[ndabir]

Hi,

I am simulating a low pressure air bubble inside a high pressure liquid. Basically this is a Riemann problem. The problem is when I assume the liquid to be incompressible, as soon as the simulation starts, the pressure will be diffused between the high and low pressure regions (it will look like a rainbow of colors).

However, if I set the liquid to be compressible, the pressure diffusion will not happen as bad as before but it is still significant. I have attached a figure to better show this.

My question is which solver settings, discretization method, etc should I use to prevent this artificial pressure diffusion. I should say reducing grid and time step has not helped at all.


P.S. I should mention that when I do the same settings as above to model a shock tube (low pressure air and high pressure water), the pressure diffusion does not happen and everything works fine.

Any ideas?

The attached figure is when liquid is set to be compressible.
pressure contours.jpg

[ghorrocks]

What are you trying to do? How do you get low pressure gas bubbles in a high pressure liquid? Won't the pressure equalise in a few zillionths of a second anyway?

[fivos]

Hi ndabir,

It all depends on what exactly you want to do; if you want a high accuracy (i.e. very small time steps, e.g. 1ns or so) then yes liquid compressibility must be included. If you intend to use larger time steps (e.g. 1μs or more) then incompressible liquid is still good. This will also depend on the bubble size..

Regarding the 'pressure diffusion', what you see is normal and actually it is not diffusion at all.. Remember that when you have depressurization you always have rarefaction wave which by definition is a smooth transition and not an abrupt change as a shock wave. This is applicable to the solution of the Riemann problem as well, but it might be not that apparent, because the tail and the head of the rarefaction have very similar velocities for small liquid velocities/pressures.

The main difference is the fact that in the Riemann problem you have 1D flow, whereas in your bubble case you have 2D (axisymmetric?) or 3D and this WILL affect the pressure distribution. You could try to solve the 1D Riemann problem but with source terms to apply axis-symmetry, as a comparison; you will see that you will get the same effect with the CFX results.

For more information, see the book of Toro for more on that
(Toro, Eleuterio F. (1999). Riemann Solvers and Numerical Methods for Fluid Dynamics) or his relevant publication on liquid compressibility (On Riemann solvers for compressible liquids, M. J. Ivings, D. M. Causon and E. F. Toro).

Out of curiosity, what Equation of State did you use for the liquid?

@ghorrocks: probably he is trying to study fundamental cavitation, i.e. bubbles generated due to cavitation and then collapsing due to pressure recovery. Pressure will equalize rather quickly, depending on bubble size/pressure difference, but in the process you will get a lot of rebounding of the bubble with associated pressure pulses radiated around, until viscous dissipation damps out the energy from this pressure difference. For more info see Rayleigh-Plesset equation (which is a simplification of NS equations for bubble dynamics http://en.wikipedia.org/wiki/Rayleigh%E2%80%93Plesset_equation)

[JuPa]

That contour of pressure is pointless without a scale.

[ndabir]

Originally Posted by ghorrocks

What are you trying to do? How do you get low pressure gas bubbles in a high pressure liquid? Won't the pressure equalise in a few zillionths of a second anyway?

I am initializing the simulation with a low pressure bubble inside a higher pressure liquid. This is basically the collapse of bubble in cavitation phenomena.

What will actually happen is the high pressure liquid will contract the bubble to smaller size eventually making a higher pressure inside bubble.

I would like to minimize this rainbow pressure change to a few grids (now the pressure changes in a large area which is several times the radius of bubble).
The pressure inside the bubble at the beginning of simulation is 50 times smaller than the surrounding pressure.

This rainbow pressure change can be seen mainly when I put the bubble close to a wall. like the attached picture which the bubble is close to a wall at the bottom of the figure.

[ndabir]

Originally Posted by fivos

Regarding the 'pressure diffusion', what you see is normal and actually it is not diffusion at all.. Remember that when you have depressurization you always have rarefaction wave which by definition is a smooth transition and not an abrupt change as a shock wave. This is applicable to the solution of the Riemann problem as well, but it might be not that apparent, because the tail and the head of the rarefaction have very similar velocities for small liquid velocities/pressures.

The main difference is the fact that in the Riemann problem you have 1D flow, whereas in your bubble case you have 2D (axisymmetric?) or 3D and this WILL affect the pressure distribution. You could try to solve the 1D Riemann problem but with source terms to apply axis-symmetry, as a comparison; you will see that you will get the same effect with the CFX results.

I totally agree with you about the rarefaction wave, however that should also happen in a few grid points distance (probably a little bit wider than the shock wave itself). In my case this so called rarefaction wave is happening in a very large distance probably in a thousands of grids away from bubble center. I have attached a plot of pressure dissipation for my case when fluid is compressible. I personally think this much pressure change is a lot.

By the way, I am using Tait equation of state for liquid and yes as you guessed correctly I am simulating bubble collapse in very short time scales of few microseconds.
pressure plot.jpg

In the attached plot as it can be seen, the uniform smaller pressure is for inside the bubble and then the pressure starts to gradually increase to match with the surrounding pressure. This is why I say it looks like diffusion. I should say that this plot is for some intermediate time not at the beginning.

Is there a way I can prevent this huge gradually pressure change? Or is it completely normal?

[fivos]

Hi ndabir,

A fundamental question that I have to ask you is how do you know that this 'rainbow color' you mention is unnatural. In my response to you I explicitly mentioned:

The main difference is the fact that in the Riemann problem you have 1D flow, whereas in your bubble case you have 2D (axisymmetric?) or 3D and this WILL affect the pressure distribution. You could try to solve the 1D Riemann problem but with source terms to apply axis-symmetry, as a comparison; you will see that you will get the same effect with the CFX results.

In other words you cannot expect the pressure distribution from the 1D Riemann problem to be valid for a 2d axisymmetric or 3D simulation of spherical collapse. The only way to make such a comparison is to apply the 1D Riemann problem, but with geometric source terms.

Allow me to restate: The effect you observe is totally physical and it has to do with the multidimensional nature of the flow. It has to do with the momentum focusing effect due to spherical symmetry; it is the same reason that during the later stages of collapse pressure will rise first at the liquid surrounding the bubble and then inside the bubble. For more information on these you can see the very good book of Franc and Mitchel Fundamentals of Cavitation (it has a chapter exactly for the pressure field of the bubble, namely 3.2.3 the pressure field).

It has nothing to do with diffusion and smearing of pressure waves.

You also need to keep in mind the following: while liquid compressibility plays a role, especially at the last stages of the collapse, at the beginning the flow velocity is small, thus the incompressible approximation is valid. I am saying that because you should expect at the first stages of collapse (not those affected by the pressure wave passing) a pressure field similar to the incompressible solution as the flow is slow with Mach no<<1.

I am working on a very similar subject and I have done quite many analysis of bubble collapses, with Fluent/CFX and custom density based solvers. The results I have got are very similar with the exception of Fluent/CFX sometimes predicting oscillations near the pressure waves, due to the stiffness of the Tait EOS.

[ndabir]

Originally Posted by fivos

A fundamental question that I have to ask you is how do you know that this 'rainbow color' you mention is unnatural.

Thanks for your clear response. I agree with your comments but I should mention that the reasons I think this may not be normal are:

1) Since the bubble should collapse under ambient pressure (say 1 atm), however when the pressure in the surrounding smears, the amount of pressure will be less than 1 atm pressure (see the plot that I attached before). I think this may cause the bubble to not shrink as much as it should (not sure about it) because the driving pressure will be smaller.

2) This pressure smearing causes problems especially when the bubble is very close to the wall. (Actually this is the main reason I am looking for a method to prevent pressure smearing).

You can check on my previous post about this issue (there is a wall on the bottom of bubble):
http://www.cfd-online.com/Forums/flu...imulation.html

Any ideas about the above post?

you mentioned you have used density based solvers for you previous bubble collapse.

Originally Posted by fivos

I am working on a very similar subject and I have done quite many analysis of bubble collapses, with Fluent/CFX and custom density based solvers.

How did you use density base methods? because I use fluent and it does not allow me to use density based solver while using vof method. Therefore I am using pressure based solver for my calculations. Do you think using pressure based solver is amplifying this smearing problem? I should say I have used pressure-based solver for 1D Riemann problem before and it predicts everything including shocks very well.

[fivos]

Hi again,

Lets take things step-by-step:

See the attached picture, named comparison.jpg. It is a comparison between 1D solution of Riemann problem (with source terms to accommodate spherical symmetry) and a 2d axis-symmetric simulation. As you will see there is the rarefaction, which involves several grid points, being gradual, but since it is water, it is rather thin. Also you will see a more 'diffuse' pressure transition, which is due to momentum focusing, i.e. non-1D effects. These results are from a custom density based solver I have (sorry, its not Fluent, see also below), for a collapsing cavitation bubble; since I have not published these yet I do not want to show exact conditions (sorry...). So, what I want to clarify, is that the 'diffuse' pressure distribution is normal and I hope it is clear. Now if it is exactly according to theory, well, maybe it is something you have to check with benchmarking with a reference solution..

I would strongly suggest you to go though the relevant literature I mentioned (Toro for compressible and Franc for cavitation).

To answer your questions:
1) This is natural, it will not prevent the bubble from collapsing. You can try for a bubble at infinity (keep the boundaries at least 100*Radius away, or you will have bias) and compare with the Rayleigh Plesset equation. With Fluent I got very good agreement. I would expect the same from CFX.


2) Now this is a good question. Again I repeat, the 'smearing' you get is normal. But the problems you have are due to the wave interaction with the boundary. In cases I have seen in the past, such interactions may cause negative pressures. If you combine that with the ideal gas EOS you use for the gas (I suppose), you get convergence issues, because the solver struggles to limit the pressure to prevent negative densities for the gas phase... The way to get around this problem is check you pressure limits; do not let pressure go too low (e.g. I have used values ~100Pa depending the case). In Fluent you can try the hidden tricks of VOF, such as enhanced compressible numerics (solve/set/vof-numerics - check also ANSYS help, there are lots of stuff for VOF, including Rhie Chow tuning which could be helpful..)

In reality you would have cavitation formation due to nuclei excitation at such areas, but it will be rather difficult to do that with CFD, so probably you will have to cut pressure and accept a small error...


A final note: Fluent 'density' based solver indeed is not compatible with cavitation, VOF and many multiphase models. However you have to keep in mind that it is not a pure density based solver either.. check ANSYS help at the section of preconditioning for the density based solver and you will see that they eventually resort to [p, u, v, w, T] variables and not the conservative set [ρ, ρu, ρv, ρw, E] which is used from density based solvers..

As long as you do not go into high Mach number flow and keep with simple resolved bubbles (and not diffuse bubble clouds, where speed of sound can drop to 0.1-1m/s) the pressure based solver is good to go. But you have to be careful with negative pressures and pressure bounding.

Good luck with your work..


BTW. if you eventually decide to go with Fluent, use something better than SIMPLE (e.g. PISO, which is nice with NITA, or even better Coupled) and do not use PRESTO!; use Body force weighted instead. If things are still tough, try blended 1st/2nd order schemes.

[ndabir]

Thanks fivos. Really appreciate the way you discussed the issue. Now it is clear to me that the pressure smearing is normal and that's good to know.

I will check the references you mentioned and hope to solve the issue with wave interaction with wall.