
[Sponsors] 
June 15, 2012, 06:59 
Tranisent analysis  Few clarifications

#1 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Hello,
I am currently using CFX 13 for simulating bubble columns and the parameters of interest are holdup, interfacial density and overall velocity and volume fraction distribution. I intend to use transient mode for the same. Having gone through documentation of both CFX and Fluent, as well as their training material on portal and finally the convergence criteria FAQ on Wiki, I still have few basic unresolved queries:
I apologize for long list and repeated use of words like ideal and best, though they doesn't exist in this field! But I am a beginner and want to get a general idea about how to practically approach CFD. Help is much appreciated. Regards OJ Last edited by oj.bulmer; June 15, 2012 at 08:04. 

June 16, 2012, 06:34 

#2 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Anyone, please?
I will keep sharing my learnings anyway which I realised after combing through the forums and experimentation. #7 You need to close the "edit run in progress" dialogue box after saving your settings to see the effect. If not closed, it doesn't affect the current settings! Well, this is strange #5 Imbalance of pvol depends on time step. As i decreased the timestep, the imbalance decreased. #1,2,3 The CFX being implicit solver, is not much sensitive to time step when it comes to transience. Yet physics and numerics is. The playing with time steps makes more sense to achieve time step rather than predeciding them Though, I appreciate help in understanding more about my questions. Regards OJ Last edited by oj.bulmer; June 16, 2012 at 08:49. 

June 17, 2012, 19:56 

#3  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
Quote:
Questions from your first post. 1. I have no idea why you say time step = 1/3 residence time. You set time step size through a sensitivity analysis. 2. I do not recommend using Courant No to set things. Again, sensitivity analysis. 3. You guessed it, set convergence toelrance by sensitivity analysis. 4. Sort of. Convergence is defined as when you are happy the parameters of interest to you are convergend to a tolerance you are happy with. This takes into account that different people are interested in different parameters, and different levels of accuracy required. But often you need to specify this to the solver as a residual tolerance, so you do a sensitivity analysis to find what convergence tolerance (or imbalances if necessary) is required to achieve your required accuracy. 5. This is a problem specific to your simulation. You would need to provide further details. The FAQ gives some tips: http://www.cfdonline.com/Wiki/Ansys...gence_criteria 6.Sensitivity analysis 7. You cannot change a transient run in progress. 8. The High resolution scheme is essentially a TVD scheme. Your second post: Quote:
Quote:
For transient simulations you can simplify things a little by using adaptive time steps, converging on 35 coeff loops per iteration (maybe 510 for complex multiphase models). Then time step size is automatically adjusted when you change the convergence level, and you have one less parameter to adjust. 

June 19, 2012, 12:58 

#4  
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Thanks Glenn for elaborate answer. Now, that's patience!
My observations: Quote:
Quote:
Quote:
Quote:
Image1: Cell residence time Image2: Residuals falling by 3 orders 

June 19, 2012, 15:32 

#5 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
Adding following details of setup for multiphase bubble column.
Mesh: Axisymmetric, Hex elements Model: Eulerian Eulerian, monodispersed, 2 mm gas bubbles (I will eventually move to MUSIG population balance model for coalescence and breakup with at least 4 bubble size groups, but that would be after I have handle on this one) Boundary conditions: Inlet: Gas  Mass flow rate of gas 0.07 kg/s, volume fraction 0.25 Liquid  Normal speed 0, volume fraction 0.75 Outlet: Degassing Symmetry: Two symmetric boubdaries and tip nipped at axis where I specified free slip boundary I use transient adaptive timestepping with 59 coeff loops and High resolution discretization scheme. I seem to have two discrepancies in my results: 1) pVol residual remains at 23% and doesn't fall. 2) For few of my inner coeff loops, the linear solution says "ok" or "F" though I am using smaller time steps. I would like suggestions on how to mitigate this. Thanks OJ 

June 19, 2012, 19:47 

#6  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
Quote:
Quote:
Quote:
Quote:
For your convergence issues: Have a look at the FAQ here http://www.cfdonline.com/Wiki/Ansys...gence_criteria it talks about steady state runs but much of the comments also apply to transient. Other comments: * Try double precision numerics * Try smaller time step (although with adaptive time stepping you achieve this by setting a tighter residual tolerance) * Try adding imbalances to the convergence criteria * Try improving mesh quality * Put the residuals in the output file and have a look in the post processor to find which areas are not converging. This may give some tips on how to address it. 

September 7, 2012, 12:49 

#7 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 8 
May i ask, what is the definition of 'Characteristic Length' and 'Characteristic velocity' please? is it simply the length of pipe and the velocity of the fluid flow respectively please?
__________________
Thank you for your kind attention. Kind regards, mactech001 Currently using: ANSYS v13 

September 8, 2012, 07:28 

#8 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
"characteristic" just means something representative. So for a pipe the characteristic length could be the diameter, for flow along a surface the distance along the surface, for a square in cross flow the edge length.
But note this is only an estimate of time step size. This should be used only as a starting point for a sensitivity analysis, and the sensitivity analysis finds the real time step size you need. 

September 10, 2012, 11:14 

#9 
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 8 
may i ask: is the attached RMS residual plot of a transient analysis, show a good transient analysis convergence and indication of reliable results please?
__________________
Thank you for your kind attention. Kind regards, mactech001 Currently using: ANSYS v13 Last edited by mactech001; September 10, 2012 at 11:25. Reason: additional attachment 

September 10, 2012, 18:19 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
Your graph shows that at the start of the run you have loose convergence (in terms of residuals), and as the run progresses the residuals for each time step get tighter. By the end they are very tight.
But this is only one part of the requirements for an accurate analysis, so whether this is adequate convergence needs to be checked (sensitivity analysis), and there are many other things to check before you can say this is a reliable result. See http://www.cfdonline.com/Wiki/Ansys...publishable.3F 

September 11, 2012, 02:56 
HI Glenn

#11 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 6 
I would like to add something regarding "timestep" selection as were advised by some wise guy..... .
"It is a common blunder to reduce the timesteps to improve the convergence" he said so. Is it true??? Infcat he laughed at me when I told him that I also tried to reduce timestep to improve convergene...damn!! 

September 11, 2012, 07:22 

#12 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
I need some context to answer that question  steady state or transient? A run which is converging nice and you wish to go faster, or a run which is having difficulties converging at all?


September 11, 2012, 11:12 

#13  
Senior Member
Join Date: Nov 2009
Posts: 125
Rep Power: 8 
Quote:
Hello Glenn, thank you for your kind comments and time again. When one speaks about "Keep lowering your residual value until the solution no longer converges monotonically", am i right to understand that, i should obtain a residual plot where the line reaches the convergence residual RMS value but stay horizontal please?
__________________
Thank you for your kind attention. Kind regards, mactech001 Currently using: ANSYS v13 

September 11, 2012, 17:04 

#14 
Senior Member
Danial
Join Date: Nov 2011
Posts: 179
Rep Power: 6 
HI Glenn
It was about transient simulations and we were having discussion about convergence that if smaller timesteps could make convergence better. 

September 11, 2012, 19:26 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,577
Rep Power: 90 
mactech  No, you determine what convergence tolerance is required using a sensitivity analysis looking at output variables of interest to you.
Danial  In a transient simulation smaller time steps will make convergence easier. There are (of course) expections to this, for instance if the time step gets so small so that numerical round off becomes important. In this case smaller timesteps will be harder to converge, and you should use double precision numerics to reduce the round off error. Also if the flow is LES so you are resolving very small vorticies then a smaller time step will resolve more of these vorticies and that may make convergence trickier. But in this case you probably just have to put up with it as the entire idea of LES is to resolve the small eddies. 

Tags 
bubble columns, convergence, transient 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Eigenfrequencies static and modal analysis  Laura_mecheng  ANSYS  1  May 15, 2012 03:40 
multifield problems on ia64  zegtuhetmaar  ANSYS  7  October 21, 2010 13:18 
3D analysis of Ahmed body  Irshad22  FLUENT  0  December 17, 2009 05:33 
Short Course: Computational Thermal Analysis  Dean S. Schrage  Main CFD Forum  11  September 27, 2000 17:46 
Is CFD Science or Art ?  John C. Chien  Main CFD Forum  36  October 5, 1999 12:58 