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:

1. In transient analysis, generally a third of residence time is suggested for time step. But in case of bubble column, the flow keeps circulating for a long time, while gas escapes earlier through degassing boundary at top. What should be residence time here (perhaps a turnaround time, which is large!)?
2. Some guidelines advise to use courant no. (generally ~2-5),velocity and mesh size to get time step. If mesh is nonuniform, which cells should be considered for mesh size?
3. In general it is recommended that at each timestep, residuals should fall from first coeff loop to last loop by O(1e-3) to a value set for convergence criteria (say 1e-6). This presents a rule of thumb and though needs some tweaking, is easy to implement. But this discards the use of physics as advised in point #1 and #2 point. Which of these three methods is best? I believe time step sensitivity analysis may help, but don't have a reference guide about how to do it.
4. I believe "convergence" implies few things. Monitors of interest are flat or oscillating at a set frequency, imbalances ideally less than 0.01% and residuals meeting convergence criteria at end of each time step. Is this right?
5. I observed that imbalance of P-Vol keeps fluctuating no matter how small or big the time step is. How to deal with this?
6. What is ideal time for total time duration in any simulation for a fairly accurate representation of time averaged results?
7. I would like to use "Edit run in progress" option in CFX solver instead of going to Pre every time I need to change timestep or discretization scheme. But though I change the timestep and save it, it doesn't seem to affect the run in progress in any way. Am I missing something here?
8. Given that TVD schemes work best for such cases, I would like to use it. But where are they hidden under the hood?
   

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 p-vol 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 pre-deciding them

Though, I appreciate help in understanding more about my questions.

Regards
OJ

Patience is a virtue.

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.cfd-online.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:

? I have no idea what you are saying. It seems completely wrong. Whether the solver is implicit or explicit, they both require an appropriate time step size for accuracy.

One of the most common mewbie mistakes on this forum is to take some flow time scale, divide by a smallish number and say that should be a good time step. I have lost count of the number of times I have heard that. The correct answer is sensitivity analysis.

For transient simulations you can simplify things a little by using adaptive time steps, converging on 3-5 coeff loops per iteration (maybe 5-10 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:
I referred the Fluent 13 training material slides. Attached is the snapshot. Though, I meant "cell residence time" and not "domain residence time." as the latter would be unarguably too large to capture the time scales of smaller eddies anyway. In general, roughly 20 timesteps in every period are advised in those notes. Sorry for the wrong choice of words, the post could have been more clearer :)

This again is referred from the Fluent training material, as shown in attached snap. Though both of above methods are restrictive and give a ball-park value of the timestep, I agree that I need a timestep taylored for my setup, which can be arrived at with sensitivity analysis. Though I have a general idea after going through Wiki FAQ and some threads here, do you suggest any comprehensive guide that elucidates this concept?

In fact, you can! Like I said, after changing your preferences, you need to save and close(!) the "Edit run in progress" dialogue box. And you see the effect next time step. I nearly jumped off my seat when I found out about it after repeated failures.

Wow! That would suit my setup as there are discontinuities owing to two phases. I went through the theory guide and the "Beta" seems to be some sort of flux limiter to forbid the second order scheme extremum near discontinuity. Though the guide adds that it can be shown to be TVD only when used in one dimensional situation!

Image1: Cell residence time
http://www.cfd-online.com/Forums/mem...-timestep1.jpg

Image2: Residuals falling by 3 orders
http://www.cfd-online.com/Forums/mem...-timestep1.jpg

Adding following details of set-up for multiphase bubble column.

Mesh:
Axisymmetric, Hex elements

Model:
Eulerian Eulerian, mono-dispersed, 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 time-stepping with 5-9 coeff loops and High resolution discretization scheme.

I seem to have two discrepancies in my results:

1) p-Vol residual remains at 2-3% 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

In that case use it as the starting point for a sensitivity analysis. The sensitivity analysis will find the real answer. This is the case for CFX, Fluent or any other solver actually.

This is not appropriate for CFX as CFX calculates its residuals quite differently from Fluent. Again the best answer is a sensitivity analysis, but for CFX you will probably find the residual you achieve is related directly to accuracy, so 1e-4 is loose convergence regardless of mesh size, simulation type etc, and 1e-5 is adequate in most cases and 1e-6 is tight. The fact that the CFX residuals are normalised like this makes this sort of check far easier.

The doco says it reduces to exactly a TVD scheme for 1D. For 2D and 3D it is similar to a TVD scheme, that is why I said "essentially a TVD scheme". If you want second order accuracy but want to minimise wiggles at sharp gradients then hi res is the one to choose.

You are very wise to get things working and accurate on a simple case before adding the complex physics.

For your convergence issues:
Have a look at the FAQ here http://www.cfd-online.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.

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?

"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.

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.cfd-online.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?

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.