Cavitation Convergence Problem
 

Hello.
I studied all post in this site about this problem. but nothing happened.
I Have a butterfly valve that i am studying cavitation around it.
In one phase simulation there was not any problem and my rms reduse to 10^-6 and result was totaly acceptable .
But when i started in tow phase problem started.
example :
1- run 10 degree open valve in one phase at pressure 108217 pa with initial condition : inlet pressure : 130000 pa
2- run 10 degree open valve in two phase at pressure 108217 pa with initial condition from level 1.
cavitation not occured yet in level 2.
3- running 10 degree open valve in two phase at upper pressure like 110000 , 120000 , 130000 , and ...
All result are perfect until cavitation start.
My rms goes to 10^-1 and my monitor point doesn't goes to constant.
-----
My next step in to run one phase in any specific pressure and then run two phase in that pressure.
-----
I attached solver output files.
Any one has any idea ??
Appreciate your answer ...

Cavitation rarely converges steady state. You almost always need transient to get it to converge. Also it is highly sensitive to mesh quality. Make sure you have the best possible mesh.

Thanks for your answer.
So i have 3 another question.
1- How can i understand my mesh is the best possible mesh ?
I reed somewhere if i use refined mesh the convergence become harder !
It is correct ?
So is it possible that i reach convergence by using coarse mesh ?

2- I cant use steady stats solution at all ? Or with some optimization it could happen ?
And what configuration should i use in transient in ansys cfx ??

3- For initial condition which of previous post approach is better ?
Continue from one lower pressure to a higher in 2 phase ?
Or start from 1 phase in all pressure and use it in 2 phase at that pressure ?

For cavitation modelling any improvement in mesh quality will be worth it. If your mesh is 90 degree hexas with 1:1 aspect ratio then there is no need to improve. There is no universal answer to how good your mesh needs to be. Do some trials of different mesh qualities in your configuration and see what convergence differences it generates.

Refined mesh = harder convergence. Correct.

Yes, that means you might converge on a coarse mesh but when you refine it fails to converge.

2 - Yes, you can use steady state solutions. The problem is getting them to converge for cavitation simulations. It is very difficult. If you get convergence with a steady state model then fantastic - but in my experience this is uncommon and most models need transient.

I would recommend transient simulation with adaptive time stepping homing in on 3-5 coeff loops per time step. Make sure the max and min time steps are wide enough that you never hit them.

3 - Either can work. Increasing the pressure is more physically realistic for the startup transient, but if you only want the steady result this is not important.

Thanks for your replay.
I trying your suggested Solution.
I will be back soon for result !
Thank you ..

As you told hexas element with 1:1 aspect ratio is very well.
But my mesh is tetrahedral and wedge.
My aspect ratio in mainly 1:16 and somewhere is 4 !!
My orthogonal quality Is mainly 0.88 to 1.
I tried to use hexas element but "hex dominant" method make poor elements and region can not sweep so i cant use "sweep" method.:confused:
---
In changing steady stats to transient simulation :
Maximum Number of timesteps : 2000
Time steps : Adaptive
First Update time : 0
Timestep Update Freq : 1
Initial timestep : 10 s
Option : Num. Coeff. Loops
maximum : 3 Hours
Minimum : 1 s
target max loop : 5
target min loop : 3
timestep dec : 0.8
timestep inc : 1.06

with this configuration noting goes better and my model dont converge again.
---------
What is my problem ???
My time is finishing and my model in not ready .. :(

My previous post said:

Your minimum time step of 1s is likely to be far too big. Time scales for cavitation are very, very fast. Try 1e-10s.

Ok !
I did it .

1- I set max coef to 6 in solver and 0.1 s for timestep and 50 s for total time. but it didn't converge in one timestep.

2- In 0.01 s for timestep and 5 s for total time it converge after 15 coef loop in one timestep.

I saw that U-Mom-Bulk , V-Mom-Bulk , W-Mom-Bulk converge very fast and goes down to 1e-4 but P-Vol dont converge at all, even in 1e-15 timestep it remain on 1e-2 and dont go lower !
In 1e-15 timestep U-Mom-Bulk , V-Mom-Bulk , W-Mom-Bulk goes to 1e-12 but P-Vol !!!
What is this problem ????

Finally I set max coeef to 20 and timestep to 0.01 and totaltime to 5 s.
All U-Mom-Bulk , V-Mom-Bulk , W-Mom-Bulk , P-Vol goes down to 1e-4 and it is ok. I continued to run to 62 run .
After checking result they didn't reasonable and correct.
What i should do to ??
Is it possible that my solve dont converged ???
How can i find it ???
I Really Really tank you for your very kindly answers.

Thank You Glenn .
Finally I got true result and my simulation finished. :)
I should continue with upper pressure .
I hope no problem wont be happen.
Thank you again. :)