Dear all,

we are currently looking with CFX 5 (5.4.1 & 5.5) to our turbulence modelling in high speed compressible internal flows with swirls. We use standard k-eps , RNG k-eps and Reynold stress models. We noticed that by default CFX 5 always uses a first order upwind schema to solve the eddy dissipation and turb. kinetic energy. Setting these to second order resulted in more dissipation (we use a full tet mesh with an inflation layer of prisms, y+ values are within the range 30-300). setting eddy dissipation to second order does not work (highly unstable code). setting turbulent kinetic energy, k, to second order gave different results (more dissipation in swirl and boundary layer). We are currently looking for benchmarks of turbulence models using CFX 5 with high speed internal flows (Re > 10E8). Any body who can help us? Did anybody use CFX 5 to simulate the DLR F4 wing/body drag prediction case (can be found at http://www.aiaa.org/tc/apa/dragpredw...d_Results.html)?

Regards,

Bart

There are several different turbulence validation cases for CFX-5 available directly from CFX. Are none of these applicable, or were you looking for some independently obtained results?

Neale.

First order discretisation of the advection terms in the turbulence equation should be adequate. By default the diffusion terms are second-order. It is far more important to use high order accuracy for the mass and momentum equations than it is for the turbulence equations (the turbulence equations are physically much more diffusive).

I agree that mass and momentum have to be second order in the first place. We saw however a substantial difference when changing the order for the turb. kin. energy to second order. Second order for the eddy dissipation was not possible (result exploded, no convergence). With a second order schema for k the flow shows much more dissipation.

It doesn't suprise me that using second order epsilon blows. The source terms are quite non-linear and any small pertubations would likely make it blow. What exactly did you do? UDS+NAC with a specified blend factor (Beta=1) or UDS+NAC with High Resolution.

You would have needed to type the command language directly to try this out, well, at least in CFX-5.4.1 or CFX-5.5. So did you make a mistake when you entered it?

Is there a reason you want to run second order on k and epsilon anyways? There's no sound argument that this will actually help anything.

Neale.

I used UDS+NAC in CFX 5.4.1 (we are in the process of doing it for CFX 5.5). We want to test the turbulence models by setting up benchmark cases (incl experiments). For high Re flows (>1E8) we would need a very fine grid in the inflation layer. Keeping the y+ in th eproper range is one thing. Resolving the boundary layer is another. We thought you need two things: finer grid and/or higher order methods. For mass/momentum/energy this is obvious. But setting k to the high resolution schema makes a difference (considerable). If a finer grid has the same effect as a higher order scheme would have than applying a higher order scheme is cheaper(we already have 5 milj cells +)

If the boundary layer is important to the flow physics, then I think that you should have at least 4-5 nodes in the boundary layer wherever practical. A higher order advection scheme will not create information for you. You still need enough grid to resolve what is important.

Have you tried SST in CFX-5.5 yet? To get decent results it's almost a requirement to resolve the boundary layer. One other thing nice about SST though is you don't need to worry about y+ so much because it automatically integrates to the wall where necessary and uses the scalable wall functions otherwise.

BTW, did you look at Fluent's results on the drag prediction workshop? Pretty brutal. The drag bucket prediction was completely off and they couldn't even get a converged result, especially with the coupled solver.

Neale

Hi Neale,

You mention a drag prediction workshop. Is this on the web at all? If so, can you let us know the URL.

Regards, Glenn

We are about to start with the SST model in CFX. We might have a problem however because we are under the impression that the SST model can not deal with wall roughness (correct me if I'm wrong) which we really need. I had a look at the Fluent results of the drag prediction workshop. However at least they have some results. I'm trying to get CFX to perform the same benchmark. If it is ok you have a great marketing tool. If not you still have some development work to do.

DLR F4 benckmark case:

http://www.aiaa.org/tc/apa/dragpredw...d_Results.html

I have the IGES file if you're interested

Alright then, I see your dillemma with SST. There's always something. Although I've never been convinced that the wall roughness means much on anything other than flow through a pipe.

As far as that validation case is concerned I would agree with you completely if it were some academic code from a university, or a code from a government lab, as generally they are not accountable to anybody and can do what they want. We're talking about probably the biggest commercial CFD vendor. People pay a lot of money to them and expect the results to be correct.

Neale

Dear Neale,

Ofcourse I expect CFX to deliver a code which delivers correct results. However, turbulence being one of the last unsolved items in physics I would like to know how good the implementation is of current turbulence models in CFX. I think their first priority is making money, which could interfere with making a code which is the best available today. So instead of relying on a piece of paper provided by marketing stated that all is well on the modeling side, I would like to see benchmarks. By the way, a code developed by Universities is publicised and results can be verified. They are accountable to the scientific community, if the make publications in f.i. journal of fluid mechanics.

Bart

Dear all,

I can assure you that CFX is committed to implementing models correctly. All the details of the implementation are clearly outlined in the documentation. Furthermore, CFX has and continues to publish in Engineering journals.

Some of the discussion here surrounds the implementation of the SST model. It just so happens that the inventor of the SST model, Dr. Florian Menter, works for CFX at the office in Otterfing Germany.

Turbulence modelling remains one of the hottest areas of research in CFD. Universities have the flexibility to try many new ideas, because they do not have to implement, or even develop a generally applicable model. Eventually these models make their way into the commercial arena, after their effectiveness is proven. That said, CFX continues to research and provide cutting edge solutions. In general, however, we must remember that turbulence models are just that, a model, and therefore there are simulation where the assumptions break down and the model will not apply.

Reading back in this thread, there is concern about the sensitivity of the turbulence model to 2nd order discretization. Since the turbulence terms are much more sensitive to sources than advection, the discrepancy is likely due to poor resolution with the mesh, not the model. The momentum terms will suffer due to the bad mesh long before the turbulence terms, and thus generate more error. Of course it is difficult to say for sure without seeing the problem. My advice is to further refine the grid, don't worry about the order of the scheme.

Lastly, if you are really interested in papers published by or about CFX, you should check out the community pages at: www.software.aeat.com/cfxcommunity. Every CFX user can access this information.

Best regards, Robin

Hi Robin,

I'm glad that we can keep the CFX developers sharp. You should not be offended. We just want to be assured that the models we apply in our design process are the best around. There is always the change that we do not have suffiecient knowledge of CFD. That's our responsibility. Next to that, we (CFD department of my company) want to have this warm feeling that we have a fighting change of comparing our CFD results with experiments. Validating the CFD models is and will be a large part of our work and I'm sure CFX is doing their best of providing good software. But I hope you do understand that we do not rely on the brochures automatically. Just keep on providing us with results of benchmarks.

Bart

Yes, results from codes developed at universities are generally published. But, the codes they use are not necessarily freely available. That leaves us in the situation where to verify results one must implement the algorithms themselves and verify it. Most of what is in CFX codes (CFX-5 & CFX-TASCflow) wrt. numerics was published by researchers at the University of Waterloo in the early to mid 1980s. Their turbulence and multiphase models are also all published in the literature, if you are willing to look for it. So, in that respect they are doing just as good a job as any academic institution. So, feel free to veryify their techniques for yourself.

My opinion of JFM has significantly dwindled in the last 2 years or so. The review process is long and drawn out, as well as not being very good. For example, I've seen a recent paper on detonation (last year) which is not original, and the exact same calculations had been done 5 years ago and published elsewhere. What the heck is that?

Benchmarks (validation, whatever) are available from CFX as well, maybe not for the exact same case that you are interested in, but they have some. These are far more than just a marketing brochure. I think that they will even give you the files so that you can reproduce the results yoursefl if you want.

Neale.

You're completely right. What's left for me is the following. The general idea (don't ask me why or who) is that commercial codes cannot be trusted. I think that flows in industrial applications are generally that complicated (turbulent, multiphase etc)that CFD in general has a roblem in givng accurate result. It requires normally just a engineering judgement on just how wrong they are. We do not have an alternative way of solving (we have to use a commercial code). We also have to convince people of our result. Lots of people are critical enough that they will not rely in our color plots because we say so. So a large part of our work is showing just how good these results are. Do not get me wrong, I'm very satisfied with CFX.

Yes, I think that the one must take a CFD code for what it is, commerical or otherwise. It's simply a tool and it's up to the user to show that the results are really a good approximation to the initial boundary value problem you are attempting to solve.

I don't think that commercial software is as "black box" as many seem to believe either. There's no magic involved, they are using numerical techniques developed in the 70s and 80s. The main thing that CFD companies have to worry about is attempting to tweak the numerics so that they are as robust as possible without sacrificing accuracy and strict conservation. They have to market to such a general crowd that there is really no other way. This does not mean that you can't get a good answer with a commercial package, it's just that you might have to spend a bit of time to get what you want, which would be the same if you were developing your own software.

I'm glad your happy with CFX, so am I.

Neale