In 2D foil flow case, cavity generation using Fluent is possible. but, as iteration goes, the cavity grows, finally diverged. How can I converge the solution in this case ? After the cavity generaton, continuity was going to diverge. I think cavitation is not steady problem. (almost) So, hard to get steady(converged) solution. is there any criteria for cavitation problem, even if continuity is not converged ? Otherwise, I want to know right setting about that. Have a good day, all ~~

Hi!

Fluent cavitation model is a litle bit "special". You are right - to get a converged solution in steady case is a nightmare. The thing that helps is that you decrease termination criteria. Playing with underrelaxation doesn't really help a lot. The question is also which version of fluent you are using? The model in 6.1 is much better than in previous versions - but still very unstable... Why is the model "special" - the only possibility to get a well converged steady solution is to do unsteady solution and wait for it to becomes steady...you can imagine that it takes a while. In an unsteady case simulation you will have many problems with pressure reflections. The underrelaxation of pressure corection causes a pressure wave which travels trough your domain and is reflected a your inlet/outlet boundary conditions. That means that also unsteady solution is very hard to do...

You can also try the usual tricks for more stabe simulation...a good one in this case is to increase the velocity very slowly (in steps - 0, 1, 2, 5, 10 m/s) or decrease pressure until you reach the desired conditions.

Good luck with your work

MATEUS

Mateus,

I was very interested to read your reply to beginner. I have been struggling to get a steady state solution using the cavitation model for some time and hoped that things would improve with 6.1 but of course they didn't! What kind of time step do you recommend for the unsteady solver?

Many Thanks

Stuart

Hi!

It is generally considered to take about 100 time steps per 1 period (1 cavitation cloud separation or cloud pulsation). Frequencies of separation are very different for each case. In my case (I work mainly on simple hydrofoil) these frequencies are about 300Hz, what coresponds to time step 0.00002s - I still get good and stable simulation with time step 0.00005s, any longer time step leads to divergence. For other cases frequencies are: ventoury section (18 degrees confusor, 8 degrees difusor) 45Hz, NACA0012 - 15 Hz...As I said very different. Velocity and alngle of attack have also big influence here.

Generally Strouhal number lies between 0.15 and 0.4 - you can then calculate the frequency.

Regards

MATEUS

Sir you are a gentleman and a scholar. Thank you.

Stuart

Hello Mateus

Thanks for your contributions concerning the cavitation model in Fluent. In your explanation, you mention the problem of pressure reflections:

"In an unsteady case simulation you will have many problems with pressure reflections. The underrelaxation of pressure corection causes a pressure wave which travels trough your domain and is reflected a your inlet/outlet boundary conditions."

My questions: a) Can you describe shortly how the underrelaxation of the pressure correction causes a pressure wave? And b), how can a pressure wave travel through the domain, if the primary phase (liquid), which normaly takes up most part of the domain, is assumed to be incompressible (according to the limitations of the cavitation model)?

Hi!

If you simulate the dynamic behaviour of cavitation you will allways have a problem with the way you treat the bounary conditions and reflection on them. Even if you use an incompressible fluid you get the same problem because of the numerical speed of sound (underrelaxation of pressure correction).

I don't know why but this part of cavitation simulation (treatment of reflection) is usually not described in papers. There are few tricks that you can apply to solve the problem, but the only way to do it in Fluent (if you don't have source code) is to make a really long mesh...

If you simulate steady case you do not have this problem.

Regards

MATEUS

Thank you for your answer. Indeed, I am aware of the problem of unphysical pressure wave reflections at inlet/outlet boundaries. So far, I haven't seen a commercial code that addresses that issue in a proper way (I am speaking now explicitely for non-reflecting boundary conditions in connection with two-phase modelling). But I could imagine that e.g. in Fluent it should be somehow possible to write your own boundary condition via udf.

By the way: do you have some references concerning your statement "Even if you use an incompressible fluid you get the same problem because of the numerical speed of sound (underrelaxation of pressure correction)"?

Thank's in advance

Hi!

As I said - references are a big problem in this case. I've learned the most of it from notes from ex-collegue from our institute. He did write a PhD but it's in german and cavitation modelling and problems with it is just a very small part of it. You can download it at:

http://elib.tu-darmstadt.de/diss/000221/Diss_Habr_2.pdf

regards

MATEUS