
[Sponsors] 
May 6, 2014, 23:13 
Question on transient simulation in OpenFOAM and FLUENT

#1 
New Member
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 5 
Dear all:
Recently I'm trying to use OpenFOAM to simulate transient incompressible flow, and have some questions to inquire. I know that in FLUENT, for transient flow, iterations are required within each time step, to confirm the result can converge at the end of the current time step. The default value is 20, which means if the result cannot converge within 20 iterations, the solver will march into next time step. This is normally how the transient solver works in my mind. However, when perform transient simulation in OpenFOAM, using either PISO or PIMPLE, it seems that no iteration is required within one time step (Of course iterations are still required when solving equations, that's not my question). This can be seen clearly from one section of the log file: Code:
Courant Number mean: 0.279317 max: 0.999569 deltaT = 0.00175747 Time = 5.92794 DILUPBiCG: Solving for Ux, Initial residual = 8.03872e05, Final residual = 3.01259e10, No Iterations 4 DILUPBiCG: Solving for Uy, Initial residual = 7.47932e05, Final residual = 2.18265e10, No Iterations 4 DILUPBiCG: Solving for Uz, Initial residual = 5.96536e05, Final residual = 1.09994e10, No Iterations 4 GAMG: Solving for p, Initial residual = 0.000123055, Final residual = 4.66822e10, No Iterations 10 time step continuity errors : sum local = 1.54552e12, global = 2.47586e13, cumulative = 4.13283e11 GAMG: Solving for p, Initial residual = 2.08618e05, Final residual = 6.33155e10, No Iterations 8 time step continuity errors : sum local = 2.09623e12, global = 2.88986e13, cumulative = 4.16173e11 DILUPBiCG: Solving for epsilon, Initial residual = 2.95649e05, Final residual = 9.94966e11, No Iterations 4 DILUPBiCG: Solving for k, Initial residual = 4.52894e05, Final residual = 6.86864e10, No Iterations 4 ExecutionTime = 3449.02 s ClockTime = 3453 s Courant Number mean: 0.279319 max: 0.999571 deltaT = 0.00175747 Time = 5.9297 DILUPBiCG: Solving for Ux, Initial residual = 8.04511e05, Final residual = 2.77023e10, No Iterations 4 DILUPBiCG: Solving for Uy, Initial residual = 7.47824e05, Final residual = 2.18558e10, No Iterations 4 DILUPBiCG: Solving for Uz, Initial residual = 5.97415e05, Final residual = 1.09586e10, No Iterations 4 GAMG: Solving for p, Initial residual = 0.000123775, Final residual = 5.54077e10, No Iterations 10 time step continuity errors : sum local = 1.83445e12, global = 2.88968e13, cumulative = 4.13283e11 GAMG: Solving for p, Initial residual = 2.07948e05, Final residual = 5.90437e10, No Iterations 8 time step continuity errors : sum local = 1.95485e12, global = 2.66983e13, cumulative = 4.15953e11 DILUPBiCG: Solving for epsilon, Initial residual = 2.95488e05, Final residual = 9.23568e11, No Iterations 4 DILUPBiCG: Solving for k, Initial residual = 4.52872e05, Final residual = 4.31262e10, No Iterations 4 ExecutionTime = 3449.6 s ClockTime = 3453 s May I ask why this happens? Actually the same situation happens in the "pitzDaily" case in the tutorial pimpleFoam directory, so I think maybe this is some mechanism exist in OpenFOAM. Can anyone help me to explain it? Thank you very much! 

May 7, 2014, 17:12 

#2 
Senior Member
Artur
Join Date: May 2013
Location: Southampton, UK
Posts: 299
Rep Power: 12 
I don't know about how Fluent handles things I'm afraid. However, to solve the entire problem several times at one time step using PIMPLE you may increase the nOuterCorrectors in fvSolution to whatever value you wish. If you set it to 1 the solver will operate in PISO mode which, as you've pointed out, only iterates over each equation a number of times.
There is a substantial amount of discussion on this forum as to how the two algorithms differ, see for instance these threads: http://www.cfdonline.com/Forums/ope...algorithm.html http://www.cfdonline.com/Forums/mai...mplework.html Peace, A 

May 8, 2014, 01:29 

#3  
New Member
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 5 
Quote:
Thank you very much for your reply and the information. It is very helpful. According to the references and CFD books, PISO is a kind of noniterative method for transient problem. I also found in this thread: http://www.cfdonline.com/Forums/ope...algorithm.html It seems that if the nOuterCorrectors is set to 1, the PIMPLE becomes identical to PISO. Therefore, if I am not wrong, maybe the pisoFoam corresponds to the noniterative PISO scheme in FLUENT, and pimpleFoam correspdons to the iterative PISO scheme in FLUENT, which providing the capability to perform outer iterations. Regards, Nick 

May 8, 2014, 03:22 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 20 
I was wondering the same things when switching from Fluent to OpenFoam, but you are right.
pisoFoam is the same as if you set (in Fluent) the maximum number of iterations per time step to 1. PimpleFoam with any number of outer iterations is the same as a regular transient simulation in Fluent. I did not check, whether piso=piso and simple=simple in Fluent and OpenFoam, but what you write is generally right.
__________________
The skeleton ran out of shampoo in the shower. 

May 8, 2014, 22:30 

#5  
New Member
Liu Jun
Join Date: Mar 2014
Posts: 3
Rep Power: 5 
Quote:


Tags 
fluent, iteration, transient 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Possible Bug in pimpleFoam (or createPatch) (or fluent3DMeshToFoam)  cfdonline2mohsen  OpenFOAM  3  October 21, 2013 09:28 
FLUENT or OpenFoam for Particlesurface intercation simulation?  Amir1  Main CFD Forum  0  May 10, 2013 17:15 
Question: BC openFOAM vs. FLUENT  oehmu  OpenFOAM  2  December 14, 2010 17:14 
Fluent elbow in Openfoam  chemeng  OpenFOAM  1  January 21, 2010 04:52 
OpenFOAM vs Fluent for cylinder at Re%3d150  lr103476  OpenFOAM Running, Solving & CFD  40  December 18, 2008 10:09 