CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Cavitation Convergence Problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 15, 2015, 11:48
Default Cavitation Convergence Problem
  #1
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
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 ...
Attached Images
File Type: jpg output.jpg (41.4 KB, 79 views)
Attached Files
File Type: docx output.docx (93.2 KB, 12 views)
bejanyar is offline   Reply With Quote

Old   July 15, 2015, 20:35
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   July 16, 2015, 00:57
Default
  #3
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
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 ?
bejanyar is offline   Reply With Quote

Old   July 16, 2015, 03:16
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   July 16, 2015, 06:16
Default
  #5
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
Thanks for your replay.
I trying your suggested Solution.
I will be back soon for result !
Thank you ..
bejanyar is offline   Reply With Quote

Old   July 17, 2015, 02:59
Default
  #6
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
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.
---
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 ..
bejanyar is offline   Reply With Quote

Old   July 17, 2015, 07:31
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
My previous post said:

Quote:
Make sure the max and min time steps are wide enough that you never hit them.
Your minimum time step of 1s is likely to be far too big. Time scales for cavitation are very, very fast. Try 1e-10s.
ghorrocks is offline   Reply With Quote

Old   July 18, 2015, 14:00
Default
  #8
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
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.
bejanyar is offline   Reply With Quote

Old   July 19, 2015, 04:19
Default
  #9
Member
 
Hamidreza Bijanyar
Join Date: Jun 2015
Posts: 40
Rep Power: 10
bejanyar is on a distinguished road
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.
bejanyar is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
a problem with convergence in buoyantSimpleFoam skuznet OpenFOAM Running, Solving & CFD 6 November 15, 2017 13:12
serial/parallel problem in force saving convergence history behest FLUENT 11 July 22, 2014 04:49
Submerged fin, Convergence problem supermouniette FLUENT 10 July 6, 2009 11:47
CONVERGENCE PROBLEM - oil boiler MM FLUENT 1 February 15, 2007 06:24
convergence problem with FLUENT cavitation model Belete Kiflie FLUENT 3 February 20, 2006 11:16


All times are GMT -4. The time now is 09:49.