
[Sponsors] 
October 26, 2000, 15:02 
hints on time steps

#1 
Guest
Posts: n/a

I will have to simulate a system in which the final time is, in laboratory systems, of about 2 days, and in industrial facilities are several months. Are there some strategies to obtain faster results?
I only have less than 9 months to finish my project not years to wait for in front of the screen. Thanks Arturo 

October 26, 2000, 15:29 
Re: hints on time steps

#2 
Guest
Posts: n/a

(1). If that is the case, then there is no way to make numerical weather prediction, several days ahead of time?


October 27, 2000, 09:52 
Re: hints on time steps

#3 
Guest
Posts: n/a

Hi Arturo,
to be genuine I really do not understand your question. May be you can say somethings more. Cheers Maurizio 

October 27, 2000, 11:08 
Re: hints on time steps

#4 
Guest
Posts: n/a

Hi Maurizio.
I am new at fluent and CFD, so maybe my questions are too simple or just can't be answered. I'm trying to use fluent and some other codes in transient state and usually you supply an initial step time, but then the code readjust itself if there are convergence problems ( I guess). Sometimes the adjusted times are in the order of 0.000001 secs. or less. If I have to simulate (in real time) days or months; are there some tricks in order to obtain faster results?( convergence?). Maybe I have to simplify the model or change the solver, etc. That is what I would like to know from the people that has more experience. Thanks. Arturo 

October 27, 2000, 11:47 
Re: hints on time steps

#5 
Guest
Posts: n/a

Hi Arturo,
still too much information is missing to give you a really useful answer. Anyway as a general hint: if you are doing a transient calculation (i.e.you are looking for time accurate results), the time step you assign depends on the physics of the problem, i.e. on the time scale of the phenomena in concern. These can be milliseconds (1.0e6) or days (8.64e+4). This is up to you to discover. Furthermore if the time step is not the right one, unluckely Fluent will not adapt to a new one but will simply "diverge" or give wrong results. Therefore you should be careful: the code can do really much but, while using it, it needs to have the user's brain switched on ! Ciao Maurizio 

October 27, 2000, 15:37 
Time Scales

#6 
Guest
Posts: n/a

Being relatively new to fluid modeling and simulation, could you please expand on time scales?


October 29, 2000, 04:21 
Re: hints on time steps

#7 
Guest
Posts: n/a

Arturo, As Maurizio said, you may little explain the physical problem you are trying to simulate in order for us to think about the appropriate length of the time step and its number.


October 30, 2000, 04:58 
Re: Time Scales

#8 
Guest
Posts: n/a

Dear Clinton,
in general each physical phenomenon has a characteristic time to occur. For example, if we think to chemical reactions, a suitable time for fast reactions to occur can be 1.0e8  1.0e7 seconds. There are also more slower reactions as those for the NO_x formation in combustion products which can have characteristic times such as 1.0 second. As another example consider a turbulent flow. In this case there is a large hyerarchy of vortexes (from very large to very small) which evolve with different velocities and therefore different time scales. For example in a air flow (average velocity 50 m/s and channel diameter 1 m) for the smaller ones (those called Kolmogorov vortexes) and the larger ones the time scale can vary from 4.0e9 > 0.2 seconds (I have just done a rough calculation assuming 10% for turbulence intensity). Furthermore if you consider the channel lenght as being 2m, the average flow time scale is: 0.04 seconds (representing the average residence time of the fluid in the channel). These different examples are just to show what kind of complications you can encounter in flow: imagine a turbulent reacting flow in which you whant to simulate accurately all time scales!! In fact, it is the existence of a so broad range of time and space scales which make Direct Numerical Simulation particularly demanding from the computational point of view (with DNS you are forced to solve up to smaller scales, no average is allowed). To fynally link this considerations with the real life of each of us CFD guys, imagine that you want to simulate a phenomenon with requirement of time accuracy (a transient or somethings which eveolves in time); if you choose a to large time step, the think you want to see can be completed well before the time you have set (imagine this like what a shortsighted can see without glasses). Therefore you have to "tune" your time step with the relevant time scale(s) of the problem you are solving to capture its main features (what the shortsighted can do using his glasses: now he can see also little objects). I hope this helps Ciao Maurizio 

October 30, 2000, 05:52 
Re: Time Scales

#9 
Guest
Posts: n/a

I think also that the shutter speed of a Camera is a good example of the time scale. If you have an object moving faster than the shutter speed, the camera will not be able to capture it. So, the sutter speed should be equal if not faster than the object itself. Am I correct Maurizio??


October 30, 2000, 06:50 
Re: hints on time steps

#10 
Guest
Posts: n/a

Explain the problem to us. If I may make the assumption that conditions do not change throughout lab test, the solution should obtain some sort of steady state scenario, right? I am not strong at choosing the right time step. You can think of the time scale as the inverse of the frequency. Chances are that you will need to have a good idea of the time scales for a more accurate solution. If time is your concern, I first suggest you run simple cases first. Get the feel that you are taking the right approach. Start with a 2d steady state solution. then go to 3d solution steady state. you may also want to obtain an inviscid and/or laminar solution before trying turbulence models. you can begin with a coarser mesh for decreased computing time, and then you can refine the mesh, especially in certian areas that require high refinement. Make sure you are heading in the right direction with the quicker and simplified solutions so when it comes time to run your final solution, which is unsteady, that actually simulates the lab equipment, you won't risk waisting time by taking wrong approaches. You should also consider obtaining high power computers and/or allowing for parallel processing. Would the rest of you agree?


October 30, 2000, 07:19 
Re: hints on time steps

#11 
Guest
Posts: n/a

Yes I agree with you, this is always the procedure to run a CFD project


October 30, 2000, 08:37 
Re: Time Scales

#12 
Guest
Posts: n/a

HI Ahmed,
yes, a sort of it. Ciao Maurizio 

October 30, 2000, 14:03 
Re: hints on time steps

#13 
Guest
Posts: n/a

Hi, thank you very much; all the discussions have been very helpful, now I have a better idea in what can I have and what I can't.
The nature of my problem is in transient state. I am trying to simulate a packed bed in which a liquid flows that contains small particles, the packed bed is clean initially and, depending on the nature of the particles and the packing that conforms the bed the smalls particles get attached to the packings that confoms the bed. Eventually the deposition of the particles changes the volume fraction of the solid (the packing). This leads to an increase of the pressure drop. I am using the Eulerian multiphase model in fluent 4.5 to model it. I am still trying to implement the model of deposition of the particles that is governed by a scalar transport equation. But even without that model when I simulate the bed, increasing the solid's volume fraction with a very slow and smooth function, the step time goes to 105 or lower, it takes ages to have one hour of realtime simulation. I don't really know what will happen when the full model will be completed but I think that the step time will become smaller. In the lab the experiment data is for about 2 days and for the industrial installation is several months. My computer facilities are scarce so I am very interested in the subject. Thanks to all for the interest, I really appreciate that. Truly 

October 31, 2000, 02:58 
Re: hints on time steps

#14 
Guest
Posts: n/a

I think your problem is in some ways similar to mine  the chemical reaction of a large coal seam.
As has been pointed out there are a range of time scales and when you do a fully coupled simulation of the physics you need to set the time step to be equal to or smaller than the smallest timescale in your system.( Note this may change over time) As you've pointed out this can be very small. However there are some things to do. Do you need to solve a fully coupled system  can the coupling be relaxed somehow or do some physics of the system have timescales so small compared to the other timescales, that one my consider them to respond instantaneously to changes in the physics occurring at the larger time scales and perhaps be treated as essentially steady processes?? This is what I'm attempting  and it works. That is, I assume that the state at each point in time in my system is essentially at steady state, and then use these results to make changes to those parts of the system that have long timescales, generating a new representation of the system at the next time step. This is some sort of pseduosteady assumption. In your case, perhaps changes in the bed properties occur slowly, so on this timescale which might be on the order of days, the flow is essentially steady. Perhaps, using you models, you can assume a distribution of the bed and solve for the flow and particle deposition. From this steady state solution you'll get the rates of deposition to the solid, and you can update the solid properties, generate a new model and resolve for steady state again. In this way it may be possible to solve for the evolution of the system over long time scales without resolving all the details at the small timescales, which will be very computationally intensive. Regards Greg Perkins 

October 31, 2000, 03:03 
Re: hints on time steps

#15 
Guest
Posts: n/a

Further to this, I am wondering if anybody has solved these types of problems in Fluent by some hybrid steady  transient method  in which you assume some equations are steady and some are transient  depending on the physics. Rather than completely steady or completely fully transient.
Anybody? Greg 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Multiple floating objects  CKH  OpenFOAM Running, Solving & CFD  12  March 21, 2016 14:05 
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3  bookie56  OpenFOAM Installation  8  August 13, 2011 04:03 
directMapped problem  panda60  OpenFOAM Bugs  4  July 8, 2010 10:23 
calculation diverge after continue to run  zhajingjing  OpenFOAM  0  April 28, 2010 04:35 
export time steps for ensemble averaging  Thomas Baumann  Siemens  0  March 2, 2010 04:19 