[james.conger]

I have been using simpleFoam to simulate 2D turbulent air flow over sails. This works well for cases where the air flow is roughly parallel to the airfoil (sail) shape. The solutions typically converge in under 2000 iterations.

In cases where the sail is fully stalled (sailing downwind) the solutions oscillate over a period of ~800 iterations. The oscillations are periodic and continue indefinitely. This appears to roughly mimic the real-world situation where vortex shedding creates oscillations when sailing downwind. In other words, I suspect that the long period oscillations are a reflection of reality to some extent.

For my purposes I am interested in the average behavior. I would be interested in what approaches other people have taken in dealing with this type of meta-stable behavior.

A movie of the velocity profile over time and a plot of the oscillations is available at:

https://sites.google.com/site/sailcf...-visualization

[jherb]

A computational expensive solution would be to do transient simulations (with pimpleFoam). The simulation should converge for every time step. Then you can average over the converged solutions of the time steps.

Perhaps also the fixedMeanValue boundary condition for pressure does help:
http://www.cfd-online.com/Forums/ope...tml#post418371
http://www.cfd-online.com/Forums/ope...tml#post477560

[james.conger]

I had overlooked that mean value boundary condition. Certainly worth a test.

Many thanks!

[james.conger]

Surprisingly enough, it turns out that 3D simulations under the same conditions usually converge quickly without showing the oscillations. The 3D simpleFoam results show a large eddy behind the stalled sails (downwind simulations) with a complex flow pattern. This Reynolds averaged result is nice to work with and so far correlates with real data taken from the test boat.

I would be interested if other people have seen cases which are easier to get to converge in 3D vs 2D.

Partial summary of 3D results at:

https://sites.google.com/site/sailcf...3d-close-reach

[joegi.geo]

Hi, I will give you my two cents. That behavior is simply an indication of a highly unsteady flow, so the steady solver have problems getting to a converge solution.


In 3d you get to a converge solution because of the diffusion due to the coarse mesh. I bet that your 2d mesh is very fine so that one resolves better the spatial scales (it captures the unsteadiness). If you use a coarser mesh in 2d you will get to a converge solution as well. Also, if you use a very fine mesh in 3d you will see that you wont get a converge solution.



You can try to reduce the relaxation factors, maybe you are using the standard values (p=0.3, U=0.7), try to reduce U (an the turbulence variables) to 0.5.


Maybe after getting the steady solution, it can be a good idea to change to an unsteady solver and let the simulation run for a few seconds.




jg

[james.conger]

Thanks for your suggestions. You are right that on average there was a finer resolution on the 2D mesh. Also, I made the 3D mesh much more uniform, which might have contributed to the solution.

Note that we have taken a movie of a line of streamers held in the eddy region of the real boat and it certainly demonstrates that things are chaotic (as expected.)

I will have to go to a non steady state solution in the future to deal with wave motion, so I can experiment with that idea too.

Thanks again.