
[Sponsors] 
March 26, 2004, 18:01 
L2 norm

#1 
Guest
Posts: n/a

hi there,
Let's say I am modelling something with complicated flow structures (for example with flow seperation). Is it true that for this type of analysis, with the presence of flow seperation, the residuals at that zone is going to be much larger than the average, consequently "blowing up the L2 norm". And because of this, when inspecting whether a converged solution is reached, we can't rely on the residuals monitor by itself cos it is pretty dificult to get residuals down below 1e3  1e6. Am I right? My thought on this is (please correct me if I were wrong) we need to look at, let's say the force or moment values vs iterations, also average velocity and pressure etc. is no longer changing and conservation of mass at boundary etc, to determine if indeed a converged solution is reached. Am I still missing something? The reason of this post is right now I am modeling a half airplane at transonic speed (cut along the XZ plane), and there are sepration zone somewhere, supersonic flow somewhere in the domain, and the L2 norm of u,v,w, etc. are really high (1e3  1e5). My feeling is there is no way I can trust this result with such a high L2 norm. But even with a much finer mesh, I am seeing no reduction to L2 norm. I know I am not expecting something like 1e6, but L2 norm bigger than 1e0 sure spells trouble. What should I do? Please help! Thanks alot!!! 

March 26, 2004, 23:48 
Re: L2 norm

#2 
Guest
Posts: n/a

Since your configuration is quite complicated, complex flowfield tends to be unsteady, altogether make things hard to juldge. But a ABC knowlege in numerics and CFD must take L2 norm to drop to some accepteble level for trusting the simulation. how many orders of magnitude has been reduced from initial flowfield ? 1) are you solve NS or Euler equations? 2) have you validate your solver in other simpler case ? 3) Has other peple computed similar config. how about their L2norm?


March 29, 2004, 21:13 
Re: L2 norm

#3 
Guest
Posts: n/a

Have you tried simply putting in some monitor points in the areas of concern?


March 30, 2004, 10:47 
Re: L2 norm

#4 
Guest
Posts: n/a

Hi Guys, thanks for the response.
To simplify the model even more, the model now only contains a fuselage, pylon and nacelle. I have removed the wing to further simplify the flow field. Currently, the L2 norm for u, v, w, P, TKE, TED are 4.2e2, 1.2e1, 1.4e1, 1.4e1, 7.6e2, and 3.1e6 respectively. In my first post, I mentioned that I am suspecting the L2 norm is "blown up" due to some excessively high residuals at some particular locations. Therefore I also plot ave residuals. Results show my ave residual (of the entire domain) for u, v, w, P, TKE, TED are 1.8e1, 4.9e3, 6.1e3, N.A. (too bad), 2.8e1, 5.9e1, all of these average residuals are much smaller compared to L2 norm values. I also calculate the ratio of max residual to L2 norm. The ratio for the TED is about 98%, which confirms my worry that indeed the TED L2 norm is blown up due to maybe one node with excessively high residual. The ratio for u, v, w, P(Not available), and TKE are around 10%. Too bad the code I am using cannot tell me at what location which those max residuals come from. FYI, I am solving NS equation (compressible as M inf = 0.7). The code I am using is CFdesign. I can setup some monitor points in the domain while it is running. But I still can't get the residuals at those locations. I can only get the u,v,w,p,tke,ted values at those specified locations. I have similar analysis (low subsonic) before on a different airplanes, and the L2 norm of u,v,w,P, tke,ted are of the order of 1e2, 1e2, 1e2, 1e4, 1e0, 1e3, and the ave residuals are much lower. Any other suggestions guys? Thanks alot!! 

March 31, 2004, 00:27 
Re: L2 norm

#5 
Guest
Posts: n/a

Look at your monitor points to see if the u,v,w,p etc. variables stabilize to a certain value  you do not directly monitor the residuals at monitor points usually.
Output you results at intermittent timesteps. Look at your results as they converge. If you are getting bad max residuals in a few cells then the values of variables such as pressure in that location are likely to be a bit suspect. You might want to consider using isosurfaces to locate the maximum pressure or density. You might then find you have a very high, nonphysical value in only one or two cells  isosurfaces will help you identify the location quickly. Are you using an unstructured, hybrid or multiblock mesh? Either way you might also consider checking the aspect ratio's of your elements particularly in the region where you are not converging. If you are using tetrahedral elements, then look at the skew and face angle type criteria for cell distortion. If the elements are bad in some areas you should consider remeshing or smoothing the mesh locally. Lastly, transonic flow can be a pain in the butt to converge due to the inherently unstable nature of the flow. Is it possible that your flow might want to form a shock in an area of the flow where there is some speed up of the flow and an accompanying drop in pressure? Shock thickness is normally three or more cells and if you don't have enough cells where the shock it trying to form then you may get convergence difficulties such as you are experiencing. Hope this helps! 

March 31, 2004, 12:03 
Re: L2 norm

#6 
Guest
Posts: n/a

Thanks for all the advice.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
L1 norm in discontinuous Galerkin Method (DGM)  jinwon park  Main CFD Forum  1  August 7, 2008 14:50 
abt: L1 and L2 norm in FVM  jinwon parkq  Main CFD Forum  9  August 1, 2007 14:36 
Reduction in Residual Norm vs. Mesh Refinement  CFD Rookie  Main CFD Forum  5  January 28, 2004 11:45 
Which norm should I use?  Tony  Main CFD Forum  2  August 19, 2002 14:03 
How to get residual norm in an UDF ?  Anthony Wachs  FLUENT  0  October 25, 2001 08:22 