My research project is about a cylinder head design and intake flow calculation. We already Designed the cylinder head with Catia but we are now investigating about the kind of meshing and method we must use and the errors we must expect on this kind of computing. We must use Fluent and probably GEOMESH. Do you have any experience of this kind of calculation? Do you know the errors between CFD and Experiment we should expect? thanks for your advices and answers.

Julien Plenchette

This is a highly complex problem,1).always transient, with moving piston, (2). compressible with open/closed system due to valve motion, (3).complex flow coupling in the inlet manifold, wave interaction. manifold inlet condition is unsteady.(4). geometry of the valve and the inlet can be highly complex for producing the desirable flow motion inside the cylinder. (5). depending upon the valve position and flow rate, separation pattern varies greatly. (6). flow separation can be sensitive to the sharp corner of the valve geometry ,thus making the turbulence modelling difficult. But the advantage of using the unstructured mesh is that for fixed valve position -flow through simulation(no piston), the mesh is probably easier to generate. It is possible to use structured mesh, but the topology is highly complex . And it is difficult to control. (7). I have seen published papers in this area ( simplified geometry), so, you may want to dig into the international journals to see the mesh density distributions used by other people ( most of them used structured mesh). (8). since the real problem is compressible, transient, reacting, turbulent flow with open/close and moving boundary, it going to take some times to address the "error" issue. So, the answer is, the unstructured mesh is definitely easier to generate in this case because of highly complex topology.

Japanese SAE did a big benchmark study on this problem about 1 year ago with cooperation of many CFD vendors (including Fluent). I have recently seen an english translation of this paper published in Europe (Titled: CFD Overview and Comparision of Commercial Codes - Benchmark CFD Study of Aerodynamics and Engine Cold Flow). To summarize there are several interesting observations:

(1) Different vendors used quite different mesh topologies (2) mesh resolution in and near valve seat area, and just below the valve location is crucial. (3) typical mesh cell count of ~500,000 hexes (or more) for good results; there is no substitute for lots of mesh resolution in these problems (4) good results require a mesh optimized for the specific problem (5) validation with some available test data is necessary; without this data for guidance your results may not correspond with reality; lab data helps provide insight for meshing strategy. (6) (my opinion) you should use RSM (turbulence model) to increase your confidence in the answer. K-e for this problem gets swirl results within 10% about 1/2 the time. For a 4-valve head I would not trust a result generated by ke. RSM is usually within 10% on swirl though there are pathological exceptions. (7) greatest difficulty in the result isgetting the correct strength of separation from the valve skirt on the side of the valve nearest the port's inlet runner.

Good luck and have fun.

Je suppose que vous êtes Français. Au sein de Numeca, qui est société active en CFD, nous avons déjà fait face à ce type de problème en utilisant notre code. Nous avons fait ce type de caculs pour l'industrie aéronautique et celle des compresseurs. Si vous me donnez plus de détails, nous pourrons peut être vous aider.

A bientôt

Rémy Tasse

You could have a look at an online article "Numerical simulation and experimental verification of DI diesel intake port designs" devoted to this under: http://www.cyclone.nl/ports/ports.htm (including experimental validification data)

Hope to have been of some help, Henk