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

LES Velocity Profile

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 28, 2013, 10:55
Default LES Velocity Profile
  #1
Member
 
Join Date: Apr 2011
Posts: 38
Rep Power: 7
amanbearpig is on a distinguished road
Hi, I am having trouble running a turbulent simulation of flow over a flat plate. I have air at 1 m/s traveling over a 10m long plate, giving me a Re~600,000 at the outlet. I have followed the Fluent Best Practices guide for my mesh, with my y+ <1, x+ ~ 20, z+ ~ 40.

I started with a k-e RANS run, took the velocity and turbulence data from 1m in, set that as my inlet boundary condition, re-ran RANS again, then took that solution as my initial solution for LES. I initialized turbulence and changed to the transient solver, and am using the vortex method at the inlet for turbulence/unsteadiness. I ran for about 5 flowthroughs, then started collecting statistics. After ~10 flowthroughs, I have looked at the results, and my velocity profile (using mean velocity) is not right.

I plotted my u+ vs y+ and compared to the law-of-the-wall expected results (Spalding curve) but my results do not match. They follow the expected curve for ~1/3 of the curve length, then rise up, giving me a higher u+ than I should get for the corresponding y+.

I have tried this using RANS, LES, and DES. RANS and DES match the Spalding law-of-the-wall curve beautifully, but LES does not. What could be my problem?
amanbearpig is offline   Reply With Quote

Old   May 28, 2013, 11:10
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,220
Rep Power: 22
flotus1 will become famous soon enoughflotus1 will become famous soon enough
So your computational domain is 10 m in streamwise direction. What about the other directions? What boundary conditions did you use?
Quote:
I started with a k-e RANS run, took the velocity and turbulence data from 1m in
If you really want to do it this way, you should take the profiles from as far downstream as possible.

Nevertheless, I recommend periodic boundary conditions between inlet and outlet. This will leave you with much less modeling uncertainties concerning the inlet specification.
Additionally. z+=40 and x+=20 are probably too coarse for a wall-resolving LES.
flotus1 is offline   Reply With Quote

Old   May 28, 2013, 12:01
Default
  #3
Member
 
Join Date: Apr 2011
Posts: 38
Rep Power: 7
amanbearpig is on a distinguished road
Quote:
Originally Posted by flotus1
So your computational domain is 10 m in streamwise direction. What about the other directions? What boundary conditions did you use?
My domain is ~.5m in the normal direction (y) and .36m in the spanwise direction (x). My inlet is velocity inlet, my outlet is outflow ( I compared with pressure-outlet as well and there is little to no difference). The top of my domain is given the 'symmetry' condition, with the bottom (the plate) set as 'wall'. The boundaries in the spanwise direction are periodic boundaries.

Quote:
If you really want to do it this way, you should take the profiles from as far downstream as possible.
I set my inlet boundary condition from the the profiles at 1m in just to aid in tripping turbulence with the vortex method. When I calculate my velocity profile I do it at 10m.
amanbearpig is offline   Reply With Quote

Old   May 28, 2013, 12:11
Default
  #4
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 544
Blog Entries: 14
Rep Power: 18
sbaffini will become famous soon enough
Some details are missing:

1) Is x your streamwise direction and z the spanwise one? If it is the case i would invert your spacings as dx+=40 and dz+=20. Still, unless you are using a periodic condition streamwise and an equilibrium boundary layer, these values are gonna change in x.

2) What are your discretization parameters? Central schemes for convection and second order in time are mandatory. Also, my experience is that PRESTO! is more dissipative than other pressure discretizations but it is the only one providing meaningful spectral energy distributions and RMS profiles. Finally, the courant number should be below 1, possibly around 0.1

3) What is your SGS model? Static Smagorinsky model is not suitable here and other options should be considered.

4) How much wrong is the velocity profile? And the velocity fluctuations (RMS)? The shear stress (average uv)? Is it laminar like or just overestimating the log part and the x-RMS peak?

5) The vortex method (which is the method of choice in Fluent) requires mean vleocity and turbulent profiles at inlet. I don't understand your procedure to assign them. I would compute an Equilibrium B.L. solution with a Reynolds Stress Model and simply assign them to your inlet method.
Why do you need to do that twice?

At the end of the day, this is still a damn problem to simulate with a low order code and in no way you can be sure of the success of your simulation.
sbaffini is offline   Reply With Quote

Old   May 28, 2013, 13:41
Default
  #5
Member
 
Join Date: Apr 2011
Posts: 38
Rep Power: 7
amanbearpig is on a distinguished road
Quote:
Originally Posted by sbaffini
1) Is x your streamwise direction and z the spanwise one? If it is the case i would invert your spacings as dx+=40 and dz+=20. Still, unless you are using a periodic condition streamwise and an equilibrium boundary layer, these values are gonna change in x.
Sorry, yes, x is my streamwise direction and z spanwise, and I am actually using the mesh sizing you suggest above, apologies if I mistakenly said otherwise above.

Quote:
2) What are your discretization parameters? Central schemes for convection and second order in time are mandatory. Also, my experience is that PRESTO! is more dissipative than other pressure discretizations but it is the only one providing meaningful spectral energy distributions and RMS profiles. Finally, the courant number should be below 1, possibly around 0.1
I'm using PISO scheme for Pressure-Velocity coupling, Bounded Central Difference for Momentum, Body Force Weighted for Pressure, and Bounded 2nd Order Implicit for Transient discretization. My max CFL number is well below 1, close to ~.1 actually as you suggest.

Quote:
3) What is your SGS model? Static Smagorinsky model is not suitable here and other options should be considered.
I am using the WALE subgrid scale model. I have also examined the Dynamic Smagorinsky model but this showed no great improvement.

Quote:
4) How much wrong is the velocity profile? And the velocity fluctuations (RMS)? The shear stress (average uv)? Is it laminar like or just overestimating the log part and the x-RMS peak?
The shear stress is OK, it matches decently well. The problem is in the velocity profile itself. It is not laminar, and it overestimates the u+ (or Ux if I look at dimensional values).

Quote:
5) The vortex method (which is the method of choice in Fluent) requires mean vleocity and turbulent profiles at inlet. I don't understand your procedure to assign them. I would compute an Equilibrium B.L. solution with a Reynolds Stress Model and simply assign them to your inlet method.
Why do you need to do that twice?
I admit the method I used may be slightly more complicated than need be. It is the way that was suggested to me by my superiors as the method that had been used before. It seems to me that it should work ok, though yes I could do use a RSM and put the stresses in with the inlet BC. I run it twice because the RANS runs are not very time-intensive, though this is not needed I suppose.
amanbearpig is offline   Reply With Quote

Old   May 28, 2013, 13:51
Default
  #6
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 544
Blog Entries: 14
Rep Power: 18
sbaffini will become famous soon enough
Your settings are ok.

Do you recognize any of your problems in the results in the paper below:

http://www.lamc.ing.unibo.it/aimeta2.../MEM-273-0.pdf

In that case it is just that LES is far from perfect, especially in Fluent
sbaffini is offline   Reply With Quote

Old   May 29, 2013, 11:41
Default
  #7
Member
 
Join Date: Apr 2011
Posts: 38
Rep Power: 7
amanbearpig is on a distinguished road
The results from that paper look remarkably like what I am seeing. My nondimensional velocity profile looks almost identical to theirs. I have switched my momentum scheme to the unbounded central differencing, and am seeing an improvement - though not perfect - as well.

Do you happen to know if the future investigations into the pressure interpolation schemes mentioned in the paper yielded any information? As I said above I have been using Body Force Weighted, but wonder if trying Second Order might be helpful? Thank you very much, you have been very helpful sbaffini!
amanbearpig is offline   Reply With Quote

Old   May 29, 2013, 12:40
Default
  #8
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 544
Blog Entries: 14
Rep Power: 18
sbaffini will become famous soon enough
The investigations were actually done but i don't have a paper. The result is that PRESTO is to prefer over a second order scheme. Less rigorous tests led to the same conclusions for the standard and linear schemes. Sadly i have no info on the Body force weighted but, according to my experience, it is very similar to the PRESTO! scheme and i do not expect significant differences among the two.

Notice, however, that the main conclusion of the test above was not based on the mean velocity profile but on velocity fluctuations and the relative spectra, which were strongly and badly affected. The mean velocity profile was actually better in terms of overall agreement with the DNS one but, still, the velocity profile was much more a boundary layer one than a channel one, with a sort of potential zone in the middle of the channel (which is clearly wrong).
sbaffini is offline   Reply With Quote

Old   June 25, 2014, 03:59
Unhappy Alternate URL for Paolo's paper?
  #9
New Member
 
Alan Belle
Join Date: Feb 2014
Posts: 1
Rep Power: 0
abelle is on a distinguished road
Quote:
Originally Posted by sbaffini View Post
Do you have a new link to your paper Paolo? This one seems dead, and I would really like to read it.
abelle is offline   Reply With Quote

Old   June 25, 2014, 05:22
Default
  #10
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 544
Blog Entries: 14
Rep Power: 18
sbaffini will become famous soon enough
Dear Alan,

i have no idea why the link is gone (thanks for the information). At the moment i have no access to my laptop, but i will post the paper here (possibly in my blog page on this site) as soon as possible. However, consider reading my Ph.D. thesis (still in the blog). Chapter 6 should have all the information contained in the AIMETA paper (actually there is much more than that).

Regards
sbaffini is offline   Reply With Quote

Old   March 31, 2016, 05:00
Default
  #11
New Member
 
Join Date: Dec 2015
Posts: 9
Rep Power: 2
Cfdbug is on a distinguished road
http://www.lamc.ing.unibo.it/aimeta2.../MEM-273-0.pdf



Do you have a new link to your paper Paolo? This one seems dead, and I would really like to read it.

Sorry,but i cant find the link in your blog.could you please give me a new link to the paper ?
Cfdbug is offline   Reply With Quote

Old   March 31, 2016, 05:15
Default
  #12
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 544
Blog Entries: 14
Rep Power: 18
sbaffini will become famous soon enough
If you search for the paper:

Sensitivity Analysis on Numerical Parameters for Large Eddy Simulation with an Unstructured Finite Volume Commercial Code

you will find it both under google scholar or researchgate directly. However, the comment on the thesis is still valid.

Best regards
sbaffini is offline   Reply With Quote

Old   April 4, 2016, 10:02
Default
  #13
New Member
 
Join Date: Dec 2015
Posts: 9
Rep Power: 2
Cfdbug is on a distinguished road
Thank you so much! Good luck!
Cfdbug 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
UDF error - parabolic velocity profile - 3D turbine Zaqie Fluent UDF and Scheme Programming 9 June 25, 2016 19:08
Scale discrete inlet velocity profile with groovyBC cboss OpenFOAM 1 June 20, 2010 13:02
[boundary condition] logarithmic velocity profile cfdworker FLUENT 2 April 17, 2009 23:36
Velocity Profile Jeff FLUENT 1 November 24, 2008 09:21
Prescribed inflow velocity profile - how to? Alan Main CFD Forum 10 October 28, 2005 12:14


All times are GMT -4. The time now is 06:45.