CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   wake galloping simulation (http://www.cfd-online.com/Forums/cfx/97106-wake-galloping-simulation.html)

colopolo February 9, 2012 00:18

wake galloping simulation
 
Hi, All

I am trying to simulation of wake galloping in case of two tandem cylinders.

Before doing this, I ran simulation of viv of single cylinder at low-reynolds number (Re=200).
The results is a good agreement with the results of wind tunnel test.

After that,
I put another cylinder behind single cylinder (distance = 4D) at Reynolds number is 20000.

The 2nd cylinders does not move at all even if velocity is high and time step is enough small for satisfying Courant number.

my condition is like this.
D=0.08 m. Vel=4.5m/s
density=air density
the first distance is around 0.00003m (it satisfies yplus)
I suppose y_displacement of cylinder is a quite big (0.5~1.0*D) with respect to velocity.
motion equation is written by CCL. (this ccl is same format as viv of single cylinder)

The below is a part of CCL;
C = 0.053 [N s m^-1]
Dens = 1.185 [kg/m^3]
Free Stream = 4.5 [m s^-1]
SectionArea = alength*Span
alength=0.02 [m]
Span = 0.08 [m]
kSpring = 298.3 [N m^-1]
mCYLINDER = 3.44 [kg]
tStep = 0.01 [s]
CD2 = Drag2/(0.5*Dens*SectionArea*Free Stream^2)
CL2 = Lift2/(0.5*Dens*SectionArea*Free Stream^2)
FFlowY2 = force_y()@cylindertwo
Drag2 = force_x()@cylindertwo
FY2 = force_y()@cylindertwo
dCYLINDERDenomY2 = kSpring + mCYLINDER/tStep^2 + C/tStep
dCYLINDERNewY2 = dCYLINDERNumerY2/dCYLINDERDenomY2
dCYLINDERNumerY2 = FFlowY2 + mCYLINDER*velCYLINDEROldY2/tStep +
mCYLINDER*dCYLINDEROldY2/tStep^2 + dCYLINDEROldY2*C/tStep
dCYLINDEROldY2 = areaAve(Total Mesh Displacement Y)@cylindertwo
velCYLINDEROldY2 = areaAve(Mesh Velocity Y)@cylindertwo

C and k from experiment.

Could you give me any ideas why it does not move at all?

Summary;
1. good moving of a single cylinder at Re=200.
2. not moving of 2nd cylinder of tandem arrangement at Re=20000.

Thanks in advance.

ghorrocks February 9, 2012 07:25

Is the Re=2e5 simulation showing transient flow structures? The turbulence model might be suppressing all the turbulent flow structures, leaving a steady state flow and therefore no motion.

colopolo February 9, 2012 22:50

Quote:

Originally Posted by ghorrocks (Post 343538)
Is the Re=2e5 simulation showing transient flow structures? The turbulence model might be suppressing all the turbulent flow structures, leaving a steady state flow and therefore no motion.

Thanks for your comment.
According to result of CFX,

Domain Name : Default Domain
Global Length = 4.4283E-01
Minimum Extent = 2.0000E-02
Maximum Extent = 2.7200E+00
Density = 1.1850E+00
Dynamic Viscosity = 1.8310E-05
Velocity = 4.1022E+00
Advection Time = 1.0795E-01
RMS Courant Number = 7.2755E+00
Maximum Courant Number = 3.2937E+01
Reynolds Number = 1.1757E+05


So, do you have any ideas to solve a problem which you pointed out?
what turbulence model is best for my case?

Thanks

ghorrocks February 9, 2012 23:56

First, can you answer the question - does your current simulation show transient structures?

colopolo February 9, 2012 23:58

Quote:

Originally Posted by ghorrocks (Post 343703)
First, can you answer the question - does your current simulation show transient structures?

I solved my case in anyway.

Thanks for all your help

ghorrocks February 10, 2012 01:14

Can you post what you did to fix the problem for future reference?

colopolo February 10, 2012 04:38

Quote:

Originally Posted by ghorrocks (Post 343709)
Can you post what you did to fix the problem for future reference?

I got a clue from your comment. now I am doing my approach is working or not. I will post it in later.

colopolo February 14, 2012 04:41

1 Attachment(s)
Quote:

Originally Posted by colopolo (Post 343731)
I got a clue from your comment. now I am doing my approach is working or not. I will post it in later.


My idea was failed -_-;;

I have reviewd papers about wind-induced vibration of two tandem cyliders.
Most of studies have been conducted at low-Reynolds numeber (such as, 100, 200 or up to 1000).

the result of my simulation is a kind of good agreement with the results of experiminet or numerical simulation at Re=200.

Main purpose of my simulation is to comapre with the results of two tandem cable (downstream is oscillating due to wake galloping) in wind tunnel test.

The experimental condition is as below;
1. Diameter =0.08 m,
2. spacing between cylinders : 3D~ 7D
3. wind velocity - 0m/s ~ 6 m/s
4. natural frequency of cylinder =1.68 hz
(I attached wind tunnel test results.)

The range of reynolds number is approximately 5E3 ~ XX*10E4. it is a quite higher reynolds number than Re =200 or something.

I have no idea what I am missing. I checked CD, CLrms of fixed tandem cylinder before 2dof simulation, I got reasonable values.

Then I ran transient case using sst model with y+~1 and checked turbulence structures (such as vorticity contour).

But I got unrealistic value of displacement.

Some of papers mentioned that tow dimensional flow was not possible for Re>250.

Do I approach this case by three-dimensional simulation?
or what am I missing ?

Thanks in advance.

ghorrocks February 14, 2012 17:44

More than the flow being three dimensional, you will probably find the traditional RANS turbulence models are unsuitable for this regime. You may well have to use a DES/SAS/LES style simulation to correctly capture the shed vorticies.

colopolo February 14, 2012 20:09

Quote:

Originally Posted by ghorrocks (Post 344458)
More than the flow being three dimensional, you will probably find the traditional RANS turbulence models are unsuitable for this regime. You may well have to use a DES/SAS/LES style simulation to correctly capture the shed vorticies.

Thank you for your comment.
That is right. If I run 3D simulation I have to use a DES/SAS/LES.

I wonder that this reason really makes the cylinder does not move or not.
Do I have to run 3D?

I still want to rung 2D simulation for saving time and cost.

ghorrocks February 14, 2012 20:48

DES/SAS/LES are inherently 3D methods. You cannot do them 2D.

colopolo February 14, 2012 20:51

Quote:

Originally Posted by ghorrocks (Post 344479)
DES/SAS/LES are inherently 3D methods. You cannot do them 2D.

I know they are being in 3D simulation.

My question is;

Above the ranges of Reynolds number, does it impossible to let cylinder move in 2D simulation?

ghorrocks February 14, 2012 20:54

Can you clarify your question? Do you want to constrain the cylinder to 2D motion or are you asking if the Re range you quoted (5e3-e4) can be modelled at 3D flows?

colopolo February 14, 2012 21:07

Quote:

Originally Posted by ghorrocks (Post 344481)
Can you clarify your question? Do you want to constrain the cylinder to 2D motion or are you asking if the Re range you quoted (5e3-e4) can be modelled at 3D flows?

sorry to confuse you.

0. 2d simulation at low reynolds number case
- reasonable result (done)
1. I did 2D simulation of experimental case.
2. I got an wrong result - not moving cylinder.
3. I thought what I was wrong in set-up simulation.
- ccl is ok
- grid is ok
- maybe flow condition is wrong? <- beacuse it is high reynolds number?
-> drive me this simulation should be run in 3D?
(this is question #1)

4. if I don't need to run 3D, what shall I do to set up 2d simulation for cylinder motion? constrain problem in my 2D simulation?
(this is question #2).

ghorrocks February 14, 2012 23:10

I assume the Re of the experimental case is 5e3-e4. In this range you would expect vortex shedding, and I suspect (but have not confirmed) that it would be 3D, not 2D and turbulent. I also suspect that it starts becoming turbulent around this Re so you need LES/SAS/DES.

So if my suspicions are correct you will need to run it 3D with a LES/DES/SAS model.


All times are GMT -4. The time now is 11:23.