CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   1 Was FSI for a flow over a cylinder (http://www.cfd-online.com/Forums/cfx/85532-1-fsi-flow-over-cylinder.html)

 vmlxb6 February 28, 2011 13:51

1 Was FSI for a flow over a cylinder

3 Attachment(s)
Hello,

I need help with this as I am stuck on this for a long time now. I am trying to find out the displacement of a cylinder in a cross flow. The cylinder is subjected to move in the transverse direction only. I am not getting correct displacements of the cylinder. I am using a CEL expression for Mesh deformation.
To check my mesh and BC, I tried to run a transient case of a flow over a fixed cylinder and compared the results. They were alright. That means the Mesh, Boundary layer, physics of the problem, Boundary conditions are all fine. But when I use this mesh deformation, I cannot validate my results.

My geometry simple. It is just a square domain with a circle at the centre (i.e 2-D)

The CEL expression is very much similar to the CEL expression given in the tutorial Ch: 22 Fluid Struct interaction and mesh deformation.

The only difference is that the tutorial has a spring while I also have a damper with the spring.

I am attaching the pic of the mesh and the CEL expression am using.

Any kind of suggestion is highly appreciated. Thank you.

Attachment 6698

Attachment 6699

Attachment 6700

 cfdgremlin February 28, 2011 15:59

I've done very similar calculations for turbulent flow, with some reasonable results.

Are the forces on the cylinder what you expect for the flow Reynolds Number? If they are in the right ball park, then it is a simple matter to calculate the free undamped vibration amplitude and compare it with what you get out of CFX. This will at least tell you if your expression formulation is right.

 vmlxb6 February 28, 2011 16:07

@ cfdgremlin

I have not compared the forces yet. What I presumed was that the displacements were low bcoz of low forces. Is there any papers/txt book etc with which I can compare my force data for a moving cylinder, to see if ???
I guess the forces on the stationary cylinder will be different from that of a moving cylinder.
I tried running a stationary cylinder case (which did not involve FSI-mesh motion), and the forces/lift coeff were correct.

Thank you for writing !!!

Regards,

Prof. Chaos

 ghorrocks March 1, 2011 18:20

Have you done all the normal sensitivity checks? Mesh, time step, convergence?

 singer1812 March 1, 2011 18:30

You can apply the motion to either a subdomain or the walls for this type of problem. Using a subdomain allows you to push the deformed mesh into a region that is better able to handle it. If you dont expect a large deformation, by all means move the walls.

Havent checked your ccl expressions but they should boil down to

a=F/m

after manipulation:

dCYLINDERNew=(velCYLINDEROld+F/mCYLINDER*tstep)*tstep+dCYLINDEROld

I think F in your case should be

FFLow-C*velCYLINDEROld-k*dCYLINDEROld

Which I dont have time to check if all this boils down to what you had in your num/dem ccl.

You should monitor, at the very least, the following values to see if they make sense:

FFLow
C*velCYLINDEROld
k*dCYLINDEROld

And with the equations above mesh motion should be defined as Specified Displacement

 vmlxb6 March 3, 2011 04:19

@ Ghorocks & singer 1812

I used the same mesh to simulate the lift forces over a stationary cylinder. And it gave correct results. Doesn't that mean that the mesh is fine ???

The problem could be when the mesh deforms. The boundary layer near the cylinder walls also deform thus giving wrong results. (I dont know, Its just a wild guess.)

Am using Mesh stiffness to increase near small volumes & stiffness model exponent = 2. Can that cause a problem ???
Should I be using 'increase near boundaries' ???

@ Ghorocks: The solution seems to be converging. The time step is small enough. The RMS courant is close to 0.22 & max courant is 0.7

How to check if the mesh is fine. My mesh is certainly fine for a transient stationary case. But how do I find out the same for a moving mesh ???

@singer: The cylinder wall does have specified displacement. How do I know if Fflow, C*vel or K*disp makes sense ???

 singer1812 March 3, 2011 10:30

You are to decide if they make sense or not.

Are you starting this from a solution interpolated from the non-moving mesh solution? Perhaps, FFLow should be close to the value from that, near the beginning for solution.

At the start of solution I would guess that the spring and damping term should be small, and if the cylindar continues to not move much, should balance out FFlow. If that is not the case, maybe you have something messed up in your logic.

 vmlxb6 March 4, 2011 10:25

@ Ghorocks & singer 1812

1. For a flow over a (moving) cylinder. If I scale my force i.e multiply by the length, should the 2-D case give the same result as that of a 3-D case.

2. For a transient case simulation, is 10^-4 a good convergence criteria ??? Or should I be reducing further.

Thank you.

 ghorrocks March 6, 2011 18:10

Quote:
 For a transient case simulation, is 10^-4 a good convergence criteria ??? Or should I be reducing further.
That is a good starting point but you need to prove it is OK for your situation with a sensitivity study.

 vmlxb6 March 6, 2011 18:44

Thanks Ghorrocks

 vmlxb6 March 15, 2011 08:11

Hello,

I have run out of options. I have been trying this for a long time now but unable to match experimental values. Can anyone please have a look at my files as I have reached the dead end.

Thank you.

 cfdgremlin March 15, 2011 14:49

Can I ask just a couple more questions:

1. Is this a laminar or turbulent flow simulation?

2. What are the details of the experiment? Are the results from a published paper? What are the end-load conditions? Is it a rigid or flexible cylinder? What fluid is used? etc ...

3. How far out are the displacements in the simulation compared to the experiment? Is it a factor of 2, 10, 100?

Thanks

 vmlxb6 March 15, 2011 15:29

Hey,

1. The experiments were run at Re = 525. Hence Laminar.

2. End load conditions ????? I have no idea

3. It is a rigid body

4. Published in Journal of fluid & structures

They are getting A/D = 0.06 while am getting it as 0.03~0.04. In the CEL expression that I have attached, I have used a first order accurate forward differencing scheme. That may be the reason. I dont know it yet. Am still figuring it out.

Thank you for responding.

 cfdgremlin March 16, 2011 12:17

Are you able to reveal the details of the paper (name, author, date)?

 vmlxb6 March 16, 2011 12:50

Name: On the maximum amplitude for a freely vibrating cylinder in cross-flow

Author: J.T. Klamo, A. Leonard, A.Roshko

Journal: Journal of Fluids & structures 21(2005) 429-434

 cfdgremlin March 21, 2011 13:35

I have only been able to read the abstract, but the authors are well renowned in the field.

In the simulations I have performed, both with using CEL expressions and 2-way FSI with ANSYS, it has been difficult to exactly match the experimental data (although mine were at higher Reynolds numbers). The maximum amplitude usually occurs at "lock-in", and this phenomena is associated with a sharp jump in amplitude ratio.

I would recommend that you perform a number of simulations either side of your targeted conditions to see how the amplitude responds.

Hope this helps.

 vmlxb6 March 21, 2011 14:05

How are you doing a 2-way FSI ??? Does that mean that your Cylinder is deforming ?????

Can I have a look at your CEL expression ??? What discretization scheme are you using ???

Thanks

 vmlxb6 May 16, 2011 02:29

@ cfdgremlin

Hey,

You mentioned that you used a CEL as well as a 2 way FSI. My question is, was the 2 way used to find the structural deformation of the cylinder ???

Thank you.

 All times are GMT -4. The time now is 15:43.