CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Suitable mesh resolution for Deteched Eddy Simulations (http://www.cfd-online.com/Forums/cfx/119405-suitable-mesh-resolution-deteched-eddy-simulations.html)

siw June 17, 2013 02:24

Suitable mesh resolution for Detached Eddy Simulations
 
Hi,

I need to conduct some DES of highly separated flows (external aerodynamics of wall-mounted bluff bodies). I've read up on the background of DES and some mesh requirement papers (refs 1 and 2). However, in my case I do not know the suitable mesh resolution to get a successful DES.

I cannot find the approach others use to conduct DES and how they know it was suitably achieved. Could those who have used DES share their approach: e.g. how do you know your mesh is suitable and how do you determine your mesh requirements (the references below are vague and don't help with starting out), do you often have to repeat simulations after finding in post-processing that your mesh (and maybe timestep) need refinement. Any other tips from people who have conducted successful DES could be useful. I can foresee that I'm just going to end up with URANS rather than DES results.

Thanks

Ref 1: F. R. Menter, Best Practice: Scale-Resolving Simulations in ANSYS CFD, Version 1.02, April 2012.
Ref 2: P. R. Spalart, Young-Person's Guide to Deteched-Eddy Simulation Grids, NASA/CR-2001-211032, July 2001.

ghorrocks June 17, 2013 06:18

This is a tricky subject. I have not done a mesh refinement for DES but I have done one for LES which is similar. The issue is that the dissipation in the model is linked to the mesh size as it is very difficult to get a sub grid model which converges to a mesh independant solution.

So for this type of simulation I would recommend either:
1) do a benchmark simulation against quality DNS or experimental results on something like turbulence decay or something like that. If you can get the turbulent decay about right then you are on the right track.
2) do a turbulence decay simulation and check you get the -5/3 turbulence energy spectrum. This is not as strong a validation, but if you can get the -5/3 decay then you know you are about right.
3) Compare your results to equivalent experimental results. If your simulation is in error then keep refining until you get the experimental results.

siw June 17, 2013 08:06

Thanks for the reply Glenn, very useful since you've done similar for LES. A direct question to you Glenn, in your PhD LES work how did you go about your initial mesh sizing choices to start out if your mesh was suitable for LES and capturing the smallest scales that your needed?

This is for my PhD where I've found a gap in the literature. So there are no other studies which consider the same geometry (all be it a very simple one) at the same flow conditions (Mach and Reynolds numbers). However, I have found a few papers using a similar geometry and at lower Mach and Re number which I'll have to compare with first.

I was not initially thinking about mesh independent DES as this is difficult since the mesh sizing is the switch between the URANS and LES parts. I was more considering at this time about making a suitable initial mesh for DES and where to start. How do others go about setting suitable DES mesh sizings. I don't want to spend days (weeks, months) running mesh after mesh only to find that each (which get finer) just give URANS results.

How does one go about assessing their data to determine the energy cassade scales (the -5/3 slope)? I've only ever done RANS and URANS before. Can this be done in CFD-Post? I cannot see anything in the User Guide to help.

ghorrocks June 17, 2013 08:31

You should read some turbulence textbooks for more detail on this. Turbulence Modelling for CFD by Wilcox is my guide, but there are others.

The basic idea is you get velocity data, filter it to separate the bulk flow and turbulent components, then do an FFT on the turbulent component. But how you actually do this depends on the method you use.

My preferred approach is to put a monitor point in to report velocity (preferably U, V and W, then you pick up any anisotropy) to report velocity versus time at a point. You then use time averaging to give you a bulk flow and a turbulent component, then FFT on the turbulent bit. My PhD thesis has an example of this in the square piston modelling chapter (http://hdl.handle.net/2100/248).

You can also filter spatially, this is also a valid approach. But the post processing to get spatial filtering is much harder than temporal filtering.

siw June 17, 2013 08:57

Glenn, you replied minutes before I corrected my previous post.

I'd be interested in your comments on the remainder of my last post.


All times are GMT -4. The time now is 11:58.