
[Sponsors] 
June 12, 2012, 04:03 
Is it converging???

#1 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
Hi everyone,
could anyone please guide me if my transint simulation of Homogeneous multiphase problem involving free surface flow is moving in right direction as It is taking too long (almost its 4 th day ), details are as follows; Type : transient Total time : 2e6s time step: 5e10s initial time = 0s High resolution and second order backward euler schemes are employed, loops are (3,10), coefficient loop timescale control with RMS (1E4). My RMS Courant Number and Max courant Number (both are zero after few initial timesteps), that is real concern. Mesh Expansion factor is also in hundreds(200+). Thanks 

June 12, 2012, 10:22 

#2 
Senior Member
Join Date: Jul 2011
Location: Berlin, Germany
Posts: 171
Rep Power: 8 
Hi Danial!
This is a bit too few of information...taking your timestep and iteration loop settings alone i would say 4th day for a max of 40.000 Iterations could be normal depending on: How Many CPU's do you use? How many Elements does your mesh contain? Apart from that do you reach your convergence criterion of RMS 1e4 within the 10 iteration loops? If yes then the first guess is that it is numerically converging. If you always have 10 iteration loops per timestep without reahing rms 1e4 then it is not converged to its final value for the step. On the other hand courant numbers of 0 juest mean that you have very little changements between 2 time steps. Other thing that could slow down your calculation is: How often do you write a transient results file and backup files. Do you write out all variables or selected variables? With a hughe mesh this could take some time. 

June 12, 2012, 19:54 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
I hope you did a sensitivity analysis on your time step size, mesh size and convergence before starting a 4 day simulation. If you did not do a sensitivity analysis then you have just wasted 4 days as you have no doubt got something wrong and will have to run it again.


June 12, 2012, 22:49 

#4 
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 667
Rep Power: 13 
Why such the small timestep size? Courant number of zero too. Not even converging to crappy 1E4 RMS, I'm no expert, but right off the bat I'm thinking your time steps are way too small. Very small time steps can lead to difficult convergence too.
Glenn, how do you do a sensitivity analysis before running the model? 

June 13, 2012, 05:09 
HI above!!

#5 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
AS far as RMS value is concerned in the beginning of solver, yes it started from 1e2 and then gained 1e4 and now after 4 daz it has reached to the value of 1e8 and yes i m writing transient files after 100 steps,this is mesh details;
Global Statistics : Global Number of Nodes = 557411 Global Number of Elements = 530304 Total Number of Tetrahedrons = 2101 Total Number of Prisms = 1136 Total Number of Hexahedrons = 521023 Total Number of Pyramids = 6044 Global Number of Faces = 66578 ghorrocks, i did not do sensitivity analysis before running solver but values were same as were previously used in model which i am replicating with same physics. 

June 13, 2012, 07:32 

#6  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
Quote:


June 13, 2012, 18:44 
Hi

#7 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
Could you please comment if it (highlighted Red) is problematic while initial conditions were Vfi (air) =1, Vfi(liq) = 0.
TIME STEP = 1 SIMULATION TIME = 5.0000E10 CPU SECONDS = 2.376E+01  COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 2.376E+01   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomBulk  0.00  9.8E11  2.2E09  1.0E+06 F   VMomBulk  0.00  9.7E11  4.1E09  1.0E+06 F   WMomBulk  0.00  2.1E03  2.0E02  1.2E01 ok  Massliquid  0.00  1.2E11  5.7E11  0.0E+00 OK  MassAir at25C  0.00  4.2E03  2.0E02  42.3 7.2E03 OK ++++++  HEnergyliquid  0.00  4.4E14  2.1E13  5.2E05 OK  HEnergyAir at25C  0.00  1.3E01  6.4E01  3.9E05 OK  TEnergy  0.00  3.5E04  1.7E03  9.4 5.2E05 OK ++++++  COEFFICIENT LOOP ITERATION = 2 CPU SECONDS = 1.113E+02   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomBulk 99.99  7.3E03  2.7E01  1.0E02 ok  VMomBulk 99.99  7.1E03  2.5E01  1.1E02 ok  WMomBulk 15.11  3.1E02  2.6E01  5.1E03 OK  Massliquid  0.54  6.5E12  1.6E10  0.0E+00 OK  MassAir at25C  0.39  1.6E03  7.8E03  42.3 6.9E03 OK ++++++  HEnergyliquid 99.99  1.0E03  2.4E02  3.7E05 OK  HEnergyAir at25C  0.00  4.1E04  9.2E03  2.7E05 OK  TEnergy  0.00  1.3E06  1.0E05  9.4 3.7E05 OK ++++++ Is anything unusual in following timestep?? It would be great help if someone could mention it.As i am newbie and it looks fine to me. TIME STEP = 1430 SIMULATION TIME = 7.1499E07 CPU SECONDS = 3.326E+05  COEFFICIENT LOOP ITERATION = 1 CPU SECONDS = 3.326E+05   Equation  Rate  RMS Res  Max Res  Linear Solution  ++++++  UMomBulk  1.00  1.4E09  2.8E08  2.7E03 OK  VMomBulk  1.00  1.5E09  3.7E08  2.6E03 OK  WMomBulk  1.00  7.6E09  6.0E08  8.0E04 OK  Massliquid  1.15  1.2E13  2.6E11  0.0E+00 OK  MassAir at25C  1.00  1.8E12  3.7E10  27.3 9.3E03 OK ++++++  HEnergyliquid  1.06  1.4E09  1.7E07  5.6E05 OK  HEnergyAir at25C  1.00  7.4E05  1.9E04  1.3E05 OK  TEnergy  1.01  8.9E06  3.1E05  9.4 5.6E05 OK ++++++ Thanks in advance 

June 14, 2012, 19:13 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
It is common to have the first coeff loop in a time step have strange residuals, which become more normal in the second loop. This is sometimes a sign of too small a time step. How have you determined your time step size?
The fastest way to find a good time step size is to use adaptive timesteps, converging on 35 coeff loops per time step (although 510 for complex multiphase models sometimes helps), in combination with a sensible convergence criteria. Also  if this model includes surface tension you will need very small time steps, so aim for the 35 goal in that case. 

June 14, 2012, 20:00 
HI

#9 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
Infact, i did not calculate timestep by myself but used the same values which i had as a data from previous model which i am replicating. And yes, my model includes surface tension, phase chnage , free surface and heat transfer so its one of the reasons ,I just used the same old values as smaller timesteps.
its almost 6th day...of solver. I should have used adaptive timestepping scheme. 

June 17, 2012, 01:23 
Hi Glen

#10 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
After 8 days of running solver, it just turned out to show some return code error 1, and how can i find error ??? that what possible be the cause of errors? Could you please give some tips???How to find specific error in output file?
Thanks 

June 17, 2012, 19:24 

#11 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
Unfortunately there is no public list of error codes. You will have to post the section of the output file around the error for us to help. Also post the CCL while you are at it.


June 17, 2012, 21:32 
Hi Glen

#12 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
Here are files (CCl details & Error ) with last few iterations befor error occured. I hope it would be helpful.
Thanks 

June 17, 2012, 21:48 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
Your time step is too small. You might need a small time step at the start to get going but you certainly do not need it down the track. Consider using adaptive time steps converging on 35 coeff loops per iteration.
Your material properties with step changes is always going to be numerically unstable. This is always going to be difficult (or impossible) to converge. Do not use expert parameters unless you know you need them. 

June 17, 2012, 22:25 
Hi Glen

#14 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
I am wondering if I can change the time step during transient simulation. Or this option is possible wIth adaptive time stepping scheme.
The other thing about materials properties, what could be the other possible options for defining them? While i have to definfe them as Temp. function to make phase change occur. Thanks 

June 18, 2012, 06:39 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
You can define time step to be a function of anything you like through CEL. But as you probably don't know in advance what the best time step size is then why not just use adaptive time stepping and let it sort itself out for itself?
I am well aware that you have defined material properties as functions of temperature to simulate phase change. Again, you can make them functions of just about anything with CEL, but whether you would want to is another question. 

June 18, 2012, 19:00 
HI Glen

#16 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
As far as , changing time step is concerned, I was asking if i can change it during solver run by any means. I will try the adpative timestepping this time, but how to guess, decrease and increase factor or max/min time step? wild guess?
The other thing about material properties, I guess defining as function of temperature in my case is the only solution, looks reasonable to me. What other possibilities, you think are practical to change the phase? Yes, you are right, CEL can be used to define any thing. Thanks 

June 18, 2012, 19:02 

#17 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
You have to stop and restart to manually change time step.
For adaptive time stepping use 1e20 as the minimum, 1e+20 as the maximum. Only restrict it if you have a good reason to do so. I will not answer your second question as I extensively answered that on a previous thread. 

June 19, 2012, 02:52 
Hi

#18 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
I gave max time step value to 1e+20 but ,it showed global error to minimize this value less than total time value which was ofcourse in micro sec.
I asked about the material properties thing because I did not know ,in what context you were saying that. As, you would have seen in Result file that I had defined them as CEL already. Thanks 

June 20, 2012, 00:05 
HI Glenn

#19 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 7 
I used adaptive scheme for time stepping this time and it seems that it worked but accumulated timesteps were just 100 (is'nt it too short for free surface multiphase); . I got a creepy notice which is botheirng me.
" +  ****** Notice ******   While evaluating   liquidNi.Static Entropy   on domain "splat",   the variable   liquidNi.Temperature   went outside of its lower limit. Its minimum value was   0.0000E+00[K]. The bounds error was handled by clipping.   If this situation persists, consider increasing the table range.  ++ Should I consider it done while "linear solution" values are OK?? And how can we improve solution even though it seems converged, does setting tight value for residuals work well or decreasing initial timestep would help better?? Thanks 

June 20, 2012, 18:37 

#20 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,806
Rep Power: 107 
Did not I say right at the start that the approach you are taking was likely to be numerically unstable? Well, this looks like numerical instability to me.


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Converging Diverging Nozzle in OpenFOAM  danishdude  OpenFOAM Running, Solving & CFD  1  September 15, 2012 00:12 
Wall scale not converging  arunraj  CFX  1  October 3, 2011 17:52 
transient converging, but not steady  PHS  FLUENT  5  July 25, 2011 14:25 
solution not converging for fine mesh..  saurabh.deshpande88  FLUENT  2  February 2, 2010 11:23 
Continuity residual not converging  Chinenye Excel Ogugbue  FLUENT  0  April 28, 2008 02:27 