Tranisent analysis  Few clarifications
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 
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 
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. 
Thanks Glenn for elaborate answer. Now, that's patience!
My observations: Quote:
Quote:
Quote:
Quote:
Image1: Cell residence time http://www.cfdonline.com/Forums/mem...timestep1.jpg Image2: Residuals falling by 3 orders http://www.cfdonline.com/Forums/mem...timestep1.jpg 
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 
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. 
Quote:

"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. 
1 Attachment(s)
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?

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 
HI Glenn
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!!:mad: 
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?

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? 
HI Glenn
It was about transient simulations and we were having discussion about convergence that if smaller timesteps could make convergence better. 
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. 
All times are GMT 4. The time now is 03:34. 