
[Sponsors] 
interFoam: timestep / mesh / PISO nCorrector dependency 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 21, 2010, 10:09 
interFoam: timestep / mesh / PISO nCorrector dependency

#1 
Senior Member
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 176
Rep Power: 16 
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.fileupload.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). 

October 21, 2010, 10:34 

#2 
Senior Member
Illya Shevchuk
Join Date: Aug 2009
Location: Darmstadt, Germany
Posts: 176
Rep Power: 16 
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.fileupload.net/download...eStep.zip.html
So is the Courant number of 0.5 way too large for the interFoam? 

October 21, 2010, 17:40 

#3 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 23 
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/232008.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. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

October 22, 2010, 05:41 
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: 17 
Hello,
I have also noticed the difference of velocity for a case with CFL0.2 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. Fluxblending schemes for interface capture in twofluid flows , International Journal of Heat and Mass transfer, 52 (2009) , 55475556. 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 

October 22, 2010, 09:52 

#5 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 23 
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. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

October 26, 2010, 04:58 

#6 
Senior Member
Suresh kumar Kannan
Join Date: Mar 2009
Location: Luxembourg, Luxembourg, Luxembourg
Posts: 129
Rep Power: 17 
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 

October 26, 2010, 08:12 

#7 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 23 
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 antidiffusive 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. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

November 19, 2010, 11:07 

#8 
Senior Member
Pawel Sosnowski
Join Date: Mar 2009
Location: Munich, Germany
Posts: 105
Rep Power: 18 
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 nontrivial 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 

November 22, 2010, 10:17 

#9 
Senior Member
Steven van Haren
Join Date: Aug 2010
Location: The Netherlands
Posts: 149
Rep Power: 15 
This is interesting, just my thoughts:


November 23, 2010, 02:59 

#10  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
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 singlephase flows. P.S (for linch). It would be so useful to have a case to look at when you report a problem ;) Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. Last edited by alberto; November 23, 2010 at 03:11. Reason: Added comment 

November 23, 2010, 03:04 

#11  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
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 Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 23, 2010, 16:26 

#12  
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 23 
Quote:
Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

December 2, 2010, 08:49 

#13  
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,900
Rep Power: 37 
Hi Alberto
I have a question related to the following comment from your post #10: Quote:
Thanks for any insights, Niels 

December 2, 2010, 12:38 

#14 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
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 timestep (It is not so easy in some case to have it in only one iteration, even with small timesteps). Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

December 3, 2010, 07:53 

#15 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,900
Rep Power: 37 
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 

January 10, 2011, 02:22 
free fall time

#16 
New Member
Konrad Uebel
Join Date: Jul 2010
Location: Freiberg
Posts: 2
Rep Power: 0 
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 

October 31, 2019, 04:24 

#17  
Senior Member
Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 7 
Quote:
I am wondering is there any criteria or rule of thumb for the setting of ncorrectors. In my DNS simulations, the ncorrectors is 2 and I have no idea if it is enough for current situation. In my case, the residuals of P and U are a little lower than 0.01 but they are rising slowly. I don't know how to change this tendency. Thank you. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
[ICEM] Negative volume error in hybrid mesh  siw  ANSYS Meshing & Geometry  4  September 3, 2014 05:25 
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 