hello,

I am doing a project in which I have to simulate the vortex shedding behind a pipeline in 2D. my problem is that I try to see the vortex shedding but concerning the drag and lift coefficient and the Strouhal number my results are wrong. Indeed instead of having a Cd of 1 I only have 0.4 and for the Strouhal number I have 0.3 instead of 0.18. I would like to know if someone has already faced this problem and if someone can help me to resolve it. thank you

Dear Le Stanc,

I have the following suggestions.

1. Has your code "converged" in the sense that your lift or drag coeffcients show a periodic response with constant amplitude ?

If your code has not achieved a "convergence", as in the above sense your results also cannot be taken as correct. This seems to be a least possible scenario in your case.

2. What temporal scheme are you using ? Are your computations time accurate ?

Non time accurate computations can hamper solution accuracy and lead to an erroneous solution.

3. What is the grid resolution ? Is the grid sufficiently fine and have you performed any grid independent study ?

On a compartiviely coarse grid, your results could be qualitatively right, and vortex shedding can be seen, but the quantitative results would not. A higher spatial accuracy demands a more finer grid, leading you to the right solution. You can decide on the optimal fineness(roughly) by a Grid Independence Study.

4. Is this a validation test case or has the code been validated before ?

If you have not validated the code before, you can try valodating using the laminar vortex shedding past circular cylinder of unit dia. at Re=100 and check out the results. If the validation fails on a fine grid with a time accurate scheme there is a bug in your code. Please take care that spatial and temporal resolution are equally important in an unsteady flow problem. Therfore, equal importance needs to be paid to the accuarcy of a temporal scheme as to the grid resolution. Most probable in your case is that you are running in non-time accurate mode on a relatively coarse mesh.

Hope this helps.

Happy debugging and Regards,

Ganesh

hello Ganesh

my code has well converged, the forces are periodic. I am using the k-epsilon turbulence model because the SST doesn't work (which is strange). my advection scheme is high resolution and the transient scheme is second order backward euler. I try different timesteps (smaller) but the results are always the same. concerning the mesh, I did a refinement near the wall but I don't know if it is sufficient, the first space is 0.004.

thank you for your answer

Regards

Dear LeStanc,

What is the y+ for your grid ? You may need to use a refined grid to meet the y+ criteria. You could also try out a different model such as Spalart-Allmaras, which is a popular one equation turbulence model for aerodynamic applications which works reasonably well for mild to moderate separation problems.

Hope this helps

Regards,

Ganesh

Dear Le Stanc, OK,maybe you should simulate other project simpler to validate your algorithms and codes;if it works,check your input data files and your Grids,etc.

Cheers,

F.B.Tian

my Y+ is 176 which is relatively good because compromised between 30 and 300.

This is just a wild guess ... Assuming you have a converged solution (which you suggest in one of your responses), I'm wondering whether your problem is one of non-dimensionalization! The trend suggests that it's possible that, for example, you're using the diameter for non-dimensionalization but your data uses the radius. Just a thought ...

Adrin