External 2D Flow - Reynolds Number Effects
 

Hello Everybody,

I'm trying to model a 2D laminar flow over a cylinder via Fluent. I got two different result and vortex street behind the cylinder both in Re=4500. cylinder diameter is 2 and viscosity is 1 in both two run. In first run velocity is 5 and density is 450 but in second run velocity is 30 and density is 75. The lift coefficient graphs of both are shown in the picture. (Black graph belongs to velocity of 5).

Shouldn't the flow pattern be determined only by Reynolds Number? Why they are different?

Thank you all

Are you using the same mesh & time steps in both cases? A mesh independent result should be the same, however if your problem is not independent in one or both cases that could cause a deviation. The graph for the U = 30 case appears more to have more frequency components then I would expect; suggesting a dispersion error.

the two solutions show different physics ... therefore in your setting the Re number is not the same.
Do you set molecular or kinematic viscosity?

Thank you for your reply. I used the same mesh and time step for both of them and both solution converged . You are right about the frequency in U=30 case. there are two main frequencies. 1.97 Hz and 2.42 Hz (Obtained by FFT of lift coefficient). The Strouhal number for 2D cylinder is reported 0.18 in references. the greater frequency has the Strouhal number of 0.164 and is close to reality. So you say that both case with same Re number must have same pattern and definitely there is a problem in modeling? and convergence in modeling does not guaranty the accuracy of results?

Dear filippo, actually the only difference in two runs is the Reynolds number. B/C I just changed the velocity and density and all other things are same. In defining material properties I set Dynamic Viscosity (N.s/m2) equal to 1 in both case and I changed density and velocity for each case . I'm not sure if the modeling is wrong or the real physics of two models are different b/c for sure the frequency of vortex shedding in case with higher velocity is greater but the Strouhal number must remain constant

Converence of the residuals does not guarantee that the solution accurately reflects the flow, merely that a solution to the discrete equations has been obtained. It's important to remember that the solution is an approximation to the flow, and it will depend on a lot of factors, the mesh and the time step being two of them. In general as the mesh and time step are refined the solution will become a better approximation, and there will be a point where further refining the mesh and timestep don't change the solution. I strongly suspect that the mesh and timestep produced a decent approximation in the first case but not in the second. The dependence on mesh size and time step is generally most visible in the spectral domain. Dispersion errors are errors that introduce additional frequency components due to the mesh/time step; this looks like exactly what is happening in your simulation. You can test this easily by re-running the simulation on a finer mesh with a smaller time step. Continue this process until the results don't change, then compare your cases.

It is possible that there are other issues, but this is the one that seems most likely to me.

Desmond,

1-In my knowledge only Reynolds number affects the flow. If there are heat transfer issues, then other dimensionless group are also involved like Prandtl (Pr) and Peclet (Pe) that are not usable here.

2-Yes I think so... do you have any other idea?

Thanks

the flow model is incompressible or you are solving the compressible form?
for the incompressible case the two solutions must be coincident

Most likely there are problems with mesh size and time step. I'm gonna try with more accurate modeling. Thank you by the way. your comments are really helpful

That is not how it works. Since you changed the velocity, the frequency of the vortex shedding will be different.
Remember: the Strouhal number has the same order of magnitude over a wide range of Reynolds numbers.
So the temporal discretization is different for both cases. See this thread fore some examples on the topic.

What is even worse is that you are simulating a turbulent flow. Re=4500 is in the turbulent regime for the flow past a cylinder.
So what you are doing is basically an under-resolved DNS. Doing so with different normalized time step sizes will trigger different results.

It is incompressible model. I am trying to change the grid and using finer time step and see if result change

Thanks. I almost understand where I made a mistake... I should change the time step and grid size. I was not sure if the differences between two models are physically reasonable.

the key is that the non-dimensional momentum equation write as

dv/dt + Div (vv) + grad p = (1/Re) Div Grad v

in which is assumed St =1 and Re is the only non-dimensional number that governs the flow.

If you solve the dimensional form you should satisfy the same constraint St=1. If you ensure such value, the solutions must be coincident.