Flow past cylinder (Re=10^5)
I am simulating incompressible unsteady flows past a cylinder with Star-CCM+.
The Reynolds number is around 10^5, assuming that diameter (D), density and viscosity are 1 (to make things simpler for me, as long as non-dimensional values are correct, it should not influence on the computation, I am wrong?) and upstream velocity U=10^5 m/s. The turbulence model is realizable k-epsilon, with standard values of turbulence intensity and turbulence length scale (various models and parameters have been tried, results are roughly the same).
The grid is a conventional 2D grid. The distance from the velocity inlet to the cylinder is 15*D, 25*D from the cylinder to the pressure outlet and 15*D from the cylinder to the sides, supposed to be symmetry boundaries. The mesh is structured with quad-cells.
The time-step size is 10^-6 s, because the Strouhal number (St) will be around 0.2, so the vortex shedding frequency will be around f=St*U/D=0.2*10^5/1=2*10^4 Hz so the period about 1/(2*10^4)=5*10^-5 s. I expect about 50 points per period of oscillation of the aerodynamic coefficients.
Given this time-step size and the refinement of my mesh, the maximum Courant number remains below 50.
The maximum wall Y+ is also maintained below 50.
The number of inner iterations is 10. It seems to be enough.
With the same geometry, laminar simulations give satisfactory results for lower Reynolds numbers.
The problem is the value of the drag coefficient, known to be around 1.2 at Re=10^5 according to many documents. No matter the changes in any parameter I have tried, my mean value of the coefficient is 0.255, which is much too far from the result I expect.
So my first questions are what could be the reasons of such a difference? Is it due to the grid? Should I enlarge the domain (Iíve given a try: it increases the coefficient, but not enough)? Which parts of the domain should I extend (distance from the velocity inlet to the cylinder, from the cylinder to the sides, etc)? What is the influence of the turbulence intensity and turbulence length scale that are specified in the inlet boundary?
I have tried to decrease the time-step size to 10^-7 s too, but the improvement is not that great: I get a mean drag coefficient of about 0.32. The vortex shedding frequency and the amplitude of the lift coefficient oscillation also vary. But the calculations take so much time, I canít reduce the time-step once more, it would last days, I canít afford it. My second set of questions is why does the drag coefficient vary with time-step size? How could I know my time-step is small enough? And what could I do to get more accurate results?
What else should I try?
Any help is welcome. If you need any further detail, let me know.
>> Mesh <<
>> Effect of a change in the time-step size on drag coefficient <<
>> Effect of a change in the time-step size on lift coefficient <<
I would actually like to ask you something about mesh generation. I am going to do similar things, but the cylinder would rotate somehow.
Do you or anyone have any suggestions on how to generate the mesh (2D or 3D) for this type of problem in Star-CCM+ and Star-CD (I am using at the moment)? Thank you.
check this site, though it is for a Laminar case
This is just a shot in the dark.
"Theory" gives 1.2 x 10^-4. You get 0.255x10^-4. The ratio is 4. Now the ratio of diameter^2/radius^2 = 4. (radius & diameter are for your cylinder).
Would it be worth checking to see that the theory and your results are on the same basis?
Hope this is some help - even if it just removes one potential problem.
I'm not sure I understand what you mean.
First, the expected result of the drag coefficient is 1.2, not 1.2x10^-4...
Then, for the calculation of the drag coefficient, I use the diameter as reference length, radius shouldn't be used. Anyway, I don't think the problem comes from the calculation of the coefficient, because laminar simulations give good results.
The basis of my results and the one of the expected results are the same as long as Reynolds numbers are the same. In my case, "drag coefficient [is] only dependent on the Reynolds number" (from "Boundary layer theory" by Hermann Schlichting, p. 9).
Here is an example of the document where you can check the expected result:
>> Evolution of Cd vs. Re, from "Boundary layer theory" by Hermann Schlichting, p. 19 (preview available on http://books.google.com/books?id=8YugVtom1y4C) <<
Good try, thank you.
Any other idea ?
The mesh needs to be remeshed. What is needed is a ring around the cylinder that has a dense distribution, these four walls have a lot to do with these wild oscillations in your results
Actually I have tried to add a boundary layer of small cells.
Perhaps not small enough... What should be the size of the first row?
I thought it was enough refined, as my max y+ is between 1 and 100 (about 30-50). If I put smaller cells, max y+ will be lower, how should I handle the wall treatment?
Thanks for the tip,
only I can ask you to review the hypersonic cylinder case on the validation server given before (there is a shot for the mesh used), you need a high density ring around the cylinder, simply said, remove these walls from your domain. the y+ values seem to be OK
flow around cylinder
From my experience, you will not get the correct results using a 2-D mesh. Flow around a cylinder is 3-D for Re>200.
For Re< 3 x 10⁵, the boundary layer is laminar, so you need to use a low-Re model. Probably the k-epsilon model that you are using is a high-Re one, so you are getting the drag values for turbulent boundary-layer.
The best option for your flow is to use the SST k-omega model, but without 3-D effects you are going to get high Cd values. Your Cd probably will be around 1.7.
Thank you very much, Fabio, for your advices.
This study is in fact a test case, a kind of preliminary work to the study of a much more complex geometry (a 3D vertical axis wind turbine). The Reynolds number will be about 5x10^5, but I know I can't get results for the flow over a cylinder at this critical point, so I first study Re=10^5. In reality, I guess flow will be fully turbulent over a wind turbine (To me, low-Re models doesn't seem to be appropriate, is it ?), perhaps I should run tests at Re=10^6 or 10^7 ?
My goal is to train and get necessary knowledge. But I feel a little worried, because it is so difficult to get accurate results on what I thought was a simple test case that I just can't guarantee usable results on a complex geometry. If I don't get good results for the flow past a cylinder, how could I get good results for another geometry ?
I'm still gonna work on the cylinder following your help, but does anyone have any advice on how I should work to study a wind turbine ? Am I going the right way (I mean: study the flow over a cylinder (fixed and rotating), be sure to get accurate coefficients, and then study the flow over a wind turbine) ?
By the way, can anyone give me reasons why drag coefficient is so influenced by the time-step size ?
If you have an answer for any of those questions, any help is welcome.
Thanks once again,
|All times are GMT -4. The time now is 19:10.|