CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Issue at the air-water interface

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 4, 2020, 02:19
Default Issue at the air-water interface
  #1
New Member
 
Manoj Kumar Gangadharan
Join Date: Apr 2015
Location: Delaware, USA
Posts: 8
Rep Power: 9
manojkg.me is on a distinguished road
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?
Attached Images
File Type: png stage1.png (17.1 KB, 13 views)
File Type: png stage2.png (14.9 KB, 12 views)
File Type: png stage6.png (18.9 KB, 14 views)
manojkg.me is offline   Reply With Quote

Old   September 4, 2020, 05:50
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,263
Rep Power: 136
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   September 4, 2020, 06:06
Smile
  #3
New Member
 
Manoj Kumar Gangadharan
Join Date: Apr 2015
Location: Delaware, USA
Posts: 8
Rep Power: 9
manojkg.me is on a distinguished road
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.
manojkg.me is offline   Reply With Quote

Old   September 4, 2020, 23:46
Default Updates
  #4
New Member
 
Manoj Kumar Gangadharan
Join Date: Apr 2015
Location: Delaware, USA
Posts: 8
Rep Power: 9
manojkg.me is on a distinguished road
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.
Attached Images
File Type: png new_mesh_itr.png (28.8 KB, 10 views)
manojkg.me is offline   Reply With Quote

Reply

Tags
cfx, free surface flows, issues, multiphase

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water diffusion into air MGabr CFX 16 November 20, 2020 02:35
How to use a UDF to set the volume fraction in the cells next to a wall? DF15 Fluent UDF and Scheme Programming 33 August 20, 2020 14:36
Table bounds warnings at: END OF TIME STEP CFXer CFX 4 July 17, 2020 00:44
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
water and air interface boundary Shivakanth Main CFD Forum 2 September 25, 2008 10:11


All times are GMT -4. The time now is 20:44.