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

Evaluation of length scale ratio for LES, DES, SAS etc.

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 28, 2015, 03:24
Default Evaluation of length scale ratio for LES, DES, SAS etc.
  #1
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 521
Rep Power: 16
siw will become famous soon enough
Hi,

This post is based on the guidance in Best Practice: Scale-Resolving Simulations in ANSYS CFD by F. Menter which is now in the CFX Help.

Before running a SRS (i.e. LES, DES, SAS etc.) a precursor RANS simulation is run from which it is possible to post-process and determine if the mesh in the scale-resolving regions is fine enough to capture to eddy scales that you require. The BPG (version 2.00) page 34 gives the equations:

R_{L}=\frac{\Delta_{max}}{L^{RANS}_{t}};\ L^{RANS}_{t}=\left(\frac{k^{1/2}}{C_{\mu}\omega}\right)^{RANS}

but how is possible to get \Delta_{max} which is the maximum edge length of each mesh element (hexa, tetra, penta, pyra) from CFD-Post in a RANS simulation?

In CFX-Pre, when SAS, DES etc., is selected the Output Control / Results / Extra Output Variable List now includes Mesh Length Scale. Does anyone know what this is exactly because it is not mentioned in the CFX Help Guides? Maybe it is possible to run a SRS for one timestep just to get access to Mesh Length Scale in CFD-Post to evaluated R_{L}. If anyone has conducted any SRS in CFX can they explain how they evaluated that their mesh is resolved enough for their purposes before running the time consuming SRS (or a few iterations of).

Thanks

Last edited by siw; October 28, 2015 at 04:23. Reason: Extra info.
siw is offline   Reply With Quote

Old   October 28, 2015, 06:51
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You do not need exact numbers for this check. Approximate is close enough. So if you are considering this sort of model you should be closely controlling your mesh and you should have a good idea what the element edge length in the important regions are.

I think there is also the length variable accessible in CFD-Post. You would have to check it is correct before proceeding, however.
ghorrocks is offline   Reply With Quote

Old   October 28, 2015, 09:18
Default
  #3
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 521
Rep Power: 16
siw will become famous soon enough
Glenn, you said that one should have a good idea of the element edge length, but what do you use to judge that? Do you approach a scale-resolving simulation with a minimum eddy size that you want to resolve (i.e. from well known energy spectrum) and then use the precursor RANS and equations above to refine the mesh based on some preliminary runs on a baseline mesh?

Just for the purposes of running a test case I am modelling the flow around a wall-mounted bluff body. So having made a preliminary mesh with a refined scale in the body wake, but the element size is not based on any prior knowledge/calcs (what would they even be?), have run a precursor RANS to I was intending to determine the length scale ratio, hence the original CFD-Post question.

Then the next question in mind for the SRS (SAS, DDES or whatever) is what eddy scales do I want to resolve: e.g. 50% down from the integral length scale. There is a plot in Turbulent Flows by Pope (attached here) which I think can be used to relate, generally, the required element size to the desired resolved eddy scales.

By doing this then there would be no need to run SRS for awhile and find the mesh has insufficient resolution to capture the desire eddy scale.
Attached Images
File Type: jpg Pope.JPG (22.3 KB, 51 views)
siw is offline   Reply With Quote

Old   October 28, 2015, 10:31
Default
  #4
Member
 
Join Date: Jan 2015
Posts: 63
Rep Power: 4
highorder_cfd is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
You do not need exact numbers for this check. Approximate is close enough. So if you are considering this sort of model you should be closely controlling your mesh and you should have a good idea what the element edge length in the important regions are.

I think there is also the length variable accessible in CFD-Post. You would have to check it is correct before proceeding, however.
I think that as guideline as element size (Volume)^(1/3) can be used, and L_RANS/element size needs to be at least 4,5 mesh elements per turbulent length scale in the LES region. To be honest I have never run a LES from scratch, but I was trying to learn how to do it time ago and guidelines like these were given in some text I did read.

One of the documents I read is "Quick Guide to Setting Up LES-type Simulations" Prepared and compiled by Dr Aleksey Gerasimov
European Technology Group ANSYS UK Ltd
highorder_cfd is offline   Reply With Quote

Old   October 28, 2015, 19:26
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I have not done LES type models for a long time, but the approach I use for industrial LES models are:

* Do a RANS model to get an estimate of the turbulence field in the flow
* Work out the turbulence length and time scales in the flow
* Note you can skip the previous two steps if you already have a turbulence spectrum or good turbulence information for the flow.
* Use turbulence spectrums or estimates of Taylor length scales to establish the length scales you need to resolve.
* Generate a new mesh with mesh element edge lengths based on what is required. As highorder says you need a few elements inside the desired length scale so you can actually resolve a vortex of that size.
ghorrocks is offline   Reply With Quote

Old   October 29, 2015, 04:50
Default
  #6
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 521
Rep Power: 16
siw will become famous soon enough
Glenn, what do you use to work out the timescale, I had a quick look through Wilcox's Turbulence Modeling in CFD but did not notice a simply relationship? Do you rather use adaptive time stepping and specify in CFX-Pre the CFL number to be about 0.5 and let the solver find its own time step?
siw is offline   Reply With Quote

Old   October 29, 2015, 06:26
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I use adaptive time stepping and let CFX sort the time step out. But home in on 3-5 coeff loops per iteration, not a CFL number.
ghorrocks is offline   Reply With Quote

Old   October 29, 2015, 07:31
Default
  #8
Member
 
Join Date: Jan 2015
Posts: 63
Rep Power: 4
highorder_cfd is on a distinguished road
Hi Glen

1)For how many time steps do you run your simulation before starting the time averaging? ( I read at least 10 000 to start the turbulent structures)
2) For how many time steps the time averaging is usually conducted? (I did read at least other 10 000, thus 20 000 in total)

Thanks in advance
highorder_cfd is offline   Reply With Quote

Old   October 29, 2015, 17:38
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I run it until I am happy the turbulence has reached equilibrium, and then run it long enough that I have convinced myself I have enough that I am covering all important time scales. General guides like you time step count are dangerous as you can think of plenty of scenarios when they do not apply.
ghorrocks is offline   Reply With Quote

Old   October 30, 2015, 04:10
Default
  #10
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 521
Rep Power: 16
siw will become famous soon enough
Glenn, you said above about aiming for 3 to 5 coefficient loops per iteration and not a CFL number, but as the attached images show you need to set conditions in the Analysis Type (e.g. CFL number) as well as in the Solver Controls (i.e. Coefficient Loops). What do you do in this regard?
Attached Images
File Type: jpg Analysis Type.JPG (84.0 KB, 21 views)
File Type: jpg Solver Control.JPG (75.9 KB, 26 views)
siw is offline   Reply With Quote

Old   October 30, 2015, 06:35
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Those controls are managing very different things. The time step control tab only controls the adaptive time step settings. The convergence tab only controls how convergence is handled. You want to make sure that you do not artificially limit the convergence by putting the minimum coeff loops to 1 or 2 and the maximum to a large number, maybe 10. Then you can adapt to 3-5 coeff loops knowing that the solver can use more or less loops if it requires it.
ghorrocks is offline   Reply With Quote

Old   May 18, 2016, 18:56
Default hi
  #12
Member
 
Qureshi M Z I
Join Date: Sep 2013
Posts: 75
Rep Power: 6
m zahid is on a distinguished road
hi, if anyone has this document "Best Practice: Scale-Resolving Simulations in ANSYS CFD" please share this for knowledge . advance thanks
m zahid is offline   Reply With Quote

Old   May 19, 2016, 02:25
Default
  #13
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 610
Rep Power: 14
Lance is on a distinguished road
1 second on google
http://resource.ansys.com/Resource%2...ef+Version+2.0
Lance 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
Smallest length scale in Large eddy simulation maphd Main CFD Forum 12 August 8, 2015 13:04
3D figures for 2D axisymmetric cases and length scale romantico Main CFD Forum 4 June 7, 2010 10:39
Length scale separation in LES Ray Main CFD Forum 1 June 7, 2002 08:50
Von Karman Integral Length Scale Txingurri Main CFD Forum 0 May 2, 2002 12:05
Characteristic Length Scale Thomas P. Abraham Main CFD Forum 2 April 20, 1999 17:16


All times are GMT -4. The time now is 00:48.