Issue at the air-water interface
 

Hello,
I am performing a simulation involving free surface for simulating the interaction between wave and a rigid wall. At the very beginning of the simulation itself, I see formation of droplets on the air-water interface. Please see the attached figure. Will someone be able to point me in a direction so that I can figure out why this issue is happening?

Good to see you are looking at your results in detail. I have a lot of experience in this area, unfortunately.

First of all, make sure your simulation is converged. Rerun the simulation at a tighter convergence tolerance, use double precision, and possibly a smaller time step (if transient).

If you still get it after that then this looks like a spurious flow generated from the free surface model. This problem is inherent in the numerical approach you are currently using, so you cannot fix it by convergence or mesh. You need to adjust the free surface modelling parameters (smoothing, coupled vs segregated VF solver etc) to see what works in your case. Run a series of simulations where you adjust all the parameters one at a time until you find the parameter(s) which are important for this issue.

Thank you. I will run additional simulations based on your suggestions and update this thread in due course of time.
I am quite new to the simulation of free-surface flow using ANSYS CFX (I am code developer). And the last time I attempted a similar problem (back in 2015). I had a similar issue. The workaround I attempted was to restart the simulation from a previously stable state and run the simulation at a lower timestep or change the number of processors in a parallel run.
Another interesting observation was that this problem occurs only in a parallel run and not if the simulation is performed in a serial configuration. Back then, I didn't have more time, so I didn't spend much on the why questions.

In the present case, the situation occurs right within the first five timesteps and none of the workarounds I attempted would help me. Hence, decided to ask the community. Thank you for your reply. Even though sad, it gives me a little relief that there is something in there to explore and discover.

I will keep the thread updated. Thanks again.

Updates
 

I have worked on a few different versions of the same setup. The one thing I didn't mention in the initial post was that I was attempting to simulate a control volume and not the entire domain.
Hence

1. The boundary on the far right was supposed to be an open type boundary
2. You can either specify the mass flow rate, or pressure normal to the boundary

For the ease of performing simulation, I had defined the far right wall as a free slip wall. Even though this cause reflection within the system, the simulation duration was so small that the wave would not reach the far end during the simulated period (this was my justification).

The post-processing showed that this was not the case. So I have made changes to the boundary. Other changes as listed below were also made

1. A more refined mesh that has better resolution along the no slip walls was made.
2. The control of residual were brought down to 1E-5.
3. Increased the sub-cycling iteration time steps to make sure that the simulation is converged at every time step.

In the present state, I have set it up for 30 iterations, but in the new mesh, the simulation is converging within 12-14 time steps. (Please see the attachment).
The simulation is currently in progress, but I am happy to report that the whole bubble forming issue no longer exist.

Thank your all the tips and providing me a little hope and faith. I will update the thread once I am done with the simulation.