[joey-mastlab]

Here are some images of the progress so far. I don't understand why the streamlines look like this. I feel like something is clearly wrong.

Screenshot 2023-09-26 100358.png

Screenshot 2023-09-26 203415.png

[ghorrocks]

Streamlines can be misleading on transient simulations. I only use streamlines on steady state simulations. So I would not plot them. The volume fraction cross section and velocity vectors are much more useful.

My assessment of your image is that so far it is looking good. The water surface has remained sharp, and the lump in the water surface is a surface wave caused by the flow suddenly starting up. This is all physically believable, so I think things are good so far. I would let that simulation continue.

[Gert-Jan]

In postprocessing a multiphase calculation, better use streamlines based on the Superficial Velocity (Velocity*Volume Fraction) instead of Velocity.

[joey-mastlab]

Hello I hope you had a good weekend. After some trial and error, I was able to get the simulation to run smoothly. This morning when I checked though, it had stopped because my PC ran out of storage. I transferred the previous backups to an SSD and I got it going again. Here are images of the residuals and the volume fraction at iteration 570. Let me know your thoughts.
Screenshot 2023-10-01 at 11.27.44 AM.jpg

Screenshot 2023-10-01 at 11.30.15 AM.jpg

[ghorrocks]

That looks like it is working as intended (or at least as I understood it). The free surface is being resolved well and not blurring too much, the air is doing sensible things and it appears to be converging each time step.

From your first post you showed that there is a test section and port where the air bubble is currently trapped. I understand you made it a wall for this preliminary simulation. I bet if you made it back to an opening again then it would have convergence problems (feel free to try this).

Can you explain to me what happens in the actual device when water goes into the test section and port?

[joey-mastlab]

Originally Posted by ghorrocks

Can you explain to me what happens in the actual device when water goes into the test section and port?

The test section will have very straight flow and have a velocity of around 3.5 m/s. The port will be used just for ventilation so any air that gets sucked in won't create a pressure difference.

[ghorrocks]

But your last image shows that fluid will go up the test section, at least in the start up transient. So this is not a good place to put the boundary, you should put it higher up where the water will never reach it. Then you can make it an opening and it should not cause convergence issues. The same goes for the port.

[joey-mastlab]

Ive already raised the port and that seems to be fine so far. I will have to make the test section opening higher in the next simulation to see how much higher it will rise up.

[ghorrocks]

OK, post some images of it when you have something to show.

[joey-mastlab]

I have started a new simulation with a higher test section. The port and test section are still blocked off as I want to make sure no water touches it before I open them up. Here is an image of the volume fraction for iteration 50 and the corresponding residuals.
Screenshot 2023-10-04 at 9.23.07 PM.jpg

Screenshot 2023-10-04 at 9.26.32 PM.jpg

[ghorrocks]

I see some spots of VF in the air region, and your free surface has some strange kinks in it. I did not see that in your previous images. This might be a problem - do you have any idea what is happening there?

Also I note you are using the segregated VF solver. This simulation might run better with the coupled volume fraction solver. You can activate that is the solver options tab in CFX-Pre. Do a test run to see if it helps (sometimes it helps a lot and sometimes it is worse, you need to try it and see in your specific case).

[joey-mastlab]

I saw those weird spots too. My thoughts are that: 1) maybe its a convergence issue since this is so early in the start up of the simulation, or 2) when I specified the VF initial conditions, I set it so the water level will be touching the top of the diffuser before the test section. In the previous simulation, there was an air gap there as can be seen in the images from that model (the green section at the top of the diffuser). Those are my two thoughts as of right now. I'm going to let this run until the morning (about 10 more hours) and see how it's progressed before I make any changes regarding the coupled VF vs. the segregated VF. This will also let me compare the two types of solvers. Let me know your thoughts.

[ghorrocks]

Yes, let that run and see how it goes. Try the coupled vs segregated VF solver tomorrow regardless of what the results are.

[joey-mastlab]

Here is the image from timestep 500. There is something still weird going on with the free surface. I'm taking a break from the free surface simulation and I am going to work on making some changes to the closed section model. I will be back though within a week or two!

Screenshot 2023-10-06 085451.png

[ghorrocks]

Yes, definitely weird. I suspect a convergence problem, try a tighter convergence tolerance and/or the coupled VF solver.

Also - are you running double precision. That will help as well, but slow the solver down a bit.

[Gert-Jan]

Originally Posted by joey-mastlab

It is a homogeneous model. Here is an image of my mesh.
I accidentally didn't save the last run so I don't have the output file. I'm rerunning it now so I will post it tomorrow.

Attachment 96342

If you still use a mesh like in your query of september 25, I recommend to spend a more time on your meshing approach. When solving a free surface problem like yours, I would never ever use a tet mesh since this gives a blur anyway. You should use hex elements. Given your geometry, I think this should be possible using a sweep mesh. ANSYS Workbench can do this.

[joey-mastlab]

Hello,
I've resumed working on the free surface model of the flow tunnel, but I'm encountering persistent issues with the air/water surface during the simulation.

Here are some of the steps that I’ve taken:

• To reduce the computation time required to approach one full convection time step, eliminated the wall inflation layers and set free-slip boundaries on all walls, which cut the mesh size by an order of magnitude. My reasoning was that an approximated solution using a coarse mesh would be a better initial condition for the finer mesh (at least compared to zero velocity).
• On startup, I was getting chaotic waves at the free surface. I reduced the inlet velocity from 1.55m/s to 0.005m/s to minimize the impulsive start-up and check that buoyancy is actually behaving like expected.
• The buoyancy model doesn’t seem to be working, even with very low inlet velocities. I get an instability at the free surface that develops into large-scale mixing. For kicks, I tried changing the sign on gravitational acceleration and there was no significant change in the results.
• I've conducted two scenarios using water (997 kg/m^3) and air (1.23 kg/m^3) densities as the reference density, but neither of them seems to improve the results.

I've included screenshots and OUT files corresponding to these scenarios for your reference. Hopefully you have some insights on what could be causing these issues and some recommendations.