When using CFD to perform film-cooling simulations, is it necessary to place a grid everywhere (including the film-hole and plenum) or can I put an exit profile at the film-hole exit.

Thanks

I've seen several papers where they have shown that the internal part of the hole and the plenum plays an important role and that you have to include it in the simulation. However, this is most often too expensive, I guess it depends on what kind of accuracy you want.

I had a colleague at Chalmers who worked on a new more economical way of handling this type of problems by introducing source terms in the equations instead of resolving individual holes. Let me know if you're interested and I'll give you his email address.

(1). That is one way you can do, but you don't know whether the condition you selected is the right choice. And then, you also have to worry about the pressure boundary condition. (2). So, other than the large memory required, it is the right way to specify the boundary conditions on the back side of the hole. (if you are talking about the jet mixing in a combustor, then it is a different story.)

Huhh?

(1). Yes, it is important to create a mesh to cover the flow field, the film holes and plenum. (2). The boundary condition in the plenum would be easier to handle and it should produce more accurate flow field solutions.

As Jonas pointed out there are several papers that talk about the effect of including holes in the simulations. It is also very true that grid size becomes huge for any real problem. I looked at film-cooling for my Master's thesis at the University of Texas. Other researchers at Clemson were also doing very similar work with similar success. My thoughts on the problem are that besides the need to model the hole and the plenum, an even more important effect is turbulence model.

Recently I have looked at some other options that my company's CFD-ACE+ code provides. One of the most attractive is the use of arbitrary interfaces with a fully conservative formulation. This helps in reducing the problem by an order of magnitude (compared to all tets, which is not a good choice), and by atleast a factor a two compared to block structured (which may be very difficult to use in complex geometries). I have not done any detailed study yet, but if someone is interested, please drop me an email and I can elaborate on the approach.

Okay Thanks

Thanks, I will keep that in mind

Thanks, I will keep that in mind

Let me add a few comments to that... I had yet another colleague at Chalmers who looked in detail on the effect of turbulence modeling on this kind of film-cooling simulations (resolving the holes very well). He tried many different turbulence models, including various Reynolds stress models and various two-equation eddy-viscosity models. I think that the conclusion was that turbulence models are important and that going to more advanced differential Reynolds stress models does not necessarily give any significant improvements - he had similar results with a simple k-omega model. There is a PhD thesis about this and several papers published by Stefan Jansson, Chalmers University of Technology. I haven't got his current email address but his supervisor, Professor Lars Davidsson (lada@tfd.chalmers.se) surely has more info.

I have also seen some papers (don't remember the references), where the choice of various turbulence models did not affect the solution significantly.

However, there are important issues related to modeling turbulence. First the nature of the flow is highly anisotropic near the injection from the whole. Use of any model that treats turbulence quantities as scalars (scalar K, scalar epsilon), in my opinion, means admitting a known limitation. Another imporant issue is how well the boudary layers are resolved. Use of k-epsilon model with wall functions (what I used, and what many others use) means the boudary layer is not resolved. Velocities very near the wall would not be correct. I don't know which of the two effects is more important though, and would like to investigate some time. Or may be others have alreay looked at it.

(1). I think in terms of the general jet trajectory, it doesn't require any high level modeling. (2). On the other hand, the jet will cause the boundary layer ahead of it to separate as if it is a solid cylinder. (3). The region behind the jet is a wake next to the wall. It is a separation bubble also. (4). So, by sommon sense, one needs to use a low Reynolds number model ( or the like) to resolve these areas. With the use of wall function, it can not capture these features accurately. (5). Then there will be a horse shoe vortex associated with the downstream jet, a secondary flow feature. (6). So, if the wall layer behavior is important, as is the case for the film cooling, then turbulence models at the low Reynolds number level are rewuired. (7). The other important factor is the mesh itself. It is important to cover the boundary layer, the jet region (which is bending and spreading as it moves downstream). (8). If one uses a commercial code to solve a jet-in-a-cross-flow problem. The RAM memory required is rather large just for a single jet. I have studied this type of problem since early 70's. I think, it is a good 3-D benchmark test case. Because of its wide range of applications, it will remain a very active problem.