
[Sponsors] 
June 6, 2013, 10:31 
interfoam performance

#21 
Member
Join Date: Mar 2013
Posts: 96
Rep Power: 6 
Sponsored Links
I have a similar problem whit the performance of inteFoam. My problem concern a circular pipe filled with liquid and closed to both extremity. At initial time the right wall of the pipe is opened and gas allowing gas to go inside and liquid outside. My aim is to validate OpenFOAM for this kind of problem so I compared its performance with Fluent. The comparison seems very good but there is a strange difference. In my simulations I use a fixed Courant number and adaptive time step. The difference between is that Fluent give me a deltaT around 10e04 while OpenFOAM give me a deltaT around 10e6.So the simulation run very slow with OpenFOAM...Why this different behavior?There i a way to speed simulation? I obtain a little accelerate through decreasing tolerance but I would obtain i larger time step if possibile and kwon why there is this difference between two code. thanks to all 

Sponsored Links 
June 6, 2013, 10:42 

#22 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 217
Rep Power: 14 
If you are using the solver settings from the tutorials, you may have the maxCo and maxAlphaCo both set to 0.5. I typically will push these to 2.0 and 1.0 (at least) and then set nAlphaSubCycles to 5 in fvSolutions. Depending on how you have configured the BCs what is likely happening is that you are getting high velocities in the gas phase (probably inflow on a pressure outlet) that are driving down the dt. Setting maxCo to a higher value than maxAlphaCo will let the time step be controlled more by the velocities near the interface.


June 6, 2013, 11:03 

#23 
Member
Join Date: Mar 2013
Posts: 96
Rep Power: 6 
Thanks for your reply
I increase my Courant number to 0.8 in order to obtained a faster solution but with this Co I obtained a fluctuating solution. In fact, for this kind of problem the Courant number must not be more than 0.5, other experience says that courant number must not be more than 0.35 so I set its to 0.25. Regarding the velocity fields it seems ok. With the calculated velocity the courant number should be about 10e04 but is 10e06 

June 6, 2013, 11:09 

#24 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 217
Rep Power: 14 
This precisely why you use subtime stepping on alpha. So if you set maxAlphaCo to 0.5 and nAlphaSubCycles is 3 then you have a Co per alpha step of 0.5/3 = 0.167. This is why I say use 1.0/5 = 0.2. You could push it to 1.5/5 = 0.3 and still probably be OK.


June 6, 2013, 11:22 

#25 
Member
Join Date: Mar 2013
Posts: 96
Rep Power: 6 
I set nAlphaSubCycles=2.
Two questions about you reply. 1)There is a way to verify if the real Courant numeber is Co/nAlphaSubCycles? Beacause in the output file the max Courant number remain fixed to 0.25 and not to 0,1225 2)I know that nAlphaSubCycles are the subcycle inside alpha equation. Through subcycle we have a more stable solution without incresing time step. Why nAlphaSubCycles should have to change Courant number? 

June 6, 2013, 11:46 

#26 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 217
Rep Power: 14 
So when you say Courant number are you meaning maxCo or maxAlphaCo? interFoam should print out both values.
Here, "Courant Number" is limited by the maxCo setting in controlDict and "Interface Courant Number" is limited by maxAlphaCo. In the VOFstyle algorithm, only the Co at the interface is the problem. The Co has to be small enough that it takes ~4 time 'steps' for the interface to travel through a cell. So it comes from the local mesh size and local velocitynot sure if you are taking that into account when calculating by hand. Since the solution of the volume fraction transport will be the limiting thing on time step size AND since all the computational time is spent in the pressure solve with the alpha solve being relatively cheap, you solve the alpha eqn multiple times with smaller timesteps for every one pressure solve. This is nAlphaSubCycles. Anyway, if you have nAlphaSubCycles set to 2 and you put the maxAlphaCo to 0.8 then you are having and effective max Co on each alpha solve of 0.4 which is unstable as you have seen. In any case, the value printed at each timestep is the OVERALL Co so to get the Co on a given subtime step of alpha you divide this by nAlphaSubCycles. It changes Co because the time step size on each subcycle step is dt/nAlphaSubCycles. If you really want to check what the Co field looks like at any point in time, you would have to tweak the solver or add in a functionObject. One other thing to keep in mind is that things get crazy (interface oscillations and parasitic currents) if cAlpha is greater than 1.0 (it may be 2.0 in some of the old tutorial cases). Hope this helps. Kent 

June 6, 2013, 12:23 

#27 
Member
Join Date: Mar 2013
Posts: 96
Rep Power: 6 
when I talking about Courant number I mean maxCo.
So you suggest to set maxCo=0.9 (explicit solver) and maxAlphaCo=2 with nAlphaSubCycles=10? thanks you very much for your replies 

June 6, 2013, 12:43 

#28 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 217
Rep Power: 14 
No, I suggest:
maxCo=2.0 maxAlphaCo=1.0 nAlphaSubCycles=5 

June 6, 2013, 13:00 

#29 
Member
Join Date: Mar 2013
Posts: 96
Rep Power: 6 
I understand why I must set maxAlphaCo=1.0 and nAlphaSubCycles=5.
last question: interFoam is an explicit solver so maxCo have to set <1,why you suggest maxCo=2.0? the nAlphaSubCycles acts also in p and U equations?I thinked no 

August 22, 2013, 03:38 

#30 
Member
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 6 
Hi all,
Could anyone please explain why we use MULES in alpha equation and not solve method? Thanks, Hrushi 

August 22, 2013, 03:53 

#31 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,251
Rep Power: 23 
The volume fraction equation has special requirements with regard to boundedness, conservation and diffusivity. Thus we use a special algorithm to solve it.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. 

August 22, 2013, 04:03 

#32 
Member
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 6 
Hi Anton,
Thank you for a quick reply. I have couple of follow up questions: 1. Do you know any reference that discusses these special requirements? I have read Rusche's thesis but did not find anything for this. 2. Will these requirements hold true when we change the range of fraction from 0:1 to 1:1? Thanks Hrushi 

August 22, 2013, 05:36 

#33 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,251
Rep Power: 23 
Rusche's thesis does contain a brief section on how to deal with the issues  3.2.6. Any paper dealing with the VoF method or how to improve it likely has information on the subject. In short:
1. Conservation  As an example if you have a bubble, you do not want the bubble volume to grow or shrink. It may significantly change the outcome of your simulation. 2. Boundedness  since all material properties are interpolated between the two phases, unboundedness can very quickly lead to divergence (e.g. due to negative density) 3. Diffusivity  Numerical diffusivity will eventually get rid of your fluid interface if not dealt with properly. Of course that's not acceptable for immiscible fluids.
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. 

August 22, 2013, 08:51 

#34 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 430
Rep Power: 17 
Well, solve with the proper advection TVD schemes should also do the work. In fact TVD schemes were designed to do exactly that. The problem is that, in practice, this is only true in 1D not in multidimensions, in this case FCT based schemes behave better. I discuss the topic in my PhD. thesis, that is provided in my user page at openfoamwiki.net: http://openfoamwiki.net/index.php/User:Santiagomarquezd
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 Last edited by wyldckat; May 24, 2016 at 17:47. Reason: updated link 

August 22, 2013, 22:24 

#35 
Member
Hrushi
Join Date: Jan 2013
Posts: 58
Rep Power: 6 
Hi Anton and Santiago,
Thank you for your quick reply. Really appreciate it. I am trying to solve a modified alpha equation with interfoam solver. I have no compression velocity and a chemical potential term in my alpha equation. I could not get any results with solve method, which is why I posted the question. Yesterday, I tried solving the alpha equation using mules. for (int aCorr=0; aCorr<nAlphaCorr; aCorr++) { surfaceScalarField phiAlpha (fvc::flux(phi,alpha1,alphaScheme)); /* solve ( fvm::ddt(alpha1)+ (fvc::div(phiAlpha))  fvc::div(diffflx) );*/ MULES::implicitSolve(geometricOneField(), alpha1, phi, phiAlpha, volScalarField("Sp",mobility*fvc::laplacian(G)), zeroField(), 1, 0); rhoPhi = phiAlpha*(rho1  rho2) + phi*rho2; } But my output says that I have maximum of alpha1 more than 1 at the start, which gradually reaches one but still stays more than 1 at equilibrium. Due to this, my results are really weird, and I do not know how to proceed. Any ideas? Thanks, Hrushi 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Superlinear speedup in OpenFOAM 13  msrinath80  OpenFOAM Running, Solving & CFD  18  March 3, 2015 06:36 
How to write k and epsilon before the abnormal end  xiuying  OpenFOAM Running, Solving & CFD  8  August 27, 2013 15:33 
Differences between serial and parallel runs  carsten  OpenFOAM Bugs  11  September 12, 2008 11:16 
AMG versus ICCG  msrinath80  OpenFOAM Running, Solving & CFD  2  November 7, 2006 16:15 
unsteady calcs in FLUENT  Sanjay Padhiar  Main CFD Forum  1  March 31, 1999 12:32 
Sponsored Links 