CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

multiphaseEulerFoam strange behaviour in damBreak4phase tutorial

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 2, 2012, 04:57
Default multiphaseEulerFoam strange behaviour in damBreak4phase tutorial
  #1
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
Hello Foamers,

I am trying to explore the performance of the new multiphaseEulerFoam (OF 2.1.0), but in the beginning I found a mystery behaviour in the basic damBreak4phase tutorial case.

The problem is in time 5.75s, until that time the flow is stable, the column colapses and the mixture is trying to stabilize (loose kinetic energy) and separate by density.
(T = 0.00s, T = 0.15s, T = 5.70s)


But in time 5.75s the nearly stabilized mixture vanishes into thin air.


I don't suppose that I am the only one who knows this problem. I faced it from time to time in the last year when I was exploring the bubbleFoam and interFoam but I never found an example this ilustrative to solve.

So does somebody know what is wrong in such case? What can I try to correct?

Thanks in advance, for any hint.
Martin.
darai is offline   Reply With Quote

Old   March 2, 2012, 06:42
Default Testing nOuterCorrectors
  #2
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
Hello,

First attempt to break this problem was through the nOuterCorrectors PIMPLE parameter. I know that this parameter controls the pimple.loop() cycle and I found a notice that it is used to control the number of iterations of the Reynolds-Averaged, Navier-Stokes equations. (I guess that for my laminar case we talk only about N-S equations, but the meaning is similar)

So I tried a second calculation, where I used nOuterCorrectors 5 and I compared the results. The dissipation is gone now, but... The behaviour is now chaotic. It behaves like a boiling pot, not loosing the kinetic energy and it "breakes (first acceleration of the water column)" much faster than with nOuterCorrectors 1:

(T = 0.00s)

(T = 0.05s)

(T = 0.10s)


So these results gives more questions than answers. Why is pimple behaving this way? Is it because the nOuterCorrectors parameter isn't created for transient applications, only steady state?

Thanks in advance for all the help,
Martin.
darai is offline   Reply With Quote

Old   March 5, 2012, 07:19
Default
  #3
Senior Member
 
Daniele Vicario
Join Date: Mar 2009
Location: Novara, Italy
Posts: 142
Rep Power: 8
danvica is on a distinguished road
Unfortunately I don't have any clue about this problem. I reply because, beeing a newbie in CFD, this kind of thing worry me.

In general, is it possible for a not-expert use OpenFoam to get trustable results ?

Mine is not a critic to the package, I think it's an impressive work still improving. Just a clear question.

I understand that CFD field requires deep understanding in what's behind the tool your using (probably more than any computer-aided-field)... but sometimes our job force us to be less academic.

I hope someone could solve your problem, sorry for the OT.

Daniele
danvica is offline   Reply With Quote

Old   March 12, 2012, 03:52
Default Stability of OF
  #4
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
Hello Danielle,

There are several indices that the solution you have is not close enough to the reality. First is, when the error is getting close to 1, the error estimates (in log, maximum of final error estimate for each field, for each time step)

Another is phase fraction, when you calculates multiphase problem. The phase fraction should be between 0 and 1. All above and below means stability problem and possible error.

The main problem is to understand that CFD is for verification, it has error which is calculable... without real experiment verification, it simply isn't possible to use any results.

When the calculation is problematic, you can decompose the problem and try to run simpler calculations to isolate it and deal with it. When you don't know, what next, google, read wiki, read the forum here and believe in the start, there are only few problems, nobody solved and posted before you.

And of course post your problems and tested solutions (succesfull or not) and sooner or later, you will get the answer.

Martin.
darai is offline   Reply With Quote

Old   March 16, 2012, 15:44
Default
  #5
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
Martin,
You should probably try the most recent version of multiphaseEulerFoam in the 2.1.x git repo. This solver was still 'in development' at the time of the 2.1.0 release and some important changes have been made subsequently which are reflected in the most recent version in the repo. I would be very curious to hear if you see the same problems in the updated solver.
-Kent
kwardle is offline   Reply With Quote

Old   March 27, 2012, 08:20
Default New version
  #6
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
Thanks Kent for your post,
We tried newer version and the solution is much better. It still isn't perfect, but well... better is better.
So thanks again,
- Martin
darai is offline   Reply With Quote

Old   April 18, 2012, 15:19
Default
  #7
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
FYI, there have been more updates to multiphaseEulerFoam which are currently in 2.1.x. The phase conservation should be much improved. Also there was an issue with virtual mass which seems to have been solved.
kwardle is offline   Reply With Quote

Old   April 24, 2012, 08:22
Default mass conservation problem persist
  #8
Member
 
Petr Furmanek
Join Date: Jan 2012
Location: Prague, Czech Republic
Posts: 60
Rep Power: 5
petr.f. is on a distinguished road
Hi all,

I've taken over Martins work and I'm doing more experiments with multiphaseEulerFoam. The damBreak4Phase_fine works with the default settings (i.e. first order Euler in time, endTime 6 sec). However, as we've previously ran into the problems in nearly stabilised state, I've tried to carry out the computation til 20 sec (with 2nd order backward in time) and discovered a problem totaly opposite to the one mentioned in Martin's first post. The mass is not vanishing any more, but there seems to be some strange "rain" boundary condition on the top boundary of the tank. See the attached figures - the effect begins to appear around the 8th second of the computation and by the 19th second the tank is almost full... Any idea what could be wrong?

Petr.
Attached Images
File Type: jpg multiphaseE-EF.0001_edited.jpg (16.5 KB, 29 views)
File Type: jpg multiphaseE-EF.0007_edited.jpg (11.9 KB, 28 views)
File Type: jpg multiphaseE-EF.0008.jpg (18.2 KB, 34 views)
File Type: jpg multiphaseE-EF.0019.jpg (10.3 KB, 33 views)
petr.f. is offline   Reply With Quote

Old   April 24, 2012, 11:29
Default
  #9
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 195
Rep Power: 10
kwardle is on a distinguished road
Petr,
Yes, very strange indeed, but I have seen this before. Are you using the standard BC setup in the damBreak tutorial? As I recall, I only saw this when I had been simulating a closed domain and had mistakenly set the phase velocities U* as zeroGradient on one of the walls rather than slip. Assuming you are not doing that, but are using the standard 'atmosphere' top boundary, then I think this can be helped by adding the 'phi' argument to the inletOutlet types for each of the alphas, e.g. add 'phi phiwater;' to alphawater, and so on for the other phases. Give this a try and let me know if it helps.
Regards,
Kent
kwardle is offline   Reply With Quote

Old   April 25, 2012, 01:57
Default
  #10
Member
 
Petr Furmanek
Join Date: Jan 2012
Location: Prague, Czech Republic
Posts: 60
Rep Power: 5
petr.f. is on a distinguished road
Thanks for the reply. I will try your recomendations and let you know. However, the puzzling thing is that this behaviour appears only when using the 2nd order implicit backward scheme for time derivatives (this was the only change I made to the original files). With 1st order explicit Euler everything works perfectly.

Last edited by petr.f.; April 25, 2012 at 02:32.
petr.f. is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
strange pressure behaviour with symmetricPlane boudary condition - interFoam duongquaphim OpenFOAM Running, Solving & CFD 10 August 20, 2013 14:00
Strange behaviour when using LienCubicKE and NonlinearKEShih hani OpenFOAM Running, Solving & CFD 20 March 6, 2013 11:06
Strange boundary behaviour using interFoam Andrea_85 OpenFOAM 11 January 22, 2013 16:09
Strange behaviour because of contact angle (interfoam) Kim123 OpenFOAM Running, Solving & CFD 0 January 12, 2011 11:16
strange behaviour of GGI in parallel on axis symmetrical case A.Devesa OpenFOAM Running, Solving & CFD 0 April 6, 2010 03:58


All times are GMT -4. The time now is 03:12.