[namgnirps]

Hello All,


I want to simulate the following transient system:

Fluid is flowing through a pipe and an orifice into a closed chamber. The model is rotational symmetrical, the pipe orifice and a part of the chamber is filled by liquid, the rest of the chmber with gas. I built a 2.5d model of the system with transient inlet velocity as boundary condition. The process is fast: total simulated time: t=0.1s, Re_Inlet: ca. 12000.
Now I am struggeling with the following problem:



1. Simulation Error:

If I model the gas as ideal gas, I get a stack over flow error after t=0.025s (22 timesteps). I used adaptive time steps. The last timestep is T=0.0001s, which is the minimum allowed timstep. Double precision is on.

If I use constant property gas, the simulation runs fine with a fixed timestep of T=0.005s.
Do i need to reduce the minimum timestep further? Or the the problem somewhere else in the model?


2. For the model with constant property gas:

The pressure of the gas is not increasing over time although fluid is flowing into the closed system. I guess this is the effect of a constant property gas, right? Thus, will be solved, if the ideal gas model is running...

Furthermore, the volume of the gas is not reducing proportionally to the mass flow of fluid entering the closed model. Is this also an effect of the constant property gas model?


Thank you for your support in advance!


BR,
Namgnirps

[ghorrocks]

You will need to provide more detail of what you are modelling for us to answer that. Please post some images of your model and your output file.

Note that ideal gas is compressible and that means you now have compressible flow effects. This will mean transient pressure waves, and maybe even shock waves if your flow is fast enough. Also, are you using a free surface model? The free surface model will have a harder time if you use a compressible gas phase.

[namgnirps]

Hi ghorrocks,

Thank you for your reply!

Here two pictures of the boundary conditions and the two phases at t=0.
BCs.png

Phases_t0.png

The out-file is:
out-file.zip

[ghorrocks]

I see many problems with this simulation.

* You have viscous work turned on. Unless you think you need this model you should turn it off.
* The function dSAT out is not used.
* You are using a surface tension model. This massively increases the difficulty of the simulation. Turn it off unless you need it. If you need it you will need to do a different setup to get it to work (which will greatly slow down the simulation).
* Your surface tension coefficient does not look like a value typical of a oil/nitrogen interface. Are you sure this value is correct? (but more importantly, delete it if you don't need it)
* You have a multiphase model with homogeneous model = on, but no free surface model, yet you define a surface tension. Is this what you intended?
* You define a reference pressure of 20.36 bar, but a relative initial pressure of 20.36 bar. This means the initial pressure will be 40.72 bar absolute. Is this what you intended?
* You are using adaptive time steps with not recommended settings. The recommended settings are:
Min time step = 1e-6 [s] (or something very small)
Target Max coeff loops = 5
Target Min coeff loops = 3
And the initial time step set small enough that the first time step converges OK.

[namgnirps]

Hi ghorrocks,


Thanks for your super fast reply!


I tried to impolement all changes you mentioned. The updated model now shows a different error: "ERROR #004100018 has occurred in subroutine FINMES. Message: Fatal overflow in linear solver."


Here the corresponding out-file:
out-file2.zip


I do not know, which of the implemented changes let to the mentioned error. Maybe I implemented something wrong?

[ghorrocks]

* You should set the reference pressure to 20.36 bar and the initial pressure to 0 bar relative.
* You are now using a eularian particle multiphase model. You need to match the multiphase model to the physics of your model. What do you expect the oil/N2 to do in the device? Does it mix to droplets? Foam? A distinct free surface?
* You are getting Mach 3 on the first time step. You need to look at this first time step and determine whether this is realistic or not.

[namgnirps]

Hi,


thank you for your hints!



I implemented the oil as particle phase because Ansys recomments this option if I chose an inhomogenous turbulence model. I set it back to continous fluid and homogenous turbulence model. Furthermore I changed the model to
- smaller timesteps
- reference pressure 20.36 bar
- finer mesh.

The simulation works for the first 0.0257s now, but the timesteps get cut to the minimum timestep (1e-6 s). Then it abborts due to negative absolute pressure (see output-file).
Might this occur due to cavitation due to the high velocities? And if yes, is it promising to implement a cavitation modell?


Do you have any further recommendation regarding the model options?

[ghorrocks]

You have missed the point. Before you do anything further you need to look at your system. How are the phases interacting? Are they a foam? bubbles? droplets? Or a distinct interface? Maybe condensing on the walls?

Once you know what multiphase physics are happening you then choose a multiphase model suitable for that physics.

[namgnirps]

I think that there will be an oil jet through the gas phase which will hit the wall and then spray into droplets at the wall.

[ghorrocks]

Like this?

Jet.png

[namgnirps]

This are the phases in the simulation before it interrupts.
Phases_t0.02s.PNG

Phases_t0.025s.PNG


According to these images I assume that the jet will be rather coherent until it hits the top surface. At the surface I think the jet has to break into droplets because of the high impact speed.

On the other hand, the oil is simulated as continous fluid. So might the observed behaviour is enforced by the modelling?

[ghorrocks]

This is sounding like a free surface model. This means you should set up the simulation according to the CFX example "free surface flow over a bump". If you want to model the breakup of the oil into droplets you will need to include surface tension. Do not use any particle or bubble models.

If you expect breakup like this: http://gerris.dalembert.upmc.fr/gerr...on.html#htoc16

then be aware that this will be a seriously difficult simulation, and not for beginners. It will require an extremely fine mesh, very fine time steps and a very long run time. Also you will need a full 3D mesh, you cannot simplify it to 2D.

(Also note that I would seriously consider gerris for your simulation. It handles this sort of flow MUCH better then CFX. It is also open source so there is no licensing stopping you.)

[namgnirps]

Hi ghorrocks,


thank you for your support. I allready had the feeling that the problem is much more difficult than it looks in the first view to a cfd beginner.


For my understanding:
As I mentioned in the initial post, I did a simulation with surface tension and contious fluid phase, but with a constant pressure gas.
This simulation runs fine, but of course the gas pressure was not increasing properly.
So is the replacement of the constant pressure gas with the ideal gas the reason for the massively increased difficulty of the analysis?


Furthermore I would like to ask you:
Does the aim of the analysis have any impact on the complexity?
For me, the exact flow pattern of the jet is not important.I am only intrested in the pressures before and after the orifice.
Do you see a reasonable way to reduce the complexity of the simulation that still enables it to calculate the pressures correctly?

[ghorrocks]

Actually setting CFX up to do a free surface model with surface tension is easy. The hard bit is doing it such that the result is accurate enough to be usable, and justifying that it is accurate. Generating accurate results is the difference between a CFD practitioner and somebody just following the tutorials.

It now looks like you are talking about a free surface model with surface tension. The issue is getting this accurate requires extremely fine meshes, ludicrously fine time steps and very tight tolerances on allowable mesh quality.

For example, model a spherical drop in space with surface tension. The pressure of the drop is defined by the Laplacian pressure so has a simple analytical answer. I recommend you model this trivial example as you will soon discover that this apparently trivial simulation is challenging to get accurate.