Input File for transient cavitating flow
Hello I have a question about the input file of a transient caviting simulation.
In the cavitation tutorial it says that you should run a simulation without the cavitation modell first. That is basically the same you should do when simulating transient. I know you can fix use initial values for a transient simulation aswell but the convergence will be better. Putting everything together it should look like this: 1. Steady state of the initial transient simulation (I have a moving mesh so basically a the very first timestep) (convert .res into .cfx for next step) 2. transient simulation with water + vapour but without the cavitation modelll (so there will never be vapour) (convert .res into .cfx for next step) 3. transient cavitating simulation Is this correct? edit: At the moment I am simulating the transient cavitating flow just with the initial values but the convergence is pretty good already, it just takes ages. Will the steps I mentioned have influence on the speed of the last simulation? 
The recommended steps will get to a psuedosteady state condition faster. But if the progression from not cavitating to cavitating is important then you should start the run with a cavitation model and let the cavitation grow as it does physically.

Hello thanks for the answer.
The problem is that the results make absolutly no sense. The pressure drops far below the saturation pressure in the whole domain. When I check the initial conditions in Post I see that I already start with 1e15 vapour volume fraction. It should be 0. Quote:
How can this be when there is no equation for bubble growth? 
Cavitation models and highly numerically unstable. They cause massive jumps in density (factors of 1000 or more) and this is very difficult to keep stable. When it goes unstable the results it gives could be anything  it has gone bezerk so crazy results can come out. So if you have found a way to start the cavitation model and avoid this numerical instability then good work  they can be hard to find.

Hi!
I think you should go by the following steps: 1. Steady + noCavitation 2. Steady + Cavitation 3. Unsteady + Cavitation Good luck! :) Quote:

1 Attachment(s)
Hey thanks for your suggestion. I tryed it but I get to exactly the same results. The problem is that I dont have any boundary conditions with set pressure or something. And since the movement inside the domain is a function of time basically nothing happens when I go steady state.
I still have the same problem problems: 1. Volume Fractions: Water 1.0 Vapour 1.0e15 (I think this is the minimum value in a multiphase flow) 2. low or negative pressure in the whole domain (below saturation pressure). Its strange that eventough I have low pressure the domain is not full of vapour. I just think that its kinda impossible to get physically valid results with this setup because they look like that what we expected... qualitywise. Or am I wrong? 
You appear to be doing a moving mesh simulation, transient, with cavitation. Have you successfully done simpler simulations leading up to this  can you model moving mesh successfully? And I do not mean just simply move the mesh and get a pretty picture, I mean move the mesh and get an ACCURATE result? Adiabatic compression of an ideal gas is a good test case to make sure you can get accurate results. Then have you done a cavitation model by itself? There are validation cases of cavitating flow over cylinders, squares and airfoils which would be good benchmarks.
Once you can mode these submodels, then combine them together into the simulation with everything. If you just go straight to the everything simulation it is bound to never converge. 
Hey,
thats what I did, the last couple of month. I did a mesh motion testcase with verification data what gave me pretty much the expected results. besides that I tested the cavitation model and it converged quite good. A the moment im using the standart material library where the gas (vapour) is considered incompressible during the cavitation process. Do you recommend to do a "pseudo" compressible analysis with a function of density? 
No. The cavitation model is based on the vapour being constant density. It will work with compressible gas but the model has not been tuned for this case so caveat emptor!
Have a look at the cavitation example in the tutorials for a recommendation on how to set it up. Also it would be a really good idea to contact CFX support and see if they have a demo case to help you get started. 
Thanks for the suggestions, ill have a look at the tuts again.
I am already in contact with the support (eventough the german support cant really help =() aswell as other professionals. I finally found the uptodate paper for the cavitation model used in CFX. Besides that there are 3 validations with the last one being a transient simulation. After reading through it I have the feeling that getting quantitative results for my simulation will be quite hard since you have to tune basically every factor of the model to get things correct. And even besides that I would need some reasonable data to validate it... Anyway I am now a step further with my thoughts. Thanks 
Yes, cavitation model is very empirical. Can you post the titles, authors and publishers of the validation papers you got? They would be useful references.

Original Reference Paper Bakir et. al.
Title: Numerical and Experimental Investigations of the Cavitating Behavior of an Inducer PDF DL:PDF download (talking about the real implementation) Morgut et. al. Title: Influence of the Mass Transfer Model on the Numerical Prediction of the Cavitating Flow Around a Marine Propeller PDF Link Some validation presentation from Ansys: Link to ppt The true implementation in Ansys CFX: Zwart et al. Title: A TwoPhase Flow Model for Predicting Cavitation Dynamics PDF Paper 
Hi Sebastian,
What cavitation problem are you working on? Hydrofoil, Inducer, propeller or what? What cavitation model do you use? The default one in CFX? How do you choose the timestep? How do you create the mesh motion in CFX? What tutorial in CFX do you use for mesh moving? Do you consider the compressibility? See you soon! :) 
Quote:
1. Im simulating the cavitation of and ultrasonic horn tip (sonotrode) 2. I use the implemented one. "rayleighplesset". Its actually the zwart modell. 3. my mesh motion follows a sinus function. I use 20 timesteps from 0 to 2pi. In my case (20kHz) thats 2.5e6 s for a single timestep. 3. Ill wrote an expression for the movement (its a function of time) than I used the specified displacement/parallel to boundary option. 4. I worked through basically every tutorial that has something todo with multiphase flow, cavitation and the rigid body movement. After that I validated the movement myself with some testcases. 5. I consider water and vapour as incompressible. cfx uses a pressure based solver and is naturally incompressible in cavitation modelling. The only factore would be the pseudocompressibility with based on temperature but my simulation will be either isothermal or without the thermalequation at all. At the moment I have a pretty hard time with the correct behaviour of the domain. Right at the tip the simulation makes "some" sense but sometimes I have a terribad starting situation with the pressure or extremly strange behaviour of the pressure inside the whole domain. (sometimes 90bar with some really strange vapour fractions at some locations) If have you have more interests in these things just ask, I didnt want to explain too much if noone cares :D 
All times are GMT 4. The time now is 16:01. 