Hi

Has anyone tried to validate CFX 5.6 against log velocity profile (also turbulent kinetic energy, dissipation and eddy viscosity) using unstructured grid?

How much resolution was needed ?

There is a validation report on the community website for 5.5 - however, the grid is structured.

My second question is : Is it even possible to model the boundary lay without inflation (Prism's) ?

regards

Michael

Hi Michael,

There is a paper on the CFX Community site which discusses the difference between tet, hybrid (tet/prism) and hex meshes. They don't look at boundary layer stuff but rather some laminar flow things instead, but the princples are the same. In short, a hybrid mesh is about the same as a hex mesh biased towards the boundaries. A tet mesh biased toward the boundary in the same way is way behind, or alternatively needs orders of magnitude more elements to get the same accuracy.

So yes, it is possible to model boundary layer flow without inflation but you are going to need many times more cells than a hybrid mesh to get the same accuracy.

Glenn

Thank you Glenn

I will go hunting for that paper.

However, It rises a concern i my mind: If we need to uses different forms for structured grids in order to resolve fundamental fluid problems - then under which conditions can we trust the results achieved with unstructured grid ?

The Hybrid grids are a way to repair the faults in unstructured grid. But every time I use unstructed grid in the future, I will have a doubt that certain gradients in my flow domain are questionable.

BTW does anyone know if it is possible to setup automatic grid refinement in CAD2MESH/CFX 5.6 ? (This could ease my pain of using unstructure grid ;-) )

Regards Michael

When I'm saying grid refinement I mean the Mesh adaption facility I remember from 5.5.1

- And yes! I found it under my nose in PRE )

Regards Michael

Hi Michael,

There is no "fault" with an unstructured grid. In a properly set up simulation, as the grid gets finer all grid types will converge on the true solution. A pure tet grid which is fine enough will give an accurate answer.

As high gradients exist in the boundary layer of flows, you need a fine grid to resolve it. A hybrid or hex mesh allows you to have a fine grid across the boundary layer to resolve this high gradient, but a coarser mesh along the boundary layer where the gradients are usually much less. This means the hybrid and hex meshes are biased in the direction of the high gradients, and hence will give a more accurate answer for a given number of elements. Tet meshes cannot easily do this biasing, and so require far more elements to be able to resolve the gradients.

As to "then under which conditions can we trust the results", the answer is you must do a grid refinement study. The grid resolution required for an accurate simulation is dependant on what you are trying to do, and most importantly by how accurate you have to be. Run the same simulation on a number of mesh densities and determine for yourself how fine a mesh you need.

Regards, Glenn

Thank you Glenn - you have answered my questions.

However, I think I have not made my conserns clear in my previos mail - sorry for that.

I'm well avare of the grid sensitivity in general and how to examine it. What suprised me a bit was the huge amount of computational effort needed to resolve a simple channel flow.

A lot of effort has gone into developing unstructured grid in all the main commercial CFD packages. The benefits are better 3D modelling of complex geometries and the ability to refine the grid in local areas, where it is most needed.

I hope that structured grid will be an standard option in future releases of CFX 5.X. In a lot of the problems I work with, the structured approach could be more efficient than the unstructured. In ICEM 4 CFX, there is a hex grid generator - but so far as I can see this facility requires a seperate license.

Regards

Michael

An extra point here to be made. The reason hybrid or structured meshes are required near the boundary (walls) is because of the turbulence model being used. Accuracy is highly dependent on the Y+ at the nearest wall vertex (usually 30<y+<100 for standard models, y+ << 1 for low Re models).

With a tet mesh, you cannot control the element size at the wall and the Y+ values will be all over the place from wall element to wall element (tall tets next to short tets). An inflation layer gives a nice uniform layer of prism elements that can be controlled to within the tolerance of the turbulence model being used.

Everywhere else, tets should be just fine.

Jeff

The hex mesh generator in ICEM 4.CFX requires a separate license AND a patch install to the release CD before you'll be doing anything. I found that out because I think I was the first customer EVER to run it. It's Hexa but missing a few things here and there.