[joey-mastlab]

Hello all,

I am working on a problem that simulates a new water tunnel my lab is going to build. It will have the capability of the test section being fully enclosed and open to atmosphere. The part that I am struggling with is the simulation that has the open test section.

When I set up the problem, I have always set the outlet as an Outlet in the setup. The solver gives me an error that the outlet is 100% blocked for air and water. I then set it as an opening and now my solution won't converge.

I have attached images of everything, feel free to ask more questions if need be. I hope you all can help me
Screenshot 2023-09-07 093254.jpg

Screenshot 2023-09-07 091802.jpg

Screenshot 2023-09-07 093317.png

[ghorrocks]

Your attachments were not uploaded correctly. This FAQ might help: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

Before we go into you model, what are you trying to do here?

Do you want the free surface detail? Or can we simplify it and just use a pressure boundary for the free surface? If we simplify it that will make this a single phase model and much simpler.

What are you trying to get out of this simulation? How even the flow is in the test section? The load on the pumps? What the free surface does? Or something else?

[joey-mastlab]

Originally Posted by ghorrocks

Your attachments were not uploaded correctly. This FAQ might help: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

Before we go into you model, what are you trying to do here?

I am trying to see how the flow behaves in the test section and more importantly, how much air gets pulled into the outlet (where the pump will be).

I'll work on updating the attachments also.

[ghorrocks]

OK, thanks. That will be a bit tricky as you have a wide range of length scale (from metres in the geometry to mm in the bubbles being pulled down into the pump).

I would recommend:
1) Extending your air riser higher so the water level never gets near it. The boundary condition is much simpler if it only a single phase.
2) This model will have to be a multiphase model to capture those effects. You will need a free surface model.
3) I am not sure whether you want a homogeneous or inhomogenous free surface model. Homogeneous would mean your explicitly model all bubbles and that would be challenging due to the size range, so I think an inhomogeneous model would be better as that can use a bubble model for the small bubbles but still model the free surface.
4) I am pretty sure you do not want surface tension for this. It will make it much more difficult if you use it.

Please upload your output file.

[joey-mastlab]

I do know this is a tricky simulation. I don't exactly want to model the bubbles per say, I'm more interested in the volume fraction of air that will be pulled into the pump (outlet). Surface tension doesn't matter in this simulation.

My current results file doesnt look like the image I attached, ive been trying to make changes to get a proper simulation. I added a hydrostatic pressure boundary condition on the outlet (it used to be 0 Pa but now I accounted for the hydrostatic pressure).

I cannot attach my results file cause its too large apparently. Do you know how I can do this?

Also I would like to thank you now for helping me. My advisor and I have been stuck on this problem for quite some time.

[ghorrocks]

I don't exactly want to model the bubbles per say, I'm more interested in the volume fraction of air that will be pulled into the pump (outlet).

The bubbles are what changes the volume fraction. So don't you have to model the bubbles?

Surface tension doesn't matter in this simulation.

Surface tension does matter for bubbles. Surface tension is what makes them become round.

I added a hydrostatic pressure boundary condition on the outlet (it used to be 0 Pa but now I accounted for the hydrostatic pressure).

Make sure you read the CFX documentation on hydrostatic pressure. You will probably find that the way you were doing it previously (just using 0Pa everywhere) is actually the correct approach as hydrostatic pressure is already taken care if you have set the reference density up correctly.

cannot attach my results file cause its too large apparently. Do you know how I can do this?

I requested the output file, not the result file. If the output file is too large then feel free to trim it down so it is small enough. If the output file contains thousands of iterations then just leave the first few and last few iterations.

Also I would like to thank you now for helping me.

Glad to help. I think we can get this simulation running, so post your progress and we will try to help.

[joey-mastlab]

I hope you had a good weekend.
I guess I do need to model the bubbles then, I've been mainly working with single phase simulations and mainly looking at streamlines and shear stress, which from what I can see don't inherently show bubbles. The reason why I set a hydrostatic pressure boundary is because I previously was setting the outlet pressure as 0 Pa but it wouldn't make sense to have the outlet at 0Pa (which the outlet is going into a pump) and the test section at 0Pa. I thought that may be causing some of the issues I'm having.
I've attached the output file(sorry about that, I thought you meant the results file).
Fluid Flow CFX_008.txt

[ghorrocks]

I see you are already using an inhomogeneous multiphase model. I suspect this is the most appropriate model, but it will depend on exactly what you are modelling.

You definitely need to make your riser higher and put an opening pressure boundary on it. It should be high enough that water never hits it, it should only ever see air.

You may need a surface tension model depending on exactly how air is brought to the pump. This is a detail you can probably look at later.

[joey-mastlab]

I have made my riser significantly larger, hopefully this will prevent fluid from touching the port. The pressure boundary condition I applied is 0 atm as I previously have. I have also applied a hydrostatic boundary condition of 0.464 atm on the outlet.

The reference density I am using is 997 kgm^3 (water) and the reference pressure is 1 atm. Is this correct for this type of simulation?

In regards to air being brought into the pump, I want to eliminate that as much as possibly, ideally no air would be brought into the pump.

I'm running the simulation now so I will make a reply when it finishes

[joey-mastlab]

My simulation is done and I have uploaded some images and the output file.
Screenshot 2023-09-12 201932.png

Screenshot 2023-09-12 202222.jpg

Fluid Flow CFX_001.txt

[ghorrocks]

The reference density I am using is 997 kgm^3 (water) and the reference pressure is 1 atm. Is this correct for this type of simulation?

See CFX Solver Modelling Guide, section 7.6. You probably want the reference density to be that of air, but in your case (which is almost all water and only a little bit of air) it might be better to stay with water setting the reference density.

As for your recent results, it did not converge very well and the streamlines show something is not working correctly. The flow is not going around your circuit at all.

I would recommend:
* Doing a first pass of this with some gross simplifications. Do a single phase water model with the open section at the test section and port blocked off with a wall. Make sure that the inlet and outlets are doing what you expect and the flow looks reasonable.
* Once that is working then do a homogeneous multiphase model (so no bubble model). This is the next level up in complexity (it is a big step up, however) as there are many new issues to sort out. Have a look at the free surface and see what it is doing - if it does not appear to be entrapping bubbles then this model could be your final result.
* Once a homogeneous model is working correctly and you have shown that it is entrapping bubbles then modify it to a inhomogeneous model.

I think you will find gradually adding the complexity will help in debugging this run.

[joey-mastlab]

From section 7.6, "For a flow containing a continuous phase and a dilute dispersed phase, you should set the buoyancy reference density to that of the continuous phase." I believe water in my case would be the continuous fluid, air can get trapped in the water so I believe that does make it my dispersed model.

Im going to run that simplified simulation now with the port blocked off. I will report back with the results.

[ghorrocks]

I believe water in my case would be the continuous fluid, air can get trapped in the water so I believe that does make it my dispersed model.

That only applies to the inhomogeneous approach. In the single phase and homogeneous approaches that does not apply so the decision would be made on other issues.

[joey-mastlab]

Here are some images and the output file from my most recent simulation where I placed a wall boundary over the port and left the test section open. It looks very similar to the previous simulation. I am running one now with a wall placed over the test section, this will hopefully look more like it did when I first started this project as this is very similar to how I started.

Screenshot 2023-09-13 211206.png

Screenshot 2023-09-13 211245.jpg

Fluid Flow CFX_001.txt

[ghorrocks]

There still seems to be a fundamental error in your simulation.

Did you see post #11? Here is the key bit:

I would recommend:
* Doing a first pass of this with some gross simplifications. Do a single phase water model with the open section at the test section and port blocked off with a wall. Make sure that the inlet and outlets are doing what you expect and the flow looks reasonable.
* Once that is working then do a homogeneous multiphase model (so no bubble model). This is the next level up in complexity (it is a big step up, however) as there are many new issues to sort out. Have a look at the free surface and see what it is doing - if it does not appear to be entrapping bubbles then this model could be your final result.
* Once a homogeneous model is working correctly and you have shown that it is entrapping bubbles then modify it to a inhomogeneous model.

I think you will find gradually adding the complexity will help in debugging this run.

You might have missed that the first simulation should be single phase.

[joey-mastlab]

Originally Posted by ghorrocks

You might have missed that the first simulation should be single phase.

I did miss that it should be single phase. I ran it with air and water as the fluids but the port blocked off. I will work on running a simulation without air, an open test section and a wall placed on the port.

The simulation I just ran had a wall placed on the test section and the port. It still never converged and something is still wrong.

Screenshot 2023-09-14 091125.jpg

[joey-mastlab]

Here is the single phase version of this simulation. It looks how I would mostly expect.
Screenshot 2023-09-14 130509.png

Screenshot 2023-09-14 130543.png

Fluid Flow CFX_003.txt

[cmharwood]

I've been working with Joey on this - the help is much appreciated. One of the things we've been struggling to understand is how to set the pressures at the outlet and openings.

With a reference density equal to that of liquid water, my understanding (from reading the solver theory manual) is that the hydrostatic pressure is negated in the liquid phase. We also placed the reference location at the outlet to ensure that 0Pa was the correct outlet pressure.

The vent at the top of the de-aerating chamber is less obvious. The theory manual suggests that we need to consider the equivalent hydrostatic pressure "deficit" in the gas phase. So, should the opening boundary at the top of the chamber be at a negative pressure?

[ghorrocks]

OK, the basic single phase model works OK. That means you have the basics working.

So I would now do a multiphase model, but a homogeneous one. This means there will only be one velocity field, so no interphase slip; but it will have a free surface. What does a homogeneous multiphase result look like? I would also recommend making another simplification for the first try - block the vent off with a wall. We will look at vent boundary condition once the basic flow is working.

With a reference density equal to that of liquid water, my understanding (from reading the solver theory manual) is that the hydrostatic pressure is negated in the liquid phase.

For the variable "pressure" this is correct. The variable "absolute pressure" contains all contributions and you will see the hydrostatic head in that one.

The theory manual suggests that we need to consider the equivalent hydrostatic pressure "deficit" in the gas phase. So, should the opening boundary at the top of the chamber be at a negative pressure?

Yes, that is correct.

[joey-mastlab]

Originally Posted by ghorrocks

What does a homogeneous multiphase result look like? I would also recommend making another simplification for the first try - block the vent off with a wall. We will look at vent boundary condition once the basic flow is working
.

Here is an image of the homogeneous multiphase simulation with the port blocked off and a -45kpa pressure placed on the test section. I also ran a simulation with the test section blocked off and a -60 kpa pressure placed on the port.
The first image is the open test section.

-45kpa_test_section.jpg

-60kpa_port.jpg