[kkpal]

hi everyone!
my question may be stupid, but it's hunting me for a long time.
I'm doing something simulations about flow around a cylinder. There are two cases.

Case 1:
D=0.01m;
U=0.15m/s;
Re =100;
Case 2:
D=1m;
U=0.0015m/s;
Re=100;

The two cases are similar in domain size and as can be seen Case 2 is 100 bigger than Case 1, and they have the same mesh fineness.

In Case 1, the situation is bigger velocity with smaller cylinder and in Case 2 smaller velocity with bigger cylinder. Nevertheless, it is anticipated that if the Re is the same, Cd and Cl, which are the drag and lift coefficients respectively, should be the same in the two cases.

But in my simulations, the result of Case 1 worked very well; however, Case 2 gave very bad results.

Why is this happening? should i refine the mesh in Case 2 so that the smallest grid size is as fine as the Case 1？

[Far]

Are you assuming it steady or unsteady? It is definitely unsteady and in both situations you have to select different time step size due to difference in vortex shedding frequency.

What are the values of density and viscosity?

[kkpal]

Originally Posted by Far

Are you assuming it steady or unsteady? It is definitely unsteady and in both situations you have to select different time step size due to difference in vortex shedding frequency.

What are the values of density and viscosity?

Hi Far!
I chose laminar as the RASmodel in OpenFOAM, so I think for both cases it should be unsteady.
The timestep of both cases is small enough to keep the Courant number<1, and my nu is 1.5e-5 and rho 1.2, which is associated with air.
About the vortex shedding frequency, in my two cases they are not the same, how could I adjust my time step in order to get the same Cd and Cl?
I'm now very confused about the similarities in Re and St. For the two cases, if I keep Re the same, St will be different and vise verse. How could I choose the D and U if I want to simulate a bridge cable with certain diameter and flow velocity around it in the real world?

[Far]

Strouhal_number is ratio frequency * dia / velocity .

In first case ratio of D/U is 0.0666 and in second case ratio is 666.6 and if we assume St no 0.2 you will notice that frequency is 3.003 in one case and 0.0003 in second case. total time is 0.33 sec and 333 seconds and if we want to resolve them in 50 times steps then each time step would be 0.0066s and 6.66 s respectively.

PS: Assuming that Reynolds number is same then you should get same Cd (time averaged)

[kkpal]

Originally Posted by Far

Strouhal_number is ratio frequency * dia / velocity .

In first case ratio of D/U is 0.0666 and in second case ratio is 666.6 and if we assume St no 0.2 you will notice that frequency is 3.003 in one case and 0.0003 in second case. total time is 0.33 sec and 333 seconds and if we want to resolve them in 50 times steps then each time step would be 0.0066s and 6.66 s respectively.

PS: Assuming that Reynolds number is same then you should get same Cd (time averaged)

Dear Sijal
Thank you very much for your detailed reply, now I get a better understanding of the St number, may be i need to run the second case for enough long time to get the vortex shedding. In fact I think the proportion of U and D in case 2 is not appropriate because one period takes 3333s.

On a related subject, if i insisted in doing case 2, and I ran the simulation for enough time, do you think it is necessary to refine the mesh in case 2. I'm thinking that with 100 times bigger in the domain size, the smallest grid size also is 100 times bigger, will it affect the simulation result?

[Far]

On a related subject, if i insisted in doing case 2, and I ran the simulation for enough time, do you think it is necessary to refine the mesh in case 2. I'm thinking that with 100 times bigger in the domain size, the smallest grid size also is 100 times bigger, will it affect the simulation result?

I dont think so. Lets try and find out what happens in both cases and let us know as well.

[kkpal]

Originally Posted by Far

I dont think so. Lets try and find out what happens in both cases and let us know as well.

ok, I will do a similar case with D=0.03m and U=0.05m/s for which the frequency is about 3.3s. The original second case takes too much time.
I will post the result to here once I finish the simulation.
Thank you again, Sijal. You have been very helpful!

[m.vegad]

In fact i too had the same question troubling me since long...

i mean in case of larger domain the size of control volume next to solid region would be RELATIVELY large.... so truncation error wont be the same as in case of smaller domain (to the best of my understanding)...

If one checks the grid in FLUENT.. then for the larger size domain the mim and max area and volume reported are significantly higher than the smaller domain..

So would a mesh for smaller domain give mesh independent sol for a larger domain too!!! ( Reynolds no is the same in both cases)

[kkpal]

dear all,
here I put up the result of my test.

COMMON CHARACTERISTICS:
Domain size: (15R+40R)*30R
Mesh information: 32010 vertices, 50732 elements
Turbulence model: laminar

CASE 1:
R=0.005m, U=0.15m/s, Re=100, f=St*U/D=3, T=0.33s
Timestep=0.0001s

the drag coefficient Cd is about 1.5 and the lift coefficient Cl 0.35

CASE 2:
R=0.015m, U=0.05m/s, Re=100, f=0.33, T=3s
Timestep 0.001s
Obviously CASE 2 is 3 times larger than CASE 1 in domain size.

Cd is also 1.5 and Cl 0.35.

It is clear that these two cases gave the same result in terms of Cd and Cl. But the confusion is still there. The size of the smallest grid, as m.vegad put it, why is it not affecting the final result?