hello,

I am doing a project using CFD/CFX in which I have to simulate the vortex shedding behind a pipeline in 2D. My problem is that I see the vortex shedding but the drag coefficent and the Stouhal number are far from the results I should have. Cd is about 0.4 instead of 1 and St is 0.3 instead of 0.18. I would like to know if someone has already faced this problem and if someone could help me to resolve it.

thank you in advance

Have you chosen a suitable turbulence model? If you have a basic model this might be your problem. Also timestep and grid resolution could be affecting your results. JOn

hello Jon

my turbulence model is the k-epsilon model because with the SST model it doesn't work and I tried different timestep but the results are always the same. concerning the grid I don' t know if my refinement is enough or not. how can I know that?

Thanks

Couple of things to try. Make your grid smaller and see if affects your results, simple!! And about the SST your Y+ value is critical. Check that in post by plotting it on your pipeline surfaces. If you have not significantly refined your surfaces then it will be too high without doubt. You need a Y+ of approx 2. So you will probably have to remesh and refine your cells adjacent to your pipeline before the SST will run.

What is your Re? Depending on the answer you might have to do a 3-D simulation.

-- Jarmo

my Re is 10e5. I tried another calculation with Re=100 and the results are better so maybe I have to change my turbulence model but I don't know which to take because I was using the k-epsilon and the SST model doesn't work. I'm using CFD.

Thanks

Le Stanc

Re = 100 should be doable without turbulence model.

Unfortunately I don't have the experience with either SST or k-e for such high Re. Best suggestion is still to refine the mesh, maybe use quads near the surface?

Jarmo

hello

I tried a calculation with Re=100 and the results are good. I tried something else with Re=6000 and in this case the results were wrong another time. I'm now wondering about the turbulence model and his options. I chose the intensity and length scale option with a fractional intensity of 0.05 and a eddy length scale of 0.1m. I don't know how to choose the better option and his parameter.I hope you could maybe help me on this point.

Thanks a lot for your help

I do remember asking a similar question here a few years ago, and was pointed towards an article on spanwise variation on the drag... I can't remember any details on this (other than the fact that a 3-D simulation is needed) and do not have access to the paper, but you might want to do a search on the main forum for "flow past a cylinder" and see what comes up. Re = 100 does not require turbulence modeling, just sufficiently small time-step to get St right.

I'd also look up some NASA Technical report on turbulence models, I think author is Bardina. Should give a good idea which model / parameters to use.

I hope this helps

Jarmo

What exactly do you mean by sst does not work?

SST is a blended model (k-epsilon in the free stream, k-omega near the wall). If the mesh is too coarse then it is basically k-epsilon because the solver cannot integrate to the wall then.

For Re of 10^5 you might need to be running SAS-SST or DES actually.

I do not know what exactly he meant by sst does not work, but due to my last few days of experience, I probably know what he means.

Backgraound: I implemented the sst -kw model in the solver code I have (self written). To write this, I went through the description given in CFX manuals and in Fluent manuals. They are the same (they should be). Well I implemented and was validating my code against Fluent. (My implementation was same as CFX), to my surprise my results were different from Fluent. first I thought I implemented it wrong, but then I decided to do the same case with CFX (for some time we can use CFX also), and I found out that my results were same as CFX (but were different than Fluent).

So what was wrong (assuming both CFX and Fluent are correct). After lot of analysis, I could figure out that the production of wall in Fluent case is fixed (by some formula) and for CFX case it is not fixed.

Note : this only effects if yplus is higher , for yplus around 1 , not fixing shall give the same results because we are resolving flow well)

So i also fixed the wall production of k (as described by perics book), I got similar results to Fluent (this is why I can say wall production was fixed in Fluents case).

So in his case if he is using sst kw and if the yplus is not good, using CFX he might get meaningless results (different from k-e)

As far as not fixing the wall values of production are concerned (for CFX), my guess is if they fix it, it might screw the transition models (for which production shall be calculated based on flow conditions).

As far as wall omega is concerned, both CFX and Fluent seems to be using same formulas, as I was able to get them similar by following what CFX manuals says.

" I could figure out that the production of wall in Fluent case is fixed (by some formula) and for CFX case it is not fixed. "

sorry here read :

production of k in wall cells ...

finally I did another mesh very close to the wall with a lot of elements and in this case the SST model works. But the results are always the same, 0,7 for the drag coefficient instead of 1 compared with the experimental data.