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

Residual Oscillations

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 4, 2006, 06:57
Default Residual Oscillations
  #1
Cyril
Guest
 
Posts: n/a
I'm working on a bullet (Shock wave studies). I'm trying to find the best method to find a good model of the shock wave. I'm trying with inviscid, laminar and spalart allmaras. But in the 2 first cases, the residuals start to oscillate more or less, depending of the method. Could somebody help me to make theses residuals not to oscillate ??

You can see the mesh and the residuals here : http://img510.imageshack.us/img510/3...nstitre0up.jpg

Thanks !

P.S : If you have any suggestion about a model, or anything else... I'm very interested !

  Reply With Quote

Old   February 4, 2006, 18:33
Default Re: Residual Oscillations
  #2
Freeman
Guest
 
Posts: n/a
Hi Cyril,

It seems you have a problem very similar I had few weeks ago while simulating a 2D flow over a bluff body.

Your bullet hasn't an aerodynamic profile in its rear-end and your convergence problem may come from the fact that (in plain words) solver "finds" some kind of flow instability (e.g vortex shedding) that should be treated with the unsteady solver instead of the steady one.

As far as I know, Spallart-Almaras model is used more fore aerodynamic shapes, so in your case I would use at least the k-e Realizable model or so. Here it is the link with the threat I created with my problem: there's plenty of very good information regarding to models, discretization schemes and some reasons why 2D solver is more difficult to converge than 3D

http://www.cfd-online.com/Forum/fluent.cgi?read=35319

If after following these advices you don't fix the problem, I strongly recommend you to try solving your case in 3D.

I hope this help. Good luck!
  Reply With Quote

Old   February 6, 2006, 03:40
Default Re: Residual Oscillations
  #3
Cyril
Guest
 
Posts: n/a
Thank you very much for this. It helped me to understand well some aspects of numerical simulation.

The fact is that I'm finishing my studies, and I've never been taught about numerical calculus during my scholarship (engineering school), and some aspects of it are very difficult to get!

May I ask you an other question ? In your posts, you often talk about "first and second run"… Does it means that you "do" a first run, quick and unrefined, and then you start another one, more refined, based on the previous one ? How do you do this ?

Because for the project I'm working on (end of study project), I decided to run my calculus on the following scheme : 1-invicid, 2-laminar, 3-SA or k-e (std&hellip

Do you think that's a good idea ? (The purpose of my question, is that I can't find the same results with Fluent and {Whitham method and experimental tests results}). Factor 10 higher in Fluent !

Regards,

Cyril
  Reply With Quote

Old   February 6, 2006, 03:42
Default Re: Residual Oscillations
  #4
Cyril
Guest
 
Posts: n/a
Moreover, when I try to iterate with K-e Rzable, I've got a "turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 28 cells"... (I work with ideal gaz)

Do you think It could come from my boundaries conditions (Pressure far field and pressure outlet) ?
  Reply With Quote

Old   February 6, 2006, 14:32
Default Re: Residual Oscillations
  #5
Freeman
Guest
 
Posts: n/a
Hi again, let's see:

>>May I ask you an other question ? In your posts, you often talk about "first and second run"… Does it means that you "do" a first run, quick and unrefined, and then you start another one, more refined, based on the previous one ? How do you do this ?

It is common to do a first run with k-e std. and 1st order discretization schemes to get a "good" and easy first solution (k-e std+1st order is easy to converge). Then, after let's say 300 iterations I stop the iteration and I change settings (without initializing, of course) to k-e Rzble, non-eq wall func. and 2nd order upwind (better QUICK in your case because you've got quad. elements): then I iterate again until the convergence is reached.

>>Because for the project I'm working on (end of study project), I decided to run my calculus on the following scheme : 1-invicid, 2-laminar, 3-SA or k-e (std&hellip.Do you think that's a good idea ?

I haven't understand this very well: are you studying this 3 models separately or do you apply Inviscid, then switch to laminar and then k-e std.? If it is the former and your goal is to compare the 3 models, I don't think it is a bad idea. But your better k-e model should be Realizable at least (RSM is another world in my opinion: I thing it requires a high quality mesh to run well)

>>Moreover, when I try to iterate with K-e Rzable, I've got a "turbulent viscosity limited to viscosity ratio of 1.000000e+05 in 28 cells"... (I work with ideal gaz). Do you think It could come from my boundaries conditions (Pressure far field and pressure outlet)?

Maybe, and maybe not (what a reply xD). When I got this message was because my grid was not good enough and skewness was too high in regions with strong gradients: then I remesh my models accurately and now I get this message only during the few first iterations and then it desapears. I thing that if you start your iterations with the method I explained you above (start with k-e std, 1st order, std wall and then Rzble, QUICK, non-eq) probably this message would be "damped". You should also check your grid skewness and the boundary layer mesh over the bullet (fine enough). If my memory serves me well, the 3rd tutorial of Fluent is about Compressible Flows and the shock wave in an airfoil is computed: you may have a look at this if you haven't done it yet.

I hope this helps. See you!

Freeman
  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
transsonic nozzle with rhoSimpleFoam Unseen OpenFOAM Running, Solving & CFD 7 April 16, 2014 03:38
How to write k and epsilon before the abnormal end xiuying OpenFOAM Running, Solving & CFD 8 August 27, 2013 15:33
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM 6 April 12, 2011 11:24
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16


All times are GMT -4. The time now is 04:02.