
[Sponsors] 
September 3, 2002, 04:59 
Important:How many Iterations in each Timestep?

#1 
Guest
Posts: n/a

Hi,
I just wanna confirm the basic steps in solving for tranisent simulations. I am modeling the spread of ammonia gas in a room.The ammonia gas occupies a certain small volume in the domain initially. Basic Steps: 1.Solve the steady state solution for velocity and temp distribution in the room without the species transport 2.After converegd, use this converged solution, turn on transient mode, turn on species transport, and patch a small volume of cells in the domain with ammonia gas mass fraction. 3.Click off the "check for convergence" in the monitors for residuals for ALL entities such as xvelocity,vvelocity,zvelocity,continuity etc etc. 4.Specify the number of time steps and step size and the number of iterations in one timestep. 5.And WITHOUT initialising again, run the iterations Am I getting it right? Especially the part where in any transient simulation, we must use the converged result obtained in steady state solution. Also, can someone tell me how to determine the sufficient number of iterations used in each timestep? I was told that the number of iterations should not exceed 30. And I'm running at 20, how would I know if it is sufficient? Please help, Thanks. 

September 4, 2002, 05:12 
Re: Important:How many Iterations in each Timestep

#2 
Guest
Posts: n/a

You've got it right: first you calculate the steady state velocity field. Once you obtained that, you can start the transient simulation with species transport. You only have to solve the species transport, the velocity field can be turned off (under solve...). This is of course only the case when the presence of your species has no influence on the velocity field (I think that is always the case?) and when the velocity field is laminar (no timedependant turbulence).
As to the sufficient number of iterations per timestep: hard to say. I usually let the residuals "flatout" during each timestep: then I am certain that it is converged. Usually you don't need that, if they fall a few orders in magnitude it is sufficient, but you can only know it when you compare 2 results. If you use a smaller timestep you will need less iterations per timestep. Fluent states in its manual 1020 iterations per timestep. I have used already 3000 iterations per time step which allowed me to use a very big timestep and thus reduced my computational time by 2, yealding the same results as with a smaller timestep and fewer iterations per timestep. 

September 4, 2002, 09:16 
Re: Important:How many Iterations in each Timestep

#3 
Guest
Posts: n/a

Hey Piran,
Thanks for explaining things out for me. May I also know how big is big? For example, if I am modelling a total flow time of 2030 mins, I am using a timestep size of 15sec, and I let it run for 20 iterations in one timestep, is that sufficient?? You were saying that normally you are convinced only if the residuals flat out, but for my case, my residuals do not "flat out" but of decreasing gradient. One way in which I thought my iterations is sufficient, is by looking at the residuals for the species...for my case, I am seeing e4 and e5 for all the iterations in each timestep, that is why I assume that the number of iterations which I have chosen is ok. What do you think?? 

September 5, 2002, 12:27 
Re: Important:How many Iterations in each Timestep

#4 
Guest
Posts: n/a

Hello Julie,
I am afraid I don't have all the answers you need. I can tell you how I work, you can then decide what relevance it has to you. First of all I have to tell you that I work in microdimensions: µm and µs. For me it is very important to use not too fine a mesh and not too small a timestep: the smaller they become, the bigger the relative error. In my case, using the biggest possible timestep and the coarsest mesh is computationaly very advantageous, so I put a lot of effort into it. I don't know how important it is in your case, with much bigger dimensions. Anyway, the first step is always to check for gridindependance. I usually compare 2 simulations, one having double the amount of cells of the other. If the results only differ for a few percent (1%2%) I consider the grid to be fine enough and the result to be gridindependant. I only check for the properties I am interested in, like axial dispersion. Then I do the same for the timestep size. This is somewhat more complex though. The correct way to go about it is as follows: you first make a simulation with a small timestep and you let the residuals flat out per time step (in 1020 iterations). Then you increase the timestep and compare results. From a certain size for the timestep, the result will begin to change: it is no longer timestep independant, the timestep is too big. Once you have chosen a timestep you can start to decrease the number of iterations per timestep and see what happens. You should know what process is most important for your simulation. When I simulate reactions which are so fast that the diffusion is the most important step: I don't have to put in a lot of computational effort to simulate the reaction as precise as possible since it will have less effect on the result. When I look more closely at the residuals it tells me that when they dropped 5 orders in magnitude ( from 1 to 1e5) the diffusion is correct. The rest of the computation till they flatout (till 1e16) is for the reaction to be computed. But it has little effect on my result, so I don't bother, except when i need a very precise result. I had to do all the different steps to find out how to work. I now know how fine my meshes have to be, more or less, so I don't have to search for gridindependant every time. I have a good time step (1e4s) which is suitable over a wide range of cases. And I let the residuals flat out every time because i don't feel like checking every time if the residuals have dropped enough or not for the result not to be affected. So for your case I would say: run the simulation twice and compare results. Your time step size and number of iterations per timestep look good but you will have to find out. Something you should also keep in mind is what information you need. If you just need a general idee about the dispersion of the gas in the chamber you can afford a bigger error than when you want to precisely measure the dispersion. Also keep in mind that for postprocessing of data you need enough datapoints: if you want to calculate moments of peaks by example you will need a minimum of datapoints per peak, your timestep could be limited by it. I hope it helps something, Piran 

September 17, 2002, 00:43 
Re: Important:How many Iterations in each Timestep

#5 
Guest
Posts: n/a

Hey a BIG thank you to u!


September 26, 2002, 01:22 
Re: Important:How many Iterations in each Timestep

#6 
Guest
Posts: n/a

main think is that, u should check whether the residul for continuity is getting less in each time steps. Some recommend to run 35 iterations at every time steps, in my case I use 10 iterations per timestep and I did the same thing for 5 i/ts, it was also ok. I have a suggestion that u can make 3/4 secs and give 5 i/ts; the total no of iteration would be same and u will get a better result.
Alamgir 

September 30, 2002, 02:44 
Very Urgent

#7 
Guest
Posts: n/a

Dear Friend, I think i must seek your advise I am following the same procedure what you mentioned to solve species transport equations. I am havings reactions also enabled. When you patch a small region you get a decresed mass fraction as a function of time, which is acceptable But If i patch up the whole region with same mass fraction I should not have decreased mass fraction with rate to be equal to zero.. But I see mass fraction decreasing as a function of time I don't see why this should happen I feel I need some help in this..Please if you wanna talk please do call me at 3135851897 or please do send mail Thank you Duraivelan


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Extrusion with OpenFoam problem No. Iterations 0  Lord Kelvin  OpenFOAM Running, Solving & CFD  8  March 28, 2016 11:08 
Moving mesh  Niklas Wikstrom (Wikstrom)  OpenFOAM Running, Solving & CFD  122  June 15, 2014 06:20 
Orifice Plate with a fully developed flow  Problems with convergence  jonmec  OpenFOAM Running, Solving & CFD  3  July 28, 2011 05:24 
Differences between serial and parallel runs  carsten  OpenFOAM Bugs  11  September 12, 2008 11:16 
Unknown error  sivakumar  OpenFOAM PreProcessing  9  September 9, 2008 12:53 