[Bdew8556]

Hi guys,

Probably been over this heaps but just wanted a refresher.
Why is hex mesh deemed to produce more accurate results than a tex mesh?
Also to my knowledge TurboGrid produces a hex mesh in the impeller?

B

[aero_head]

There is plenty of information/discussion about this on the Internet. It's true you must be cautious with everything you read and confirm it yourself, however answers can give good starting points.

Tetrahedral elements can fit better complex geometry. However, when you integrate the shape functions with points of Gauss it is less accurate than hexahedral elements. In addition, one of the factors that determines the quality of your mesh is the distortion of your elements. The reason for this lays on the mapping from real to natural space of integration. To sum up, if your geometry is simple, the best option is to mesh it with hexahedral elements. If it is not possible (curved geometries, acute angles or similar) then go with tetrahedral but controlling the distortion of the elements.

Hexahedra meshes are also more economic with the number of elements because the same degrees of freedom (or for 8 nodes) for one hexahedron corresponds to six tetrahedra. It is obvious that increasing the number of elements will not increase the size of the global finite element matrices but the computations for one hexahedron are generated also for six tetrahedra. This step has to be compared in cpu time in order to state if it is interesting to use hexahedra than constant strain tetrahedra knowing that curved or linear hexahedra use Gauss integration points to generate the element characteristics (stiffness, mass, etc..) and tetrahedra use exact formula without any integration to get the same characteristics. Researchers have always used tetrahedra elements because they fit very well arbitrary shaped geometries with their simple computations.

In sum, it's a misconception that hexahedral elements are always better than tetrahedral.
Most old textbooks will tell you hexa (quad) mesh is better than tetra (tri) and show you how large the numerical errors may be introduced by tetra (tri) mesh. Sometimes, this is true, especially 15 or 20 years ago.

Historically, people prefer hex mesh due to: 1). At that time, only structured mesh can be used for most CFD solvers; 2). Less cell (element) count (so, a lot of saving in RAM and CPU time); 3). Unstructured solver was not matured.

The solver technology developments in most commercial FEA and CFD codes in the last decade have led to the similar results for hex and tetra mesh for most problems. Of course, tetra mesh usually needs more computing resources during solving stage. But his can be easily offset by the time saved in mesh generation. The accuracy advantage of hex mesh no longer exists anymore, for most engineering problems.

For some particular applications, e.g., wind turbine, pump, or aeroplane, hex mesh is still preferred, because of 1). Industry convention; 2). Well-understood physics (most users know how to align the mesh); 3). Special tools to generated hex mesh for such geometries.

However, for most FEA and CFD users, if the geometry is slightly complicated, it is just a waste to spend time on hex meshing. Your results will not be better, most of the time, if not always. The (solver) computing time saved with hex mesh is marginal compared with time wasted in mesh generation.

And yes, Ansys TurboGrid can automatically produce hexahedral meshes for all bladed components, i.e. the impeller

[Bdew8556]

Thanks very much for the response, very informative.
I wonder if you could maybe elaborate on this part:

"However, when you integrate the shape functions with points of Gauss it is less accurate than hexahedral elements."

B

[piu58]

Tetra meshes tend to be more diffusive than hex meshes.

You need a balance between meshing effort, stability and accuracy.

[Bdew8556]

Very interesting....

Why is that?

[aero_head]

Originally Posted by Bdew8556

Thanks very much for the response, very informative.
I wonder if you could maybe elaborate on this part:

"However, when you integrate the shape functions with points of Gauss it is less accurate than hexahedral elements."

B

An 8-node solid brick element, C3D8 has 2x2x2 integration scheme, meaning there are 2 Gaussian integration points along each direction. So, you need 8 integration points for full Gaussian integration. The picture added shows the integration points for a hexahedral brick element, C3D8.
Both the C3D8R and C3D8 have the same shape function. When we say fully integrated, it means that the integration points cover all the directions.
C3D8R is less accurate compared to C3D8 for larger element size. You need a considerable mesh refinement to get an accurate result for C3D8R as the accurate value is obtained at the center of the element, that is, at the point of integration.

As I stated, the full integration for a 8-node solid brick element is a 8-point scheme. But for incompressible or nearly incompressible behaviors (as for von Mises elastoplasticity), locking phenomena can appear when using such elements. These locking phenomena appear when the displacement approximation is not sufficiently rich to satisfy both the momentum balance and the incompressibility equation. To avoid this problem, one way is to use reduced or selective integration techniques.
For the reduced integration technique, the incompressibility condition and the momentum balance are computed by means of only one integration point but this leads to the possible non unicity of the solution in static analyses or to the well-known hourglass phenomena for time dependent problems. Despite of this difficulty, this approach is very efficient for explicit dynamic simulations because calculation time is directly linked to the number of integration points. But in this case, hourglass modes must be controlled.
The selective integration technique consists in using the 8 integration points but with a volume change constant over the element. The volume change can therefore be calculated either at only one integration point (in fact at the element center) or as the mean value of the volume change over the element (B-bar method).

[Simbelmynë]

Originally Posted by Bdew8556

Very interesting....

Why is that?

Numerical diffusion always occurs when the mesh is not aligned with the flow direction. Hex mesh can be aligned if the flow direction is known before the simulation. However, there is no way to align tet mesh. If you have a flow with no preferred direction, such as swirling flow, then it does not matter.



Also, if you use a least squares formulation for gradient calculations then hex cells can give more accurate results since each cell has six neighbors compared to four neighbors for tet cells. Polyhedral cells can be even better in this context.


At the end of the day I think well resolved boundary layers, correct models and a proper mesh sensitivity study is the key. You can get good results with any cell type, even though there may be differences in execution time and meshing time. There is no magic cell type if you model many different types of geometries and/or physics so someone stating that you should always use celltype XXX is wrong.

[arjun]

Originally Posted by Bdew8556

Very interesting....

Why is that?

Gradients are shape and neighbour cells dependent so the interpolation is shape and neighbours dependent dependent too. In case of Tetras you only have 4 neighbours as opposed to 6 of hexas.


Now if you extend the stencil for gradient computation, the tetras can produce as good as hexas in terms of results (as the main issue is then removed).