Hi All, I have been comparing the results from a CFX calculation of the flow around a tube with some data. I can not get satisfying results, It can be CFX (or me ) that is the problem, but the data I have is also not very good. Does anyone know any good simple testcase/testexample that I can acces online.

Thanks in advance Jan

It was the data that was the problem, I have now solved another case with perfect match. Jan

Jan,

what settings did you use (turbulence model etc)? Did you use CFX 5?

Cd and Cf coefficients are well documented as well as Strouhal numbers/frequencies. Or do you require detailed velocity data?

Astrid

I was using CFX4, now I am trying to solve it with CFX5 - hope I get the same result Jan

Dear Astrid, I was just trying to get the same Strouhal number, which I failed for the first case I was looking at, but now it works fine. Regards Jan

For research puposes, we also perform this kind of simulations. Therefore three questions:

1) What is the Re-number of your problem? 2) Which turbulence model do you use in CFX 4 and 5? 3) Does heat transfer play any role in your problem?

Astrid

Dear Astrid, Answer to you question. 1) Re = 100 2) Laminar in both codes 3) No I did predict the St # within 0.25% (in CFX4.4) so for this case I am satisfied.

The reson why I am doing this is that I have to investigate a real problem, where the flow is turbulent and with heat transfer to the pin. I just wanted to start easy and get a feeling of the problem. My largest problem is now to get used to CFX5 (((, I can not even get any transient flow in CFX5 for the same case at the moment. Odd there is only very few options in CFX5 for the transient flow (only the timestep nothing abouth the methode)

We have performed simulations at a wide range of Re-numbers. Our experience is that you require quite a lot of timesteps to obtain the required oscillations. Just give CFX 5 a bit more time....... )))

Astrid

In CFX4 the oscillations started after 40sek and became periodic. I have now done the same simulation in CFX5 and I have calculated to the time 120sek and nothing is happening (. I do think that should be sufficient, I am looking into if I have missed something. Would you share your experience with CFX5 on this type of problem Astrid?

-How important is the number of iterations in each timestep, and what is sufficient. What should the convergence level be? Any difference in single or double precision? -For turbulent problems, any good hints, is the scalable wall model the best? -Is the any problems when heat transfer is involved? Regards Jan

Jan,

Are you running second order transient? You can't turn this on from the GUI. You have to do it manually in the solver CCL file. Extract it using cfx5cmds, add the following to the SOLVER CONTROL singleton:

TRANSIENT SCHEME: Option = Second Order Backward Euler END

The numerics in CFX-4/5 completely differ so you might need to perturb the flow a bit at the beginning in CFX-5 to get the vortex shedding going. Try a transient pulse on the inlet velocity at the beginning of the run.

I would suggest that you also ensure that you are running a small enough timestep in CFX-5 that guarantees that you get convergence to your target residuals within each timestep. If you don't make sure that this is happening then your results will likely be nonsense.

Hopefully this helps you out a bit.

Neale.

Jan,

Do you read your e-mail.....

Astrid