CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Suitable mesh resolution for Deteched Eddy Simulations

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 17, 2013, 02:24
Default Suitable mesh resolution for Detached Eddy Simulations
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
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.

Last edited by siw; June 17, 2013 at 09:23.
siw is offline   Reply With Quote

Old   June 17, 2013, 06:18
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   June 17, 2013, 08:06
Default
  #3
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
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.

Last edited by siw; June 17, 2013 at 08:34. Reason: Typo
siw is offline   Reply With Quote

Old   June 17, 2013, 08:31
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   June 17, 2013, 08:57
Default
  #5
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Glenn, you replied minutes before I corrected my previous post.

I'd be interested in your comments on the remainder of my last post.
siw is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
[ICEM] Unstructure Meshing Around Imported Plot3D Structured Mesh ICEM kawamatt2 ANSYS Meshing & Geometry 17 December 20, 2011 12:45
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
Mesh size for particulate flow simulations Shahri Main CFD Forum 0 March 24, 2009 18:40


All times are GMT -4. The time now is 07:17.