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

interFoam: timestep / mesh / PISO nCorrector dependency

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 21, 2010, 10:09
Default interFoam: timestep / mesh / PISO nCorrector dependency
  #1
Senior Member
 
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 164
Rep Power: 7
linch is on a distinguished road
Hi guys,

as an interFoam introduction I wanted to recompute a couple of DNS calculations of falling droplet in a closed channel from some paper.

Trying to do that I experienced following difficulties: decreasing the time step or enlarging of mesh cell (Courant number was kept under 0.5 in all simulations) cause a significant (almost linear) increase of droplet acceleration and consequently produces an absolutely different solution. Even more incomprehensible for me is the fact, that an increasing the PISO correction loops number (nCorrectors option in fvSolution) has the same effect on the solution. E.g. I get approximately the same solution by halving the time step size and doubling the nCorrectors number simultaneously.

Does it mean the solution are not converged? So, I'm sure I do something wrong, but I don't know what exactly:-) As usual hoping for your help!

Regards,

P.S. here are some examples of time step & nCorrectors variation:http://www.file-upload.net/download-...hment.zip.html
Both cases with (deltaT = 0.005 & nCorrectors = 3) and (deltaT = 0.01 & nCorrectors = 6) deliver equal results. The free fall time in these both case is only a half as in the case with (deltaT = 0.01 & nCorrectors = 3).
linch is offline   Reply With Quote

Old   October 21, 2010, 10:34
Default
  #2
Senior Member
 
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 164
Rep Power: 7
linch is on a distinguished road
When I go for adaptive time step with a target Courant number of 0.5 (as it is the case in the dam break tutorial), the droplet becomes two times slower again: http://www.file-upload.net/download-...eStep.zip.html

So is the Courant number of 0.5 way too large for the interFoam?
linch is offline   Reply With Quote

Old   October 21, 2010, 17:40
Default
  #3
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 413
Rep Power: 14
santiagomarquezd will become famous soon enough
Illya, I was about to start a new thread relative to this topic, but I found yours, thanks for share your experiences. I'm having the same problems. I run an sloshing problem last year and now I'm trying to reproduce the results of the rising bubble benchmark proposed by Hysing et. al. (http://mox.polimi.it/it/progetti/pub...ni/23-2008.pdf). In both cases I had to decrease the timestep a lot to match a correct velocity prediction. Now I'm trying to see the effect of to set o not to set the momentum predictor and the PISO iteration, you gave us some insight. What I can't figure too is the reason of this behavior, following Issa PISO, corrections beyond 3 are unnecessary, but your examples show that this isn't the case in FOAM.

Let's continue sharing our results.

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Post-doctoral Fellow
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   October 22, 2010, 05:41
Default about the time step and accuracy of interFoam simulation
  #4
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 7
kumar is on a distinguished road
Hello,
I have also noticed the difference of velocity for a case with CFL-0.2 and CFL -0.005.But I use LES for turbulence modeling. I am still in the process of validating this difference by performing a DNS case .

Anyhow in the mean time I came across this article.
Flux-blending schemes for interface capture in two-fluid flows , International Journal of Heat and Mass transfer, 52 (2009) , 5547-5556.

In this paper they compare the numerical error with the CFL number for different interface capturing schemes. They also propose a scheme for improving the accuracy. The schemes include CICSAM and HRIC.

I wanted to know if something similar to that can be done in interFoam to improve its accuracy for reasonable CFL number.

If you dont get hold of the paper, give me your email I.D , I can send it to you.

bye
regards
K.Suresh kumar
kumar is offline   Reply With Quote

Old   October 22, 2010, 09:52
Default
  #5
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 413
Rep Power: 14
santiagomarquezd will become famous soon enough
Kumar, thanks for the reference, I downloaded from the digital library. I was wondering how to cope this problem in FOAM too. I read the article briefly and there are some differences with FOAM,

1. The VOF evolution equation is different from FOAM.
2. No further reconstruction schemes are used in FOAM, such as CICSAM.
3. FOAM applies a FCT technique over nonlinear flux in VOF equation, while only NVD/TVD schemes are used in the blending part in the paper.

If I understood well you are suggesting that problems in velocity prediction are due div schemes?

I'll read the paper in deep I try to imagine how to apply these concepts in interFoam, nevertheless I think we have to finish the analysis with respect PISO implementation, due strange behavior we post previously. BTW, I changed div schemes in FOAM, using less diffusive ones and no differences were found.

Keep in touch.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Post-doctoral Fellow
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   October 26, 2010, 04:58
Default
  #6
Senior Member
 
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 7
kumar is on a distinguished road
Hi santiago,
Thanks for the reply and suggestions. I think you are correct that the approach in interFoam is different form the one used in the paper.

But I was just wondering if there is a way to some how have a better prediction of velocity for reasonable CFL numbers like 0.2 or 0.5. Is it possible to do some diffusion correction as done in Level set methods, like the one done in the paper

" Marangoni effects caused by contaminants adsorbed on bubble surfaces" JFM 2010, vol 647

I mean along with the interface compression step, if we add another intermediate step for diffusion correction, do you think it would help.

Just a suggestion, probably you have been looking into the source of interFoam more deeply than I have been looking. So you could suggest me if it is a good idea to do it.

bye
regards
K.Suresh kumar
kumar is offline   Reply With Quote

Old   October 26, 2010, 08:12
Default
  #7
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 413
Rep Power: 14
santiagomarquezd will become famous soon enough
Kumar, thanks again for the suggestions, I'm reading the paper from IJHMT and its references, and I'm learning a lot, thanks for the reference, on the other hand, changes I made in settings for interFoam run didn't give new results, now a new case is running with a small timestep. CFL beyond 0.2 would be marvelous, but I never could obtain good velocity predictions at these values. I'm still trying to figure out what is the source of this problems, would be necessary to design a test to detect whether it is caused by momentum equation of by alpha equation or even worst by a combination of both.
Actually the main drawback of alpha equation is nevertheless it is assembled by standard divergence schemes plus, eventually, interfaceCompression, the solution is driven by MULES which is an FCT limiter. This limiter controls the amount of anti-diffusive flux that is applied to a bounded flux created by upwind, then I don't how much of the initial proposal by TVD/NVD or whatever you want to use for assemble the alpha equation remains after applying the MULES::limiter.

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Post-doctoral Fellow
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   November 19, 2010, 11:07
Default
  #8
Senior Member
 
Pawel Sosnowski
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 105
Rep Power: 8
psosnows is on a distinguished road
Hello everybody,

lately we performed several tests regarding dependency of PISO algorithm on the number of corrections.

The tests were performed firstly on a plane channel flow. We used slightly modified icoFoam solver (with added forcing term), and performed DNS simulation of turbulent flow.

As most of you probably already know, the increasing number of PISO corrections over 2 does not increase the precision of the solution.

But- what you may find interesting, the increasing number of corrections does increase stability of the method! This observation was confirmed using unstructured grid on a non-trivial geometry. The case with 2 corrections blew up after some time, while the one with greater number of corrections was able to run further (of course the cases differed only with number of corrections).

An open question is- how to determine the right number of PISO corrections for a specific case to be stable? Right now- one has to do it empirically.

Summing up, additional PISO corrections (over 2) increase stability of the method.

Best,
Pawel
psosnows is offline   Reply With Quote

Old   November 22, 2010, 10:17
Default
  #9
Senior Member
 
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 6
stevenvanharen is on a distinguished road
This is interesting, just my thoughts:

  • Issa compares to first order implicit Euler, his statement for the number of PISO-correctors to be used is based on an order-of-accuracy comparison between first order implicit Euler and the PISO algorithm. Keep this in mind if you use CN or backward Euler in OF.
  • Order of accuracy says noting about absolute error, so the number of PISO-corrections needed could indeed change with different time-step
  • for DNS: continuity error decreases with increasing corrector steps. Ask yourself: Is your mass conserved to machine accuracy?
  • in my experience the CPU-time does not necessarily increase with more corrector steps (the total number of iterations stays the same or even decreases) If it comes for free, or even speeds up your calculation, why not use it?
To put this in perspective, I use 4 PISO-corrections for DNS. Happy iterating!
stevenvanharen is offline   Reply With Quote

Old   November 23, 2010, 02:59
Default
  #10
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,880
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by santiagomarquezd View Post
What I can't figure too is the reason of this behavior, following Issa PISO, corrections beyond 3 are unnecessary, but your examples show that this isn't the case in FOAM.
Hi Santiago,

I would not take that "3 correctors" as something written in stone. The actual number of correctors depends on your mesh quality, on the case you are simulating, and on the set of equations you are trying to couple.

This said, I am not particularly fond of using PISO without outer corrections, because it does not ensure anything about the convergence of the equations, and this is particularly true in multiphase flows, where the coupling is more complex than in single-phase flows.

P.S (for linch). It would be so useful to have a case to look at when you report a problem ;-)

Best,
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.

Last edited by alberto; November 23, 2010 at 03:11. Reason: Added comment
alberto is offline   Reply With Quote

Old   November 23, 2010, 03:04
Default
  #11
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,880
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by psosnows View Post
But- what you may find interesting, the increasing number of corrections does increase stability of the method! This observation was confirmed using unstructured grid on a non-trivial geometry. The case with 2 corrections blew up after some time, while the one with greater number of corrections was able to run further (of course the cases differed only with number of corrections).

An open question is- how to determine the right number of PISO corrections for a specific case to be stable? Right now- one has to do it empirically.
Check the behaviour of the continuity error and of the residuals on the pEqn and (adding some bit of code) of the UEqn.

If you notice an improved stability of the solution with more corrector, most probably it means that with less corrector you do not achieve perfect coupling of the equations

Best,
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   November 23, 2010, 16:26
Default
  #12
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 413
Rep Power: 14
santiagomarquezd will become famous soon enough
Quote:
Originally Posted by alberto View Post
Hi Santiago,
I would not take that "3 correctors" as something written in stone. The actual number of correctors depends on your mesh quality, on the case you are simulating, and on the set of equations you are trying to couple.

This said, I am not particularly fond of using PISO without outer corrections, because it does not ensure anything about the convergence of the equations, and this is particularly true in multiphase flows, where the coupling is more complex than in single-phase flows.
Best,
Hi Alberto, thanks for your insights, I'll have your comments in mind. Actually my advisor is about to face the emulation of icoFoam and interFoam and we'll focused on this matter.

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Post-doctoral Fellow
Research Center for Computational Mechanics (CIMEC) - CONICET/FICH-UNL
T.E.: 54-342-4511594 Ext. 1005
Güemes 3450 - (3000) Santa Fe
Santa Fe - Argentina
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   December 2, 2010, 08:49
Default
  #13
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,528
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
Hi Alberto

I have a question related to the following comment from your post #10:

Quote:
Originally Posted by alberto View Post
Hi Santiago,
This said, I am not particularly fond of using PISO without outer corrections, because it does not ensure anything about the convergence of the equations, and this is particularly true in multiphase flows, where the coupling is more complex than in single-phase flows.
When you are saying outer corrections, then you are talking about something similar to what is done in pimpleFoam?

Thanks for any insights,

Niels
ngj is offline   Reply With Quote

Old   December 2, 2010, 12:38
Default
  #14
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,880
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Hi Niels,

yes I meant something like PIMPLE or unsteady SIMPLE.

My point is that the convergence of all the equations should be ensured at each time-step (It is not so easy in some case to have it in only one iteration, even with small time-steps).

Best,
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   December 3, 2010, 07:53
Default
  #15
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,528
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
Hi Alberto

Thanks, I will take a look at it and report back whether or not it does improve on the interFoam approach.

Best regards,

Niels
ngj is offline   Reply With Quote

Old   January 10, 2011, 02:22
Default free fall time
  #16
Ueb
New Member
 
Konrad Uebel
Join Date: Jul 2010
Location: Freiberg
Posts: 2
Rep Power: 0
Ueb is on a distinguished road
We have the same problems with diverging free fall times in interFoam depending on different CFL numbers. We found out that the solver predicts the free fall correctly if one set viscosities to zero. Then with almost every CFL number (not too high, because of divergence) the solver predicts the correct free fall time.
I want to use different interpolation schemes and do some tests and comparison. In fact FLUENT has the same problems, but not that worse.

regards Ueb
Ueb 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
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 3 October 27, 2013 05:34
interFoam with irregular Mesh luther OpenFOAM 9 August 14, 2009 07:43
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55
Mesh Mignard FLUENT 2 March 22, 2000 05:12
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 10:09


All times are GMT -4. The time now is 12:45.