour-cell array.

CFX is an unstructured solver, so even if you give it a structured mesh it ignores it and treats it as unstructured.

Structured mesh solvers are faster as the simple grid topology makes referencing very simple. But they are limited in that the mesh must be structured.

Thanks Glen again for the explanation.

I think what you said fits well with another definition of structured mesh i.e. a structured mesh consists of family of lines where any line from one family does not intersect with another line from same family and intersects with a line from another family at only one point (from CFD book by Ferziger & Peric).

So if I understand correctly from your replies:
1. Its always better to use hex mesh provided a good quality hex mesh can be generated for a given geometry. Otherwise, a tetra mesh should be chosen.

2. If solver time and memory requirements allow, then one can also switch permanently to using tetra mesh as a) tetra mesh generation is automated and requires less user time for meshing and b) current solvers have improved numerics that reduce artificial diffusion in tetra mesh to almost the same level as hex mesh.


2. All modern CFD solvers like CFX, Fluent etc. are generalized solvers to handle structured/ unstructured meshes.