CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Desperate HELP please: Vortex Shedding not showing circular cylinder (http://www.cfd-online.com/Forums/fluent/101327-desperate-help-please-vortex-shedding-not-showing-circular-cylinder.html)

u50mb9 May 1, 2012 08:00

Desperate HELP please: Vortex Shedding not showing circular cylinder
 
Hi I've been stuck at the same point for 2 weeks and really need help.

My vortex shedding behind the circular cylinder is not showing. I am running a 3d, LES model with smaller mesh closer to the cylinder. I feel I may have made a simple error somewhere but I cant seem to correct it.

Using a time step of 0.0001 with 400 time steps with non-iterative advancements. Also using PRESTO, PISO and Bounded Central differential Momentum

What viscosity ratio and intensity should I use? The user guide seems to be very complex.

ANY advice is welcome. Please help my thesis is due shortly and I need to verify this model.

xrs333 May 1, 2012 09:13

you are modeling Karman vortex street phenomenon, so you have to make it sure that it will emerge, the key is Reynolds Number.

u50mb9 May 1, 2012 09:19

Thanks for your reply, I'm using a Re of 1.4 x 10^5 but I cannot see the vortex street after 100 Iterations. Any suggestions how to correct this?

xrs333 May 1, 2012 13:56

have you estimated the vortex shedding frequency?

LuckyTran May 1, 2012 14:22

Quote:

Originally Posted by u50mb9 (Post 358625)
What viscosity ratio and intensity should I use? The user guide seems to be very complex.


what???? You are running LES, there is no viscosity ratio and intensity.

For LES, is your solution turbulent? One problem that often occurs with LES is that the solution relaminarizes.

Also, what's the relative time, non-dimensionalized? i.e. How much is 400 iterations?

How was your initializing? If you didn't initialize your flow with a RANS solution, expect it to take more time to develop into the proper flow field.

u50mb9 May 1, 2012 15:48

Quote:

Originally Posted by LuckyTran (Post 358678)
what???? You are running LES, there is no viscosity ratio and intensity.

For LES, is your solution turbulent? One problem that often occurs with LES is that the solution relaminarizes.

Also, what's the relative time, non-dimensionalized? i.e. How much is 400 iterations?

How was your initializing? If you didn't initialize your flow with a RANS solution, expect it to take more time to develop into the proper flow field.


When setting my velocity Inlet, I chose spec. method of turb intensity & turb viscosity ratio.

I've been told to use a non-dimensional time step of 0.005.

I didn't initialize with RANS but I will try that now. When setting up RANS how do I know what kinetic energy and diss rate factors to use?

Kind regards

LuckyTran May 1, 2012 18:23

Quote:

Originally Posted by u50mb9 (Post 358691)
When setting my velocity Inlet, I chose spec. method of turb intensity & turb viscosity ratio.

I've been told to use a non-dimensional time step of 0.005.

I didn't initialize with RANS but I will try that now. When setting up RANS how do I know what kinetic energy and diss rate factors to use?

Kind regards

Okay I see. With that method you do specify an intensity and viscosity ratio. You should know those parameters, they are your inflow conditions.

With no initialization, I would not expect to see any meaningful features before t=1, I would wait until t=10 but you can perhaps maybe see some structures develop by t=2, it is possible. With RANS initialization, it will be much quicker (so perhaps t=2 if RANS is used). Don't waste time to do the RANS initialization now, it is better to just keep iterating with the solution that you already have computed. Keep in mind that the solution is not time-accurate until the effect of the initial conditions has completely been removed from the computational domain (probably t~10, or more).

Again, with LES, always check to make sure your solution didn't relaminarize and that it makes sense. Just look at your velocity for the current timestep.

Also, disable the non-iterative time advancement if possible.


All times are GMT -4. The time now is 22:22.