CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Increasing instability for flow around as cylinder. (http://www.cfd-online.com/Forums/main/112592-increasing-instability-flow-around-cylinder.html)

jgrimshaw January 31, 2013 10:31

Increasing instability for flow around as cylinder.
 
I am currently attempting to model flow around a stationary cylinder at a Re=200,000 using Fluent 14. However, after running my simulation it appears my solution is too steady as no vortex shedding occurs.
I am currently using the URANS solver coupled with the K-e turbulance model and have tried running the simulation.
I originally used a 1st order upwind scheme and left the Pressure - Velocity coupling as SIMPLE. I then changed this to a 2nd order upwind scheme and used the PISO to do the pressure - velocity coupling.
I have found my wall y+ value and applied the appropriate wall function to my simulation but in doing so i coarsened my mesh.

Does anybody have any suggestions on how to create instability in the flow and hence produce vortex shedding?

RodriguezFatz January 31, 2013 10:51

How long have you been waiting? My experience is that you have to wait quite a long time until von Karman shows up...
Is your timestep small enough?

jgrimshaw January 31, 2013 11:18

My time step was originally 0.1s but I then changed this to 0.05s.

RodriguezFatz January 31, 2013 11:24

What is the radius of your cylinder and the velocity of your fluid?

FMDenaro January 31, 2013 11:25

what about your grid resolution? have you used second order accuracy in time?
check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

jgrimshaw January 31, 2013 11:45

My radius is 0.5m and my flow velocity is 2.364 m/s.

RodriguezFatz January 31, 2013 12:39

Quote:

Originally Posted by jgrimshaw (Post 405330)
My radius is 0.5m and my flow velocity is 2.364 m/s.

Ok, that sounds ok for the time step. Now, could you post a picture of your mesh?

How many timesteps have you been waiting before you stopped?

jgrimshaw February 11, 2013 09:28

Sorry for the slow reply I have been out of the office for a while. I am currently running 600 time steps.

The mesh i am using is posted below, along the axis it has 96 elements with a bias factor of 10. The average element size was 0.328125m which gives a CFL=0.3602.

jgrimshaw February 11, 2013 09:32

Quote:

Originally Posted by FMDenaro (Post 405327)
what about your grid resolution? have you used second order accuracy in time?
check also the value in time of the vertcal component in some points at the rear of the cylinder, along the longitudinal direction, and see if it is really steady for several non-dimensional time unit.

The time step accuracy is second order, I have been assuming it is steady as on my Cl vs time plot (otherwise known as convergence history) I have an oscillating graph which quickly dampens wafter 20% of the time has been ran.

jgrimshaw February 11, 2013 09:33

Is there any good fluent literature or troubleshooting websites that either of you could recommend.

RodriguezFatz February 11, 2013 09:38

Quote:

Originally Posted by jgrimshaw (Post 407129)
The mesh i am using is posted below

I dont find it...

jgrimshaw February 11, 2013 09:44

1 Attachment(s)
Sorry it is in the attachment of this post

RodriguezFatz February 11, 2013 09:49

What is your y+ currently?

jgrimshaw February 11, 2013 10:54

1 Attachment(s)
I do not have a exact value for the y+ around the cylinder, but the values range between 50 - 850. I have attached the plot below.

RodriguezFatz February 11, 2013 10:59

That means you are using wall functions. Maybe these wall functions restrain eddy shedding? Did you try to resolve the sheath (y+<=1)?

BTW: I don't think you need a turbulent inlet flow to get a von Kármán street. As I understand it, it is an instability that has in the first instance nothing to do with turbulence.

RodriguezFatz February 11, 2013 11:48

Are you using air? I quickly rebuild your case and I am getting a nice vortex street right from the start... Maybe you should post your settings...

Martin Hegedus February 11, 2013 16:33

You can try giving it just a little kick of angle of attack so the problem is not completely symmetric.

That being said, the instability should develop on it's own even if things were "symmetric" but it will take a while. The time to instability is dependent on how accurate the numerical method is. If it was "perfectly" accurate, the problem will theoretically remain symmetric. In other words, it is statically stable but dynamically unstable. However, I'm not sure what your turbulence model will do. It may dampen out the dynamic instability. This is a reason DES is used.

Martin Hegedus February 11, 2013 16:40

Oh, one thing to watch is lift. If it starts to oscillate from machine zero you're on your way. But, it sounds like this was zero for you? And, just to be clear, you do have two big vortices (symmetric about x axis) behind your cylinder?

arjun February 11, 2013 16:54

i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

RodriguezFatz February 12, 2013 03:08

Quote:

Originally Posted by arjun (Post 407234)
i had this issue for long time with lattice boltzmann, every time i tried i got exactly like this. No vortex shedding, untill i put the outer boundaries far away.

But do you think his domain looks like it is too small compared to the radius?


All times are GMT -4. The time now is 05:19.