Register Blogs Members List Search Today's Posts Mark Forums Read

 March 20, 2012, 20:01 convergence unsteady state #1 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 Hi everyone! I am studying a transient state study (unsteady). The first iteration is correct and it achieves a perfect convergence but, the second one... it doesn't converge at all it's that a problem?? is there anything I should change? I decreased the time step from 1E-4 to 1E-05 but it didn't converge whatsoever any idea?? thank you

March 20, 2012, 20:03
#2
Member

andres
Join Date: Sep 2010
Posts: 44
Rep Power: 8
I post a picture so you can figure it out

Hi everyone!
I am studying a transient state study (unsteady).
The first iteration is correct and it achieves a perfect convergence but, the second one... it doesn't converge at all
it's that a problem?? is there anything I should change?
I decreased the time step from 1E-4 to 1E-05 but it didn't converge whatsoever

any idea??

thank you
Attached Images
 convergence.jpg (21.1 KB, 87 views)

March 21, 2012, 14:54
#3
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic I post a picture so you can figure it out Thanks in advance Hi everyone! I am studying a transient state study (unsteady). The first iteration is correct and it achieves a perfect convergence but, the second one... it doesn't converge at all it's that a problem?? is there anything I should change? I decreased the time step from 1E-4 to 1E-05 but it didn't converge whatsoever any idea?? thank you
It's working right. Your definition of "convergence" is the problem.

From 30-40 you can clearly see the solution convergence.

March 21, 2012, 15:01
#4
Senior Member

Join Date: May 2011
Location: Germany
Posts: 130
Rep Power: 8
Quote:
 Originally Posted by cfdhydraulic I post a picture so you can figure it out Thanks in advance Hi everyone! I am studying a transient state study (unsteady). The first iteration is correct and it achieves a perfect convergence but, the second one... it doesn't converge at all it's that a problem?? is there anything I should change? I decreased the time step from 1E-4 to 1E-05 but it didn't converge whatsoever any idea?? thank you
Your residuals (for the second step) do not fall below 1E-3, but that does not mean, that your solution is not converged!

 March 21, 2012, 21:31 #5 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 thanks you all! another question though... if my time step must to be 0.00001 to achieve convergence, I have to iterate 10000 to simulate 1 second!!! and it takes hours!! like... forever! what can I do if want to simulate 5 minutes simulation? what about 1h simulation? To simulate 1 second takes 10 hours or even more... what about 3600seconds???? itīs impossible... is there anything I can do to acelerate this ? THANKS!!

March 21, 2012, 21:39
#6
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic thanks you all! another question though... if my time step must to be 0.00001 to achieve convergence, I have to iterate 10000 to simulate 1 second!!! and it takes hours!! like... forever! what can I do if want to simulate 5 minutes simulation? what about 1h simulation? To simulate 1 second takes 10 hours or even more... what about 3600seconds???? itīs impossible... is there anything I can do to acelerate this ? THANKS!!
it's impossible, unless you redefine space-time. If I drive 120km/h, can I go 120km in less than an hour?

10hrs is not very long. It's not even one day, let it run on a weekend if need be.

You should figure out why you need such a small time step and/or why you need to simulate 1 second. You can use an implicit time advancement scheme, stability is guaranteed, and just use more iterations per time-step. It all depends on what you are really after, and WHY. Why did I need to accomplish both 120km and in less than an hour?

 March 21, 2012, 21:46 #7 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 I need to simulate what's happening in my process after 5 minutes. The time step is 0.0001 to small because I have a good mesh. Good mesh, smaller cells, so small time step. "It all depends on what you are really after, and WHY." well I need to simulate a discharging process of a tank, and it will take around 5 minutes. however, 1 second is more than 10 hours... 300 seconds will be...3000hours... which means that its not possible... any suggestion?

March 21, 2012, 21:57
#8
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic I need to simulate what's happening in my process after 5 minutes. The time step is 0.0001 to small because I have a good mesh. Good mesh, smaller cells, so small time step. "It all depends on what you are really after, and WHY." well I need to simulate a discharging process of a tank, and it will take around 5 minutes. however, 1 second is more than 10 hours... 300 seconds will be...3000hours... which means that its not possible... any suggestion?
with an implicit time advancement, time step does not matter. and use a coarser mesh

 March 22, 2012, 01:39 #9 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 But NITA is only operative in pressure-based cases and I am using density-based... on the other hand, my experience says that the tank that I am simulating will discharge in about 5 minutes but fluent calculations says more than 1 hour... which is impossible... something wrong...

March 22, 2012, 01:42
#10
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic But NITA is only operative in pressure-based cases and I am using density-based... on the other hand, my experience says that the tank that I am simulating will discharge in about 5 minutes but fluent calculations says more than 1 hour... which is impossible... something wrong...

 March 22, 2012, 01:44 #11 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 mmm.... where is this option located in the interface program? i am going to google it I appreciate your help, thanks

March 22, 2012, 01:53
#12
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic mmm.... where is this option located in the interface program? i am going to google it I appreciate your help, thanks
The implicit scheme is the default.

for the pressure based solver, only the implicit formulation is allowed.
for density based, you can choose implicit or explicit formulation.

Again, implicit is default.

March 22, 2012, 17:04
#13
Member

andres
Join Date: Sep 2010
Posts: 44
Rep Power: 8
I am using implicit, as you said, it is default. But time seems to matter...I am going to try with a coarser mesh by changing advanced control parameters "max coarser"
I will let you know

thanks
Attached Images
 Untitled.jpg (47.7 KB, 33 views)

March 22, 2012, 17:42
here is the problem
#14
Member

andres
Join Date: Sep 2010
Posts: 44
Rep Power: 8
Hi! this is the problem...
I need to perform unsteady state study to get info about how a system behaves during 60 seconds.
If I use a time step of 0.00001 it converges perfect and the results seem to be right. But it will take weeks of running calculations... so it doesn't work

If I use another time step... it diverges.
If I use a coarsen mesh, it diverges because of the poor mesh.

I am working with density-based , implicit time advancement , courant number 0.1

any suggestion???
Attached Images
 Untitled.jpg (31.9 KB, 22 views)

March 22, 2012, 18:22
#15
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,819
Rep Power: 26
Quote:
 Originally Posted by cfdhydraulic I am using implicit, as you said, it is default. But time seems to matter...I am going to try with a coarser mesh by changing advanced control parameters "max coarser" I will let you know please see photo, for advise thanks
I recommend you do not touch any of the multigrid parameters unless you know exactly what's going on and after you have already debugged everything that is already wrong. The max coarser levels parameter is not the same as running with a coarser mesh. That control is to control the maximum coarse levels used in the multigrid algorithm. The coarsen by parameter controls the new resolution of the coarse grid by a factor of the original grid. In the multigrid algorithm, all solutions eventually are solved in the finest grid (the actual grid).

By use a coarser grid, I mean to go back and generate a coarser mesh from the start.

Also, for larger time step, you will need more iterations per time step to achieve convergence. If you increased the time step size by a factor of 100, you can guess that it will take 100x iterations to converge (it will be slightly less). It will definitely take more than 1x iterations. You increased the time step by 5 orders of magnitude, of course you should wait more than 40 iterations.

March 23, 2012, 14:07
#16
Member

banty
Join Date: Mar 2012
Posts: 52
Rep Power: 7
In tank depletion problem, Two time scale (Long time scale(to deplete the tank) and small time scale ( to track back wave ). it is vary important to set proper time step to capture( even in implicit solver) the phenomena that u want. U can not capture the phenomena if u are overstepping it.

to know the tank depletion time, u can use density base solver with large time step and large courant no, but for tracking wave, u must use fine mesh and smaller time step (wave should not cross one cell length in single time step.dt = cell length/wave speed)

Quote:
 Originally Posted by cfdhydraulic I am using implicit, as you said, it is default. But time seems to matter...I am going to try with a coarser mesh by changing advanced control parameters "max coarser" I will let you know please see photo, for advise thanks

 March 23, 2012, 14:22 #17 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 actually I would liket to know how long is the discharging time. How long does the tank take to discharge form 300bar to 75 bar but my experience tell me that it will take less than a minute, but Fluent... well.... tell me 4000 seconds or something like that... which is impossible. I believe itīs a problem of setting a proper time step but, I donīt know how to do it as Velocity is unknown as itīs a discharging process. How can I track (calculate) the back wave?

 March 23, 2012, 14:25 #18 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 by the way what is "large" time steps or "small" time steps.... large = 1 second? 5 seconds? 30 seconds??? small = 0.001? 0.00001?

 March 24, 2012, 04:48 #19 Member   banty Join Date: Mar 2012 Posts: 52 Rep Power: 7 its all about relative scaling. u know time to deplete the tank as about 60 sec approx. so 100 or 500 time step(60/100 or 60/500) with implicit methodology should be sufficient otherwise u have problem with solver setting.

 March 24, 2012, 08:55 #20 Member   andres Join Date: Sep 2010 Posts: 44 Rep Power: 8 why 100 or 500? is it 100 or 500 iterations with 0.6 time step or 0.12 time step? this is it? 60/100 = 06 60/500 = 0.12 but why this number ? I am going to perform the calculations and let you know but I donīt think my Velocity will go down after 60 sec or around...

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mihail CFX 7 September 7, 2014 06:27 cuteapathy CFX 14 March 20, 2012 07:45 colopolo CFX 13 October 4, 2011 22:03 Sas CFX 15 July 13, 2010 08:56 saii CFX 2 September 18, 2009 08:07

All times are GMT -4. The time now is 13:25.