|
[Sponsors] |
November 25, 2013, 21:00 |
LES for flow over bluff body
|
#1 |
New Member
Join Date: Apr 2010
Location: Athens, Greece
Posts: 15
Rep Power: 16 |
Hi all.
I would like to ask 2 things Should I run a steady state simulation and use the steady state solution as the initialization for the transient (either way) LES or could i omit the steady state run? I know this is more a question related to the transient analysis and not LES itself but is there any difference in LES? Its the first time i do a LES and i am using CFX. The simulation is about the airflow around a bluff body - something like a windbreak. It is supposed to be inside a wind tunnel. Usually i choose 30s as total time and 0.01s for the timestep size so its 3000 timesteps. I set the convergence at 10-4 RMS. Initially i do not get convergence in 3-5 loops as the cfx manual says. But quickly i do see convergence. Should i use more timesteps in order to have converged solutions in every timestep or could I just ignore the early non-converged ones? |
|
November 25, 2013, 21:52 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
If you only care about the pseudo-steady state flow then anything you can do to make the initial condition closer to the final flow will mean you do not need to run as long. As yes, starting from a steady state result will help.
If you do not care about the start up transient then don't worry about the initial time steps. If the start up is important then yes, you better fix that up. But you should consider using adaptive time stepping to automatically adjust the time steps. Be careful with LES though, sometimes the time step size always keeps moving with adaptive timesteps and that is not good. Also second order time differencing suffers when the time step size changes a lot. So if you know the time step size then it might be better to define a fixed step size. |
|
November 26, 2013, 06:06 |
|
#3 |
New Member
Join Date: Apr 2010
Location: Athens, Greece
Posts: 15
Rep Power: 16 |
Thanks a lot Glenn.
Oh one more thing. So i am finally doing both. Two different configurations that the initial values for the transient - 2nd configuration- are taken by the converged steady state solution -1st configuration. I read at the fluent manual that before running LES you should "use the solve/initialize/ init-instantaneous-vel text command to generate the instantaneous velocity field out of the steady-state RANS results". Do i need to do something similar in CFX? I don't remember any option like that...(or i don't know how to do it) Last edited by sosat1012; November 26, 2013 at 09:02. |
|
November 26, 2013, 16:53 |
|
#4 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
I don't think CFX has an equivalent option. You will just have to run it for a while and let the turbulent structures generate.
|
|
November 27, 2013, 02:45 |
|
#5 |
Senior Member
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22 |
Under 'Expert parameters/Physical Models/Turbulence Models' there is a setting: apply ic fluctuations for les.
Set it to true to apply random fluctuations to the initial results. |
|
November 27, 2013, 04:33 |
|
#6 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143 |
Thanks for the tip Lance. I have never used that option - does it work well?
|
|
November 27, 2013, 05:11 |
|
#7 |
Senior Member
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 22 |
Sort of. If I understand correctly it applies random fluctuations to the entire domain, and in my applications I have parts of the domain that are laminar. But it can be useful to kick-start the turbulence.
|
|
November 27, 2013, 06:43 |
|
#8 |
New Member
Join Date: Apr 2010
Location: Athens, Greece
Posts: 15
Rep Power: 16 |
Yes i read it too in cfx manual. I did my first run without initial fluctuation and going to check my results in a couple of hours. I will run it again with initialization in fluctuations and compare. Thank you both guys!
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ANSYS Meshing] Simple Symmetry Mesh Question - Flow around Bluff Body | Matlab69 | ANSYS Meshing & Geometry | 20 | April 23, 2012 09:55 |
Bluff body used for diffuser testing | lemat1 | Siemens | 0 | December 5, 2009 09:11 |
LES simulation of bluff body at Re(d)=1200 | arash_nl | FLUENT | 0 | June 1, 2009 13:16 |
3d mesh of bluff body for LES | Lukasz Mosakowski | FLUENT | 4 | January 17, 2006 23:09 |
UDF for lift force on a bluff body | sawa | FLUENT | 2 | April 11, 2005 03:06 |