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 1e-3 - 1e-6. 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 X-Z 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 1e-6, but L2 norm bigger than 1e0 sure spells trouble. What should I do?

Please help! Thanks alot!!!

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 N-S or Euler equations? 2) have you validate your solver in other simpler case ? 3) Has other peple computed similar config. how about their L2-norm?

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

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 1.8e-1, 4.9e-3, 6.1e-3, N.A. (too bad), 2.8e-1, 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 N-S 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 1e-2, 1e-2, 1e-2, 1e-4, 1e0, 1e3, and the ave residuals are much lower.

Any other suggestions guys?

Thanks alot!!

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, non-physical value in only one or two cells - isosurfaces will help you identify the location quickly.

Are you using an unstructured, hybrid or multi-block 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!

Thanks for all the advice.