cavitation bubbles
 

Hello dear forum users;

I´m trying to simulate the bubble occuration with a transient simulation on cfx for a sonotrode which have 20kHz frequency and 40um displacement. My problem is whenever I simulate it I got irrelevant bubble points ( bubbles with isovolume above 0.15 vapor volume fraction). I don´t know where is the problem. Do I need extra formulas inserted for this type of analysis?:confused:

Thanks in advance

Have you looked at the FAQ on accuracy? https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Have you checked your mesh, time step and convergence are adequate to resolve the features you are looking for?

Hello
Yes I´ve checked these things you mentioned. My problem is the cavitation bubbles (determined by isovolume which states the volumes containing more than 0.05 vapor volume fraction) are only occuring on the surface which is vibrating, but normally with the real experiments there are also vapor bubbles away from the surface. In my analysis vapors don´t leave the surface.https://i.hizliresim.com/AkB1EX.png

You say you have checked mesh, time step and convergence but 95% of the time the problem is those factors - can you explain what you did to check them?

How many cycles of the motion have you run this for?

I checked the mesh with the mesh quality tool. I simply try to make a finer mesh around critical areas using sizing and other mesh tools, my goal was to improve mesh quality around these areas trying different methods.

My converge criteria was 1e-5 as suggested in manuals of this page.

Although I´m not sure about the time step. I made the analysis with 20 timesteps for every period. ( 1 sinusoidal wave )

For the mesh you need to consider both the quality and the resolution. Try a finer mesh.

20 time steps per period is unlikely to be enough.

For all these tunable parameters (mesh density, convergence tolerance, time step size) you should do a sensitivity analysis to set them correctly. If you guess you will invariably get it wrong and get unreliable results - like what you are reporting.

I left the analysis run for 15 cycles last night with a finer mesh, but again against the real experiment the vapor don´t leave the surface. Do I need another setup for this

Let me explain sensitivity studies.....

You do a simulation and get a result. Then you change the parameter of interest, let's say that is mesh size. You must do a change big enough to be significant - for mesh size that would be halving the edge length (which will result in around 8 times as many nodes, so a much bigger mesh). So make a new mesh with half the element edge length and do the simulation again. Compare the results to the first simulation.

If the results are the same within a tolerance you are happy with then you have found an adequate mesh size and can proceed. If the results are different then you must refine the mesh again, halving the element edge length again and continue until you do obtain results close enough for your purposes.

For convergence tolerance each step should be a factor of 10, for time step each step should be a factor of 2. But a short cut is to use adaptive time stepping homing in on 3-5 coeff loops per iteration. That will find a good time step by itself.

If you start by finding a good mesh size with a guessed convergence tolerance and time step size, then you need to check the convergence tolerance and time step size. This may mean you original mesh is no longer adequate - so you need to repeat the mesh sensitivity study to check the mesh is OK.

You can see this can be an iterative process, and can be time consuming especially for complex models. But unless you do it you have no idea if your answers are accurate or not - and if you just guessed the parameters they are almost certainly totally wrong.

Is solving the problem multiple times take too much time? Since only one takes nearly 3-5 hours to complete.

That's why people do CFD on supercomputers. It's up to you - either do it properly and it will take a bit of time and effort, or cut corners and get rubbish results.