Hi everyone,

I tried to model a 3d cylinder of diameter 0.58m. The flow speed is constant at 0.392m/s. This means that the Reynolds number should be around the sub-critical region, i.e vortex shedding will occur.

But i run my transient simulation yesterday, and i only managed to capture the symemtrical vortices at the end of the cylinder, i.e. no vortex shedding was captured.Will this be due to a not-too-fine meshing?

But, I think there might be something wrong with my timesteps. Any of you guys had managed to captured the vortex shedding before, or have any ideas, please let me know.

Thanks, Deloat

Hi,

What Reynolds number is it at? Is it laminar or turbulent? To get vortex shedding you need to run second order differencing in time and space. Also a good idea to have a good boundary layer mesh transitioning to the bulk mesh very smoothly.

Glenn Horrocks

Hi Glen,

The Reynolds number is 2.26x10^5 (sub-critical region). I did my meshing in CFX-mesh, and use the 'point spacing and line spacing' to control the finer mesh around the cylinder.

Is there a better way to control the fine mesh around the cylinder and to control the smooth transition?

Thanks

1) What's your y+ like at the cylinder, and what turbulence model? I had some success recently with a low-Reynolds number mesh with y+ < 1 and using the SST turbulence model, but I am not an expert on this area. I hope others who are experts will advise further.

2) You asked about the timestep. What is the expected shedding frequency, and how does that relate to your timestep?

You can estimate the expected shedding frequency that by using the Strouhal number. http://en.wikipedia.org/wiki/Strouhal_number). For a long cylinder, Massey gives:

f*d/u = 0.198*(1-19.7/Re)

So, ignoring the 1/Re term at your high Reynolds number, the frequency, f, expected is:

f = 0.198 * u / d = 0.198 * (0.392 m/s) / ( 0.58 m) = 0.134 Hz

So the period of the vortex shedding is T = 1/f = 7.5 s. I was advised to use 50 timesteps per period to qualitatively demonstrate vortex shedding recently - I didn't do a sensitivity study to check timestep independence in that case. So if you follow the same guideline I think you want a timestep of about 0.15 s. How does that compare with what you have now?

Please take these as suggestions only - I hope they are helpful but I am not, I stress, an expert at resolving this type of flow to get quantitatively accurate results!

Regards, Andy

Hi,

In this region the flow is turbulent so you need a turbulence model. As Andy20 suggests the SST model with a y+ around 1 would probably be required. Also mesh quality around the cylinder is important. I would use lots of inflation layers (maybe 20-40) and make sure you adjust the mesh settings to give a good transition to the main tet/tri mesh in the near-wake region.

Glenn Horrocks

Thanks for the reply,

You said it's better to have a y+ <1. How do you check whether the y+ is less than 1?? Can you show me please?

Thanks again.

Checking y+ at wall boundaries should be part of every turbulent CFD calculation....

1) Load you results into CFX Post.

2) Create a contour on a wall boundary in the normal way.

3) In the box where you specify the details of the contour, there is a small box with a drop down menu where you select the variable you want to use. This menu only gives a small selection of the variables you can plot.

4) *Near* this menu, there is a separate button which is marked with 3 dots ('...'). This button gives access to the full range of variables you can plot. Click this button! A new box should appear.

5) Choose 'y plus' from the list in the new box. (Do not confuse it with "solver y+" which is also listed in box, but is separate - it is unlikely you will ever want "solver y+". See the CFX help for details).

6) Click OK and continue setting up the contour as normal.

7) Review the results.

8) Y+ is not the only variable you should be checking - search the CFX help for details on what values of y+ you should be using, and also read the section about how many nodes you need in the boundary layer.

Anyone who is new to CFD should *read* the CFX help pages very carefully for the advice they give on mesh checking and solution checking. I've read them almost from cover to cover and I still have to refer to them almost daily and often learn something new...

Missing out checks on Y+ and boundary layer meshing will cause inaccurate results. They might *look* realistic and converge well, but unless the y+ and other parameters are correct they will be inaccurate.

Good luck, Andy