[Pugnax]

I am having trouble getting a cavitation model, using ethanol liquid and vapor, to converge to an appropriate level. The analysis uses the Steady-State Solver and the geometry has two domains; a rotating domain which includes a cylindrical rotor, and a stationary domain which includes the stator (casing for the rotor), one inlet, and one outlet. There exists a thin, annular gap (1/10 in) between the two domains and the domains are connected via GGI interfaces. The domain settings and models used along with boundary conditions are summarized below.

I initially start with the cavitation model turned off and a high enough pressure so cavitation does not occur (in my 30psi is sufficient). After that converges, I keep all values and settings the same but turn on cavitation and initialize the run using the previous converged simulation. I can get this one converged as well to an a appropriate level. An appropriate convergence for my simulation is an RMS of 1e-5, conservation of 0.01, and monitor points for pressure, mass flow (inlet and outlet), and average volume fractions for the domains must level off and stay steady.

After that, I drop the pressure to 28psi where cavitation begins to occur. At this point I am unable to get convergence no matter how much finessing and tweaking of the timescale. Since I've been trying to run this as steady-state I have tried a complete spectrum timescale controls. I have used auto timescale with different timescale factors, physical timescale using a characteristic scale of 1[rad]/4000[rev min^-1] and average advection time for the domains as a starting point. In addition I have used different timescales for each equation class (continuity, volume fraction, etc) to better fine tune but to no avail. I've included some images of the residuals so you can see how the residuals behave. Normal methods for reducing residuals have not worked for me (i.e. if they appear bouncy your timescale is too large, if you have a small convergence rate your timescale can be increased).

Because of my issues with convergence I have followed the necessary steps in the cfd-online wiki ANSYS CFX FAQ and the solver-modeling guide. Going through these steps makes me think that its not a timescale issue or a mesh issue but a physics/modeling/material error. I believe the error is associated with the way I have defined the material properties for Ethanol Liquid and Vapor. I've attached images for the settings below. I imported these materials from the IPMT Library and changed the reference states and material properties to exclude compressibility and include steady state properties.

As a final note, I am currently running a transient run to see if it solves anything (even though I have already tried this and the residuals for each timestep become jagged and sporadic). Also I am using the BSL Reynolds Stress Model because I found that I had an easier time converging than using the k-omega SST model. I used the BSL model because of the very fast rotating, swirling nature of the geometry.

So my questions are:
1) What can be seen that is wrong or inappropriate in my model and/or physics that could be cashing poor convergence?
2) Do my material properties, as I have defined them, look correct?
3) Is my selection of the BSL Turbulence model seem correct (I haven't had any trouble getting it to converge)?
3) If nothing appears to be wrong, why am I having such a difficult time obtaining convergence?
4) As a general question, what causes residuals to become "jagged" and/or "spiky" but still, in its characteristic shape, maintain convergence?

Sorry for the long post; I wanted to provide as much detail as possible because this has really stumped me and I have never had this much trouble with a cavitation problem. Any insight, advice, or corrections would be greatly appreciated.

-Pugnax (Curtis F.)

======Domain Models & Settings======
---Basic Settings---
- Ethanol Liquid (C2H6Ol) and Ethanol Vapor (C2H6O) ---> Morphology: Continuous Fluid
- Reference Pressure: 1 [atm]
- Non Buoyant
- Domain Motion: 4000 [rev min^-1]

---Fluid Models---
- Homogeneous Multiphase
- Heat Transfer ---> Isothermal: 35[C], No Radiation
- Turbulence: BSL Reynolds Stress, Automatic Wall Function

---Fluid Pair Model---
- Mass Transfer: Cavitation ---> Rayleigh Plesset, Default Settings, Saturation Pressure = 114997 [Pa]


======Boundary Conditions======
- Inlet: (Inlet) ---> Bulk Mass Flow Rate: 0.13 [kg s^-1]
Fluid Values: C2H6Ol = 1, C2H6O = 0
- Outlet: (Opening) ---> Opening Pres and Dirn (30psi)
Fluid Values: C2H6Ol = 1, C2H6O = 0
- RWall: (Wall) ---> No Slip Condition
- StatWall: (Wall) ---> No Slip Condition
- R2S Interface R: General Connection: Frozen Rotor, GGI, No Pitch Change
- R2S INterface Z: General Connection: Frozen Rotor, GGI, No Pitch Change

======Attachments======
1) RMS Residuals 30psi Cavitation is activated
2) RMS Residuals 28psi Cavitation is activated (solver starts at the 250 time step)
3) Volume Fraction Residual (Mass-Ethanol) 28psi Cavitation is activated (solver starts at the 250 time step)
3) Material Properties Ethanol Liquid
4) Material Properties Ethanol Vapor

[Pugnax]

Also, if needed, here is my CCL file for the 28psi case.

[ghorrocks]

It has been a while since I did cavitation modelling, but I recall that I was forced to use transient simulations. Cavitation is a very transient thing (the cavitation bubble keeps jiggling around), so this is not surprising. I would recommend using adaptive time stepping, homing in on 3-5 coeff loops per iteration. Make sure the minimum and maximum time step sizes are wide enough that you never hit them.

Also note that the default cavitation model in CFX is built around water. As you are using ethanol I trust you have looked at the appropriateness of the settings in the model.

I would not use an RSM turbulence model if you are having difficulties in convergence. RSM will just make it worse. I would use a simple turbulence model (even k-e or a zero equation model) just for debugging.

Note that modelling cavitation is on the edge of known numerical models, so modelling turbulent cavitation is a step further again. While I appreciate the logic of using RSM in a rotating flow you really are in uncharted territory there. I would use a simpler turbulence model.

[Pugnax]

Thanks for your quick reply Glenn! I'm grateful for the suggestions.

I have moved on to transient analysis. Like you say, it is by its very nature a transient phenomenon and was getting no where using Steady-State. It has been my experience so far that a transient analysis works very well in obtaining convergence (across all measures) but only for so long. After approximately 8 - 12 iterations, the solver starts to diverge and becomes sporadic while imbalances leap up and down by orders of magnitude. However, I am going to try again with simpler turbulence models per your suggestion and see how they behave.

The fact that the cavitation model used in CFX is built around water is something I have known of and have spent some time reading the Theory Guide to understand how it's specifically "honed" for water. From what I can gather the Cavitation Condensation Coefficient and the Cavitation Vaporization Coefficient are empirical factors that I assume are specific for water. I have done some research as to how these empirical factors are calculated and how they might be tweaked to better compensate for ethanol, but what I have found has been sparse in literature and/or detail or has been over my head. Hmmmm, now that I think about it I should go back and look over the paper by Bakir et. al. Am I correct in saying that CFX uses that model that they describe in that paper?

In either case if you know of or could point me in the direction of some resources that would be helpful.

-Pugnax

[ghorrocks]

There is also the volume fraction and nucleation site radius of the model to consider as well. I suspect these are water values as well. The documentation references Bakir et al for validation and description of the model, it sounds like you should chase this reference up.

Use adaptive time stepping to help fix the sporadic spikes in convergence. It is hard to eliminate them, but hopefully you can reduce them enough that the simulation is useable.