
[Sponsors] 
why pisoFoam take such a long time to converge? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 14, 2013, 13:38 
why pisoFoam take such a long time to converge?

#1  
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
Hello
I have a PC with 4GB RAM 2 processors.. Ihave run a simulation with pisoFOam and today is 48 hours since i last start.. and still convergence not acheived..!! Can anyone give me a better way to acheive convergence easier with pisoFoam? I am attaching my fv solution just so that you may know what i did.. Quote:
Quote:


October 14, 2013, 15:50 

#2 
Senior Member
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Copenhagen, Denmark
Posts: 1,900
Rep Power: 36 
Good evening,
pisoFoam is intended for transient simulations, which does not necessarily have a steady state solution. Also, to my knowledge, the pisoFoam does not check for the residualControls, which you have in your fvSolution file. For steady state simulations you would probable want to look into e.g. simpleFoam. Kind regards, Niels
__________________
Please note that I do not use the Friendfeature, so do not be offended, if I do not accept a request. 

October 15, 2013, 00:56 

#3 
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
hi..
simpleFoam is not working at all for the case that running... hence am running with pisoFoam, and its working with pisoFoam.. but taking such a long time!!!! 

October 15, 2013, 05:35 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
Is this a transient simulation or steady state?
__________________
The skeleton ran out of shampoo in the shower. 

October 15, 2013, 05:47 

#5  
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
steady state..
Quote:


October 15, 2013, 05:55 

#6 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
You are using the wrong solver. You solve for a transient simulation, timescheme is Euler and your timestep is 0.5ms.
This is not steadystate. 1) Use simpleFoam! Why do you say "simpleFoam is not working at all for the case that running"? SimpleFoam is a steady state solver. 2) Use GAMG solver for pressure. 3) "Linear" discretization doesn't converge very well. You can try some more dissipative scheme (upwind, linearUpwind,...).
__________________
The skeleton ran out of shampoo in the shower. 

October 15, 2013, 05:59 

#7 
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
i already did all that with simpleFoam.. But after 300 timestep my solution crash.. and when i check in paraView, i see my domain as a blueeee one.. ie no velocity has enter... hence why i was soo desperate...


October 15, 2013, 06:01 

#8 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
Then you did it wrong
Post your simple solver settings and then the residuals.
__________________
The skeleton ran out of shampoo in the shower. 

October 15, 2013, 06:03 

#9 
Senior Member
Join Date: Dec 2011
Posts: 111
Rep Power: 19 
You have specified Euler to be used as time integrator, hence your simulation is transient. Period.
Anyways, as others have mentioned, pisoFoam will not obey the residual limits you have specified. It will run until it reaches endTime, no matter how steady the simulation are. If you want a steadystate result then simpleFoam is the one and only solver to use. However, some cases will not converge to a steady state, simply because they are transient by nature. For such cases steady solutions are difficult to obtain, and if you can get one, you are almost certain that it is nonphysical. If your case involves geometries and flow conditions leading to for example vortex shedding, that forces you to use a transient solver if you want physical results. That is just how nature works. (BTW: You can probably get almost any case to converge in steady state by using 1st order upwind schemes (=extreme diffusivity), heavy relaxation and other "stabilizing tricks", but will give you unusable results, so in practice it is not possible...) 

October 15, 2013, 06:04 

#10  
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
simple Solver settings..:
Quote:
Quote:


October 15, 2013, 06:07 

#11  
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
Quote:
Can you please give me an example where the upwind scheme is 1strorder? me i am simulating 10 shapes in a domain..that is all and its in 2D.. so i guess it should converge normally right?? for 12 days i am with this problem..and with pisoFoam its nto crashing..but today is my 3rd day where simulation is running.. so am a bit desperate now... 

October 15, 2013, 06:16 

#12 
Senior Member
Join Date: Dec 2011
Posts: 111
Rep Power: 19 
I guess that probably is just the "upwind" scheme, but I have never used it, as it produces just crap.
Why are you using zero nonorthogonal correctors? Have you tried increasing this value? Why are you only using relaxation for the pressure and not the velocities when running simpleFoam? I would lie to emphasize a few things:


October 15, 2013, 06:24 

#13  
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
my mesh is fine..
From the errors it say.. Quote:


October 15, 2013, 06:26 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
Can you post the residual plot?
1) What happens, if you set "relTol" for the pressure to 1.0e3? Do the residuals change? 2) What happens, if you use some gradient limiter? Such as Code:
gradSchemes { default faceLimited edgeCellsLeastSquares 1; } Code:
... div(phi,k) bounded Gauss upwind;
__________________
The skeleton ran out of shampoo in the shower. 

October 15, 2013, 16:12 

#15 
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
am sorry for late reply.. but for each of the above mentioned points. My solution crash..
Now am worried.... 

October 16, 2013, 05:23 

#16 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
Can you send the whole logoutput? So we can try to find the spot...
__________________
The skeleton ran out of shampoo in the shower. 

October 17, 2013, 14:59 

#17 
Senior Member
izna O'connor
Join Date: Jun 2013
Posts: 143
Rep Power: 12 
hi..afte changing the fv solution and fv schemes.. I obtain a good simulation which i checked..
.. when arriving at 1760 iteration the solution crashed.. and when i checked in paraView.. I obtain a blue domain.. Why such a nice simulation suddenly crash ? 

October 18, 2013, 03:05 

#18 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
You have to share all relevant data, otherwise no one will be able to help you.
1) log output 2) boundary condition files 3) screenshot of your domain with grid. Additionally: It seems you use the kepsilon model. In your fvSolution file you set relaxation factors, but not for kepsilon but for komega. This could be the reason.
__________________
The skeleton ran out of shampoo in the shower. 

October 18, 2013, 04:26 

#19 
New Member
Danesh S
Join Date: Jul 2013
Location: Bochum, Germany
Posts: 27
Rep Power: 12 
Hi all,
I have a question which is close to the topic. Niels said above, that pisoFoam does not check for residualControls. Does that mean, that when running a transient turbulent simulation on pisoFoam, the residual output does not indicate the state of convergence of my simulation? I have the problem at the moment with my simulation. The residual is not dropping anymore, so I have no convergence. (It is LES of Taylor Couette Flow). I use backward time scheme and gauß upwind for U divscheme. My schemes should be fine. After reading this thread I am just worrying, that the solver is not able to produce what I want. Can anybody comment on this? Thx! Danesh 

October 18, 2013, 04:38 

#20 
Senior Member
Join Date: Dec 2011
Posts: 111
Rep Power: 19 
You are correct. pisoFoam does not obey the residual controls. This is because the solution is timeaccurate, i.e. every step is a valid solution of the transient problem. Hence, each step is solved until the specified tolerance level in fvSolution, and not further. Then the time is advances and a new solution is found. The value of the time step is hence important, as the PISOalgorithm cannot handle large time steps.
Remember my earlier comments on fluid flows that generally are transient by nature. I do not feel that you have clearly outruled this issue yet. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 07:20 
Unstabil Simulation with chtMultiRegionFoam  mbay101  OpenFOAM Running, Solving & CFD  13  December 28, 2013 14:12 
same geometry,structured and unstructured mesh,different behaviour.  sharonyue  OpenFOAM Running, Solving & CFD  13  January 2, 2013 23:40 
PisoFoam case terminating  Solo Sails  OpenFOAM Running, Solving & CFD  3  November 29, 2011 08:04 
calculation diverge after continue to run  zhajingjing  OpenFOAM  0  April 28, 2010 05:35 