[ghorrocks]

OK, the homogeneous multiphase model looks weird. So let's keep doing a homogeneous multiphase until it is working properly.

I would recommend:
* Make both the port and the test section walls. So repeat this model with the fluid just going from inlet to outlet and nowhere else to go.
* Post an image of your volume fraction initial condition (can you do this by saving a backup or results file at iteration number 0)
* And the volume fraction at the end of the simulation

For free surface models usually the most important variable to get right is the volume fraction. If the volume fraction is correct then everything else will not be too far off. So let's concentrate on getting the volume fraction correct for now.

[joey-mastlab]

Here are my results from the Homogeneous Multiphase simulation where the port and test section were blocked off. I think I attached the images of the volume faction that you requested. I also attached the output file.

Screenshot 2023-09-18 154522.png

Screenshot 2023-09-18 155024.png

last_interation.jpg

CFX_001 - Copy.txt

[ghorrocks]

No, you missed the most important ones. Please post an image of your volume fraction - both your initial condition and the final result. Something like a plane through the middle of the geometry, coloured by volume fraction would be good.

[joey-mastlab]

Ah I see, here's the volume factions for the inlet and outlet. I believe thats what you mean. If not correct me please.

Screenshot 2023-09-18 at 6.27.49 PM.jpg

[ghorrocks]

No, that is not what I need.

This image shows an example problem, coloured by the y location.

Screenshot.jpg

Please do an image like that, but colour it by volume fraction. One image for your initial condition, one for the final condition.

[joey-mastlab]

I believe this is what you are requesting. Im still confused what you mean by my initial condition and my final condition. This is a plane that's colored by the water volume fraction. Im sorry if that's still not what you are requesting. Thank you for patience with this.

Screenshot 2023-09-19 at 8.16.57 PM.jpg

[ghorrocks]

Yes, that is the final result view of volume fraction. That is one of the images I wanted to see.

That images shows that the bottom section is purely water (with a small amount of air at the top wall), but the top section has a swirling mass of air/water mix before becoming a thin sheet of water on the bottom with air above.

I am guessing that this is not even close to what you want the flow to look like So we need to fix your simulation up so that it correctly models the water surface.

Please post these images:
* Your volume fraction initial condition. This is the same image as this one, but your initial condition. You can get this by writing a results file at iteration zero.
* Can you please draw a hand drawing of what you want the flow to look like. Where do you want the water surface to be?

[joey-mastlab]

Im working on the hand drawing currently. How do I write a results file at iteration 0? In solver control, I changed Min. Iterations to 0 and Max. Iterations to 1, but it through an error

[joey-mastlab]

I believe this is at Iteration 1. I haven't found how to get iteration 0. Here is my hand drawing, I tried to annotate it the best I could (excuse my poor hand writing) Hopefully this makes sense what we are trying to ultimately accomplish.

Screenshot 2023-09-19 at 9.17.13 PM.jpg

Screenshot 2023-09-19 at 9.21.22 PM.jpg

[ghorrocks]

That's OK. Iteration 1 is close enough to the start. I can see you started it with air everywhere and the inlet pumping water in.

My suggestions:
* Define an initial condition with the free surface level at approximately the location you expect it to end up in. In this case, define it as water for z<[z location of your expected water surface level.
* Block the port and test section with a wall.
* Run that homogeneous multiphase. It should trap a bubble of air at the top. But I want to see if you can sharply resolve the interface if there is work we need to do on accuracy.

[joey-mastlab]

Where do I define that initial condition at? I tried initializing the the Water initial condition with a volume fraction of 1 but that didn't seem to help.

[ghorrocks]

No, you want to define an initial condition which is close to what you think the result should be. Something like this for a CEL expression for volume fraction initial condition: if(z<1[m],1,0) where z=1[m] is the free surface level.

Setting initial conditions is covered in the tutorials. You can do it either at the domain level or at the global level with a global initial condition.

[joey-mastlab]

I was able to set an initial condition where the free surface is close to the result I'm expecting, I've attached the image of the initial condition volume fraction at iteration 1. I ran the simulation and I've attached the final volume fraction and the streamlines along with the residuals.

Inital_condition.png

final condition.jpg

streamlines.jpg

residuals.jpg

[ghorrocks]

Looks like you are making some progress there.

Is this a homogeneous multiphase model? If so the free surface appears to be quite blurred. It should be sharper then that. Please post an image of a cross section of your mesh and the output file of this run.

[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.

Screenshot 2023-09-24 195026.jpg

[ghorrocks]

Your mesh looks OK for model development - but you will have to do a mesh sensitivity study when you have the basic modelling working. That mesh is almost certainly not fine enough for accurate results.

It is actually just the CCL I need, not the full output file. I just want to see how you have set it up. You can extract the CCL with the command line cfx5cmds -read -def [DEF FILE] -text [OUTPUT CCL]; or you can just copy it out of the top of the output file.

[joey-mastlab]

Here is the top of the output file.

CFX_007 - Copy.txt

[ghorrocks]

Thanks. My comments:

* I would run this double precision. It solves more accurately (at the expense of more memory).
* I note you have surface tension activated. For something of this size the surface tension should not be significant, but surface tension makes convergence harder. Unless you think you need it you should turn it off.
* This model will need to be run transient. Read the CFX Solver Modelling guide section on Obtaining convergence, but in short: free surface simulations have transient waves on them which have no steady solution. So you need a transient simulation to capture this.

So I recommend you start from a reasonable initial condition with a transient simulation. Set the time step to adaptive, homing in on 3-5 coeff loops per iteration. Make sure the time step size limits are wide enough you do not hit them, and the initial time step should be really small (let the solver ramp the time step size up, not down).

You will probably find this type of simulation will be quite slow. That is very common in CFD. That is why people get super computers for CFD simulations.

[joey-mastlab]

I have the simulation running based off what you said. I will post the results when it finishes.

[ghorrocks]

Hopefully you have set it to produce transient results files reasonably frequently. Then you can see how it is going as it progresses. If you did not do this then save a backup file, that can also show the results as they progress. Load it into CFD-Post and check the volume fraction to check it is staying sharp.

The main thing we are trying to achieve here is to get the free surface to resolve sharply and cleanly. Your previous result had it quite blurred. So keep an eye on the