[random_ran]

Hi CFDers:

I am doing simulation of flow over a cylinder. Reynolds number is 100 in my case. Following is the descrition of my simulation:

a. computation domain
diameter of cylinder: d = 0.0889 m.
2016-09-04_140735.jpg


b. mesh detail: (Grid 1)
Over sizing: Max face size 0.015m
First layer thickness 2.2225e-3 m
Inflation layer around cylinder: 40
Growth rate: 2.5

b'. mesh detail: (Grid 2)
First layer thickness: 0.001 m (Grid 1 is 0.002 m)
number of inflation layers: 80 (Grid 1 is 40)
Over sizing of max face size: 0.075 m (Grid 1 is 0.015 m)
Mesh.jpg


c. solver : pressure base, transient
d. material: air density 1.225 kg/m3, viscosity 1.7894 kg/m-s
e. model: laminar
f. boundary condition:
cylinder: no slip
wall: specified shear(X-Component 0, Y-Component 0)
inlet: velocity 0.01643 m/s
g. reference value
Area: 0.0889 m2
h. solution method:
Pressure-velocity coupling: SIMPLE scheme
Spatial Discretization:
Gradient: least squares cell based
Pressure: Second order
Momentum: Second order Upwind
Transient Formulation
Second order Implicit
i. solution Initialization: Hyper Initialization


Result:
0.05.jpg


Following is the summary of my result:
Capture1.JPG
Capture2.JPG


My question is why strouhal number decreases as I decrease time step and why drag is bigger than experimental data?

Can someone gives me some suggestions what I can do to improve my simulation?

Thank you,

Ran

[mome]

Interesting, I don't really know tbh. My only thought was that you have too high CD and too low St, so maybe overly dissipative numerical viscosity causes that, hence it could be a mesh-thing and give feedback on time-step sensitivity.. But then again, your CD vaule doesn't change from grid1 to grid2, neither does the separation point, and your schemes are 2nd order... Sorry that I can't help really just thought it may give you ideas if I comment anyway. would like to know the solution, good luck

[random_ran]

Hi mome:

Thanks for your reply. My intuition is the mesh. I will definitely try to use some other types of mesh to compare the result.

I have also try time step 0.001s and Fluent gave me useless result (Cd=10+), my convergence criteria is 10e-3. Is this a potential problem?

Ran

[random_ran]

Originally Posted by mome

Interesting, I don't really know tbh. My only thought was that you have too high CD and too low St, so maybe overly dissipative numerical viscosity causes that, hence it could be a mesh-thing and give feedback on time-step sensitivity.. But then again, your CD vaule doesn't change from grid1 to grid2, neither does the separation point, and your schemes are 2nd order... Sorry that I can't help really just thought it may give you ideas if I comment anyway. would like to know the solution, good luck

Problem solved!

I changed residual to 10-6, then shedding frequency mathces with literatural very well. It showed that this number is extremely sensitivity to residual.

[LuckyTran]

Originally Posted by random_ran

Problem solved!

I changed residual to 10-6, then shedding frequency mathces with literatural very well. It showed that this number is extremely sensitivity to residual.

This is just my rant but this is why you should not rely on residuals, because residuals are not convergence monitors. You need to be monitoring solution values to establish whether you have achieved inter-timestep convergence. It is a big problem and many editorials have been written on it. Patrick Roache devoted a section in his book to bash residuals. Too many people have been fooled into thinking their simulation has converged by setting convergence monitors based on residuals that are too lax. More strict residual criteria certainly does help (because it generally results in more iterations per time-step) but that is not an excuse to not check to make sure your solution is correct! The onus of proof is on the author.