Problem with convergence
Hello, I'm trying to simulate the flow around NACA0012 airfoil. It is a simple incompressible viscous case without separations, to be more clear the configuration file is attached below.
I also attach the convergence history; regarding the plot I have two questions:
Please note that in these two points the CFL(=2) isn't changing.
Thank you very much in advance.
As far I see in the config file, you are running the compressible solver.
With respect to the parameters this is my recommendation.
Remember that FREESTREAM_PRESSURE is computed by the code for viscous flows!
With the values below the non-dimensional temperature, density and pressure will be 1.0:
It is better to use an upwind scheme to deal with viscous flows
If your convergence stall then, reduce the value of the LIMITER_COEFF
Remember that the NASA validation has been done with a 230529 points grid, this is 5x finer than the grid that you are using.
To start with, it is always a good idea to switch off the MG
We have done an extensive V&V of the compressible solver (described in http://su2.stanford.edu/documents/SU2_AIAA_ASM2013.pdf ) but the incompressible solver is in a V&V stage, you are very welcome to contribute (first Euler, then Laminar NS, and finally RANS).
Thank you for your reply.
In these days I tested different settings.
Do you have some advice to find a better configuration of MG technique? For my tests I considered config files of tutorials as a reference, but the solution becomes not stable.
Now I have a fair solution, but the same config file, on the same mesh, gives different results if run in parallel or serial. Have you ever experienced the same problem before?
Thank you very much,
Just a couple of notes on finding a good set of parameters for multigrid (it can be a bit of an art):
A 'W' cycle will be more expensive per multigrid iteration, but in general should provide the best overall convergence acceleration. If you are having trouble keeping stability, try a 'V' cycle too.
The number of levels that one should use is largely dependent on the individual mesh, as the agglomeration should produce successive coarser mesh levels that have 'good' agglomeration rates. Depending on the element type, the agglomeration rates should in general be in the 1/3-1/8 range for better quality. If an agglomerated rate for a coarse level approaches 1/1, it will not be as effective. Creating appropriately sized levels is important for the multigrid algorithm (the idea is to damp high and low frequency oscillations in the solution by using the residuals computed on the various fine and coarse meshes to form a better update). The agglomeration rates are printed to the screen during the preprocessing during a run of SU2_CFD. For instance, the following is printed for the inviscid NACA 0012 test case:
CVs of the MG level: 1533. Agglom. rate 1/3.41357. MG level: 1.
CVs of the MG level: 457. Agglom. rate 1/3.35449. MG level: 2.
CVs of the MG level: 166. Agglom. rate 1/2.75301. MG level: 3.
There are two parameters in the config file that give the user some control over the agglomeration process:
% Maximum number of children in the agglomeration stage
% Maximum length of an agglomerated element (relative to the domain)
By modifying these inputs, the agglomeration rates can be influenced, which can help create higher quality coarse mesh levels.
Hope this helps!
I thank you very much for the exhaustive clarification to my question and I would like to apologize for my late reply, I was testing different settings to activate multigrid strategy.
Unfortunately, I was not able to reach a converged solution because it appears to become unstable using 3 MG levels (an example is attached below) either with W cycle or V cycle. Now I'm trying to decrease the number of MG levels in order to reach the solution.
However, is it possible that I can obtain a more stable behaviour by setting appropriately pre/post-smoothing level? Are there some hints to find the best setting?
|All times are GMT -4. The time now is 16:30.|