[MadsR]

Hi Felix,

sorry for the late reply and thanks a bunch for your kind and fast help. I know that José is working on it, using your suggestions, and we will report back with the outcome.

Thanks again,
Mads

[jms]

Hi Felix,

As Mads just said sorry for being so late to give you an answer.
What I had wrong was the fvSolution file. Some of the tolerances were quite high that OF could not solve the equations correct and this is why it was taking so long time.
Furthermore, since the equations are solved better I don´t have this strange behavior on the drag curve for the NACA0012 I sent to you some time ago.

Thank you very much for all your help. It has really helped for the work I am doing in the thesis.

Best regards,

José

[FelixL]

Hello, José,


I'm glad to hear that your problem is solved and I could be of help. Feel free to ask anytime when there are new problems showing up (but which I really hope they don't).

Good luck with your thesis!


Greetings,
Felix.

[jordi.muela]

Hi everyone,

I'm validating a model to use it for find the Cd values of different geometries at different Re. Now I'm using a sphere due that is a geometry with a lot of experimental data.

I'm having similar problems to those mentioned in this thread, so please, can someone post the files fvSolution and fvSchemes which works fine?

I already tested all the suggestions explained in this thread but i couldn't obtain a good solution yet, my p residual it's still to high (and velocity residuals too...)

Thanks a lot,

Jordi.

[jms]

Hi Jordi,

I post the fvSolution and fvSchemes files which work fine for what I am doing (flow around an airfoil). What it really helped to me when I had convergence issues is to decrease the tolerance of all the residuals to a very low value (i.e. one value that none of them is getting -->1e-16).
But, what do you consider high for the residuals? I am getting residuals for the pressure equation around 1e-4. And the time of the computations when the airfoil is in the stall region is still high.

If you get any new things regarding this thread, plesease, keep me/us posted.

Greetings,

José

[jordi.muela]

Hi Jose,

first of all thanks for your fast reply! Just now i'm running a case with komegaSST model and for the moment, the behaviour seem 'better' than my previous cases, where i used the realizableKE model (Take a look to this report: http://citeseerx.ist.psu.edu/viewdoc...=rep1&type=pdf).

Well, when my current simulation finish, then I test the 'fvSchemes' and 'fvSolution' that you attached and report here how it gone! (Now i'm using the 'fvSchemes' and 'fvSolution' files of the motorBike test case).

With realizableKE I obtained residuals for p arround 1e-2~1e-3 (very high values...) but my tolerance and relTol values were highs too (arround 1e-5~1e-6 for tolerance...), but if I switch this values for others lower then i have divergence problems...

Well, I'll keep you updated about my progress!

Jordi.

[jordi.muela]

Hi José,

after few simulations changing some parameters, turbulent model and mesh, I've arrived at the conclusion that my principal problem is the mesh.

Now i'm getting reasonable results with a mesh where I refined the wake zone. I'm getting this results with the realizableKE model, the kOmegaSST model isn't working much well for me... Although i'm still having residuls for p around 1e-2 ~ 1e-3 (and I'm worried about that, but the results seems to match reasonably with the experimental..)

Thanks a lot for your help!

Jordi.

[jms]

Dear all,

I have tried to improve the speed of the computations done. I am doing simulations around a 2D airfoil (NACA0012) at Re=3.000.000 using the turbulence model k-w SST and a mesh of 123.000 cells. I have tested how the convergence speed is modified by changing relTol (from fvSolution).
I have used relaxation factor for the pressure equation=0.2 and relaxation factor for the velocity equation=0.8 since I tested once for another airfoil and this is the best I got. You can see the fvSolution file used

I have tested it for relTol=0.001, relTol=0.01 and relTol=0.1, the cases converge in 5, 4 and 6 hours respectively. A case with the same mesh run with ANSYS CFX (using the double precission solver!) takes about 1 hour to converge.

I still have to try it using GAMG solver for the pressure equation and see if I can improve it more...

Doe anybody can give me any comment about this? Any improvement to this is very welcome!

Thanks.

Regards,

José

[aerothermal]

Hello All,

Have you (Mads, José, Felix and Jordi) solved the issue? Do you all have an update?
I am very interested to have the system files and/or the mesh itself.

Just for your information, I saw a huge difference in convergence between OF1.7.1 and OF1.6-ext. The latter had a much better convergence history/duration and result. It may be related to some differences in linear solvers implemented by Jasak and others from extended project.

See some preview of the results at the thread below:
http://www.cfd-online.com/Forums/ope...tml#post307393

Regards,

Guilherme da Silva - ATS4i

[MadsR]

Hi Guilherme da Silva,

we don't have any significant to add to the above, still OF is much slower (wall clock) than CFX 13 (and other codes I have tested) in terms of getting a final converged solution. Apart from that I am very happy with OpenFOAM 1.7.1 results on 2D airfoils (both normal thin ones and more exotic ones) with and without laminar-turbulent transition modelling (with, thanks to Felix).

Interesting information you have about the 1.7.1 and the 1.6-ext convergence difference, I wonder if 2.0 is better than 1.7.1, we haven't tested that yet, but maybe someone else did? There must be a lot of revisions since they went past 1.8 and 1.9 :-P

Please update us if you find more on this issue

BR
Mads

[FelixL]

Hello, All,


I too don't have anything new to add to the above. Unfortunately I didn't have had much time lately to work with OpenFOAM, but at least I managed to upgrade to 2.0 and test a few things.

I tried to reproduce the NASA NACA0012 validation test cases ( http://turbmodels.larc.nasa.gov/naca0012_val.html ) using the grids they provided. The cases ran well, but I'm unhappy with the results, because I'm not able to get into the asymptotic range with the force coefficients at alpha=0°. That kind of bothers me and I need to look deeper into it at some time, but for now you can have my systems directory - I don't think you'll find anything new there, though.

Originally Posted by MadsR

Interesting information you have about the 1.7.1 and the 1.6-ext convergence difference, I wonder if 2.0 is better than 1.7.1, we haven't tested that yet, but maybe someone else did? There must be a lot of revisions since they went past 1.8 and 1.9 :-P

I didn't notice any improvement performancewise. The new residual control, though, comes in very, very handy!


Greetings,
Felix

[FelixL]

Oh by the way, here's the system-Directory!

[KateEisenhower]

Hello all, and thank you for this very interesting dicussion.

Felix, what made you choose the SpalartAllmaras model? I thought I read somewhere it is better to choose the kOmegaSST model for high AoAs. Has someone compared these two?

Best regards,

Kate

Originally Posted by FelixL

Hello, Mads,


your OpenFOAM settings don't seem to be optimal to me. I've run airfoil configurations with slightly more complex configurations and grids and I didn't have such extreme convergence times. I used SpalartAllmaras most of the time though, but I don't think the choice of turbulence model would make such a huge difference in terms of convergence rate.

In my opinion, simple airfoil configurations (low AoA, incompressible, 100k-400k cells) should be reasonably converged within a few thousand iterations. But this of course depends upon a lot of things.

What do you use as a starting field? Running potentialFoam first usually accelerates convergence a lot. PCG for solving the pressure equation usually helped a lot for me too (instead of GAMG).

A look at your numerical setup in OpenFOAM would be great.


Greetings,
Felix.