Problem using perturbUCylinder
 

Hi everyone,

I am using perturbUCylinder and had problem getting a turbulent velocity profile for my pipe simulation. Instead, I get a laminar velocity profile.

As I checked the perturbU.C file of this utility I saw that the code has used a parabolic profile for x-velocity, which is the shape of a laminar velocity profile. I am suspicious that this may be a reason for not getting a turbulent velocity profile.

Does anyone have any idea why Eugene has used a parabolic profile (a laminar velocity profile) for what must be a turbulent flow in the end?

Thanks in advance.

Probably because it is simple to define the laminar profile, and to make sure that it's in balance with the background pressure gradient. You can apply whatever you want though - for example, I have done as you suggest, and applied a more turbulent looking profile, to try and boost the speed of transition (the turbulent profile has a larger near wall gradient, and so greater turbulence production). I have also played with the perturbation settings, again to kick off the transition in my DNS. Just be careful not to overstimulate things though - it can take a Loooooong time to relax back to equilibrium conditions if you do.

Thanks a lot.

One more question. Have you ever got a turbulent field as a result of using the original perturbUCylinder utility (the parabolic one)? I want to know whether I really have to go through changing the code.

Also, if you have published or shared your modified code anywhere, please let me know. I think it would be very helpful to many people like me.

Yes, but for my case I had to ramp up the strength of the perturbations, ie. play with the coefficients (I boosted duplus by a factor of 2 and eps by a factor of 4 I think). I think that was probably necessary since my case was running at a lower Re number than Eugene's original run. As for code - I am just using his code; you can change the coding for the parabolic profile to whatever profile you want. But I would suggest starting with the laminar profile, maybe boost the coeffs and then run again and see if the initial perturbations start to "take off" and propagate (good) or die away slowly (bad - so bump up the perturbation further).

Good luck.

By the way - I found that plotting Q isocontours alongside contour plots of streamwise and spanwise velocity just off the wall was a good way of keeping track of what was going on. You could tell really easily whether the initially fairly uniform perturbations were starting to go nonlinear and taking off, or were instead dying away. Attached are a few example snapshots.

How to chose the value of Q
 

Hello Tobermory, recently im beginning to plot Q isocontours using paraview, I wonder how to chose the value of Q? I've ploted the Q isocontourss in Channel as blow, the value of Q is 0.002. But I do not know how to chose Q, and why using this value
https://testnew-1307662376.cos.ap-ch...m/Q_0_002.tiff

The magnitude of Q will be tied in to the characteristic velocity and lengthscales of the flow problem that you are solving. However, for the current purposes, the precise value is not important - you are just using it to visualise the perturbations to the velocity field, to observe whether these go chaotic or not. So, with that in mind, just play with the iscontour threshold value in paraview until you resolve the features that you want to see. Good luck.

I'm trying to download the code but receiving .unk file (unknown type) . How could you open the file?

Thanks to wyldckat added missing file. Link:

https://openfoamwiki.net/index.php/Contrib/perturbU