Franco Concli : Your answer refers more to OpenFoam rather than to Fluent. In ANSYS Fluent the most recommended cavitation model is the Zwart-Gerber-Belamri model (how it is called in Fluent). Essentially the Fluent developers picked-up the cavitation model developed by the CFX developer Phil Zwart and put it into Fluent, because it is much more reliable and numerically robust than the Schnerr-Sauer model, which is the one the Fluent developers were earlier relying on.

Wael Elsaady : Back to your original question. First of all you need to answer the question, whether it is your intention to :

a) run a simulation with CFD resolved bubble-water interfaces, where you are interested in the detailed bubble shapes and how they change by the change of your flow volume (which corresponds to a change in the fluid pressure concurrently)? This would lead us to a Volume-of-Fluid simulation with resolved interfaces and heat/mass transfer description at the free surface. In that case a phase change model would required to be used. Cavitation model would not do the job well (or not at all). Or:

b) you cannot resolve the fluid-bubble phasic interphases, because you are not looking on a few isolated bubbles but on a large number of very tiny bubbles. In this case you need to describe the bubbly flow in an Eulerian-Eulerian model framework by some volume-averaged gas-phase volume fraction. In that case you can try the Zwart-Gerber-Belamri model. It will provide you with an increase in gas void fraction due to the pressure change, caused by the volume change in your flow volume. But in the framework of the cavitation models you usually have no control over the bubble size. The typical size of a cavitation bubble is determined by the cavitation model itself and almost kept constant. I.e. all produced vapor is interpreted in the framework of the Eulerian model as an increase in the number of bubbles per unit volume. If you have other knowledge (e.g. that the number of bubbles rather stays constant for your conditions and no existing nuclei are contributing to formation of new bubbles), than you could just take the calculated local volume fraction of the vapor phase and recalculate it into a changed bubble diameter, based on the seeded number of bubbles in your initial conditions, i.e. keeping the number of bubbles constant instead of their diameter. This interpretation of the volume fraction could be done as a postprocessing step.

Dear Mr. Wael Elsaady ,

I have tried to find cavitation in closed system (No Inlet/Outet) with pump casing and impeller inside the casing. I tried without using cavitation model by just inspecting pressure change. It helps me to have good idea of cavitation in turbulent system. Actually that was for water treatment system.

Dear Mr sagar,

Thank you for your reply. Certainly, cavitation occurrence can be assessed by pressure gradient. However I'm curious if there any representation for cavitation or aeration in extending or shrinking domains.

Regards

Wael

Fluent has 2 main cavitation solvers in which you can select the cavitation model you prefer.

The solvers are interPhaseChangeFoam and cavitatingFoam.

The cavitation model used by the solvers are the models of Kunz and Schnerr-Saurer.

Have a look to this publication of mine

Article NUMERICAL MODELING OF THE POWER LOSSES IN GEARED TRANSMISSIO...

Article Pressure distribution in small hydrodynamic journal bearings...

If you need further help just aks.

Best regards

Franco

Dear Franco Concli

Thank you for your reply. I will go through your publications and will try to perform some cases. I am afraid that I have no experience with cavitation models.

Regards

Wael

Dear Wael Elsaady ,

in OpenFOAM also some tutorial are available for cavitation: have a look in the tut/multiPhase/interPhaseChangeFoam folder.

Franco

Franco Concli : Your answer refers more to OpenFoam rather than to Fluent. In ANSYS Fluent the most recommended cavitation model is the Zwart-Gerber-Belamri model (how it is called in Fluent). Essentially the Fluent developers picked-up the cavitation model developed by the CFX developer Phil Zwart and put it into Fluent, because it is much more reliable and numerically robust than the Schnerr-Sauer model, which is the one the Fluent developers were earlier relying on.

Wael Elsaady : Back to your original question. First of all you need to answer the question, whether it is your intention to :

a) run a simulation with CFD resolved bubble-water interfaces, where you are interested in the detailed bubble shapes and how they change by the change of your flow volume (which corresponds to a change in the fluid pressure concurrently)? This would lead us to a Volume-of-Fluid simulation with resolved interfaces and heat/mass transfer description at the free surface. In that case a phase change model would required to be used. Cavitation model would not do the job well (or not at all). Or:

b) you cannot resolve the fluid-bubble phasic interphases, because you are not looking on a few isolated bubbles but on a large number of very tiny bubbles. In this case you need to describe the bubbly flow in an Eulerian-Eulerian model framework by some volume-averaged gas-phase volume fraction. In that case you can try the Zwart-Gerber-Belamri model. It will provide you with an increase in gas void fraction due to the pressure change, caused by the volume change in your flow volume. But in the framework of the cavitation models you usually have no control over the bubble size. The typical size of a cavitation bubble is determined by the cavitation model itself and almost kept constant. I.e. all produced vapor is interpreted in the framework of the Eulerian model as an increase in the number of bubbles per unit volume. If you have other knowledge (e.g. that the number of bubbles rather stays constant for your conditions and no existing nuclei are contributing to formation of new bubbles), than you could just take the calculated local volume fraction of the vapor phase and recalculate it into a changed bubble diameter, based on the seeded number of bubbles in your initial conditions, i.e. keeping the number of bubbles constant instead of their diameter. This interpretation of the volume fraction could be done as a postprocessing step.

Thomas Frank : Maybe you are right... but from my experience, also the SS one works pretty well... at least for the cases I have tested.

Franco

Franco Concli : Depends on what does it mean, that the "model works well"? The Schnerr-Sauer model can provide sufficiently accurate cavitational flow solution. But in my experience it is much more difficult to get it to really good convergence. In consequence I have frequently seen, that people interpret a not sufficiently converged solution in a physical sense, which should never be done in my honest opinion, since it can be misleading. But what convergence means in ANSYS Fluent is an entirely new topic, where we could discuss for long time. E.g. why most of the time in ANSYS Fluent the residual of the continuity equation is never reaching sufficiently low values (e.g. 10^-5) and what does that mean for the accuracy of the solution? And why the Fluent development team is not able to fix this issue for decades... (while other CFD codes can converge the continuity equation for the same problem successfully).

Dear Thomas, I agree. In my simulations, in fact, I have comparte the numerical predictions with experimental measurements.

Best

Franco

Dear Franco Concli and Thomas Frank ,

Thank you so much for your answers.

Thomas Frank : I am really interested in a bubbly flow with a large no. of bubbles and no interest to the shape or interfaces of bubbles. So, the Zwart-Gerber-Belamri or SS model are the choices now. However, according to:

https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/flu_th/flu_th_sec_multiphase_cavitation.html

I can understand that the vaporisation comes when the pressure is below the vapour pressure. In other words, it is a function of pressure and the existing volume fraction of bubbles, not the increasing/decreasing volume fraction due to change in volume? may be?

So, if we imagine an extending closed domain (increasing volume), thus, the pressure goes down and cavitation occurs. However, how is the extended volume is represented in simulation?, as gas, liquid or mixture? In other words, Does the cavitation models in this case account for the gas volume fraction increase or it will only a function of pressure gradient and the volume fraction is determined from initial conditions?

Best Regards

Wael

Wael Elsaady : The cavitation model requires the fluid to be represented as a multiphase mixture of the fluid with vapor bubbles. Initial volume fraction can be very small, just providing a seeding for the cavitation model to take effect (an initially existing interfacial area, where mass transfer can occur). The last question in your post I unfortunately do not understand very well. In the case that the volume expansion of the domain will lead to some pressure decrease below the vapor pressure of the fluid, the cavitation model will determine a mass transfer term, leading to liquid evaporation and formation of additional vapor volume fraction.