[thedal]

Hi,

I have to do a flow over multiple square cylinders in tandem arrangement at Re 100 and get Cd Cl plots. But I find my results are wrong. I am getting zero Cl. Can anyone please tell me if the solver conditions I have given are right or not?

1. Models - Transient - 2D Laminar case
2. Material - air - density - 1 kgm-3 and viscosity 0.01 kgm-1s-2
3. Inlet - velocity inlet - u = 1ms-1
4. Outlet - pressure-outlet - Gauge pressure 0
5. Top and Bottom boundaries - Stationary Wall - Shear stress - 0
6. Cylinders of 1m side, 1.2 m apart and no-slip Boundary Condition.
7. upstream is at 7m from the cylinder and 32 m is downstream to the cylinder.
8. ANSYS Fluent Software.
9. Top and bottom distance is 21m
10. Transient formulation; Timestep size: 0.01; Number of Time steps: 15000
11. Number of Iterations per time step: 50 (max)
12. Initial condition: Inlet velocity U = 1 and V = 0;

I am getting Cl plots zero, PISO - Second order and vortices are standing at the rear end, and no vortex shedding, hence, cl is also zero.

I have posted the mesh and the result for four cylinders inline, However I am working on 2 to 10 inline square cylinders. I got the shedding for a single cylinder for the same boundary conditions, and solver. But, Multiple cylinders are not producing any lift.

Mesh:
https://www.dropbox.com/s/abthh5tjratnnxs/mesh.JPG?dl=0

Is the solution converged??
https://www.dropbox.com/s/c4l52tv7la...duals.JPG?dl=0

Vorticity Magnitude:
https://www.dropbox.com/s/u2s4alngwb...icity.JPG?dl=0

[flotus1]

8. CFD software: my guess is Ansys Fluent
9. distance of top and bottom boundary conditions or even better: a sketch
10. transient formulation:
11. time step size:
12. physical simulation time/number of time steps:
13. number of iterations per time step - is the solution converging:
14. initial condition:
15. image of the mesh used:

[FMDenaro]

We don't know the type of discretization, accuracy and grid you are using, maybe you have numerical viscosity that dumps the shedding. However, top and bottom walls confine the flow and can further dump the shedding

[thedal]

I have added as much as possible. I will put the mesh figure soon. Thanks for the reply :-)

[thedal]

Can you explain the concept of numerical viscosity dumping? If not, What else can be given? And Top and bottom are kept at 10timesD from cylinder, and Condition given there are, Shearstress is zero. Will it still confine the flow and effect in the vortex dumping? I will show the mesh and other contours soon.
Thank you for the reply :-)

[flotus1]

Originally Posted by thedal

Hi,
10. Transient formulation; Timestep size: 0.001; Number of Time steps: 15000

I rather meant if you are using a first oder or a second order transient formulation. I highly recommend second order.

So your total physical simulation time is 15s.
Lets estimate the frequency of the vortex shedding using Strouhal number for a single cylinder: ~0.2

So you only simulated 3 vortex shedding periods which is way too short to reach a statistically steady state.
Increase the time step size to roughly 0.05 T...0.01 T (with second order transient formulation) and run for a physical time of at least 50 vortex shedding periods.

[JBeilke]

And don't use PISO for a time accurate solution.

[FMDenaro]

Originally Posted by thedal

Can you explain the concept of numerical viscosity dumping? If not, What else can be given? And Top and bottom are kept at 10timesD from cylinder, and Condition given there are, Shearstress is zero. Will it still confine the flow and effect in the vortex dumping? I will show the mesh and other contours soon.
Thank you for the reply :-)

Numerical viscosity means that the local truncation error of the scheme introduce a spurious term that is in the form of the diffusion of the variable, but with a coefficient that is not physical but depends on the time and mesh size. That is typical of upwind schemes.
I suggest to plot the total kinetic energy versus the time to have a control of the flow evolution.

[thedal]

Originally Posted by flotus1

I rather meant if you are using a first oder or a second order transient formulation. I highly recommend second order.

So your total physical simulation time is 15s.
Lets estimate the frequency of the vortex shedding using Strouhal number for a single cylinder: ~0.2

So you only simulated 3 vortex shedding periods which is way too short to reach a statistically steady state.
Increase the time step size to roughly 0.05 T...0.01 T (with second order transient formulation) and run for a physical time of at least 50 vortex shedding periods.

I am sorry that I have posted wrongly, I have given time step size as 0.01 only. And I have run it for physical flow time of 150s. The flow should attain steady state by 50 or 60s actually from experimental data, which I am trying to validate with. So, I need to know what else could have been a problem. I will add the mesh and other contours.
Thank you for the reply :-)

[thedal]

So, should I prefer SIMPLEC or Coupled then? Anyway, I have done it with Coupled also, Yet vortices are not shedding. Can you also explain me why PISO should not be used, briefly?

Thank you for the reply.

[FMDenaro]

looking at the residual you now posted, I see that they seems to start oscillating at high frequencies. I suggest to follow the evolution of the total kinetic energy in time as well as some velocity components in some locations.
I cannot exclude that you need a very long time to get the onset of the shedding. What discretizion you used for the convective scheme?

[flotus1]

Slowly running out of ideas...
Did you check the domain size in Fluent? Did you tinker with the units?
You might try to set a lower limit for the number of iterations per time step by increasing the report interval.
Other than that, you could upload your case file so someone can have a look at it directly.

[thedal]

I have used Second order discretization only for Spatial and Time derivaties.

[thedal]

Yes, I have done that umpteen times, yet I didnt find which is the wrong. I will upload the case file for four cylinder in tandem arrangement. Re 100 and s/d is 1.2
Thank you

[flotus1]

One more thing: how do we know that this configuration is supposed to show vortex shedding at Re=100? Experiments? Published simulation results?

[thedal]

I'm trying to validate a numerical and experimental work done in 2012 in a paper. Agrawal et al.
So, I'm sure it gives a finite lift coefficient.