CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Important:How many Iterations in each Timestep?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   September 3, 2002, 04:59
Default Important:How many Iterations in each Timestep?
  #1
Julie
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 x-velocity,v-velocity,z-velocity,continuity etc etc.

4.Specify the number of time steps and step size and the number of iterations in one time-step.

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 time-step? 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.
  Reply With Quote

Old   September 4, 2002, 05:12
Default Re: Important:How many Iterations in each Timestep
  #2
Piran
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 time-dependant turbulence).

As to the sufficient number of iterations per time-step: hard to say. I usually let the residuals "flat-out" during each time-step: 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 time-step you will need less iterations per time-step. Fluent states in its manual 10-20 iterations per time-step. I have used already 3000 iterations per time step which allowed me to use a very big time-step and thus reduced my computational time by 2, yealding the same results as with a smaller time-step and fewer iterations per time-step.
  Reply With Quote

Old   September 4, 2002, 09:16
Default Re: Important:How many Iterations in each Timestep
  #3
Julie
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 20-30 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 e-4 and e-5 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??
  Reply With Quote

Old   September 5, 2002, 12:27
Default Re: Important:How many Iterations in each Timestep
  #4
Piran
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 micro-dimensions: Ám and Ás. For me it is very important to use not too fine a mesh and not too small a time-step: the smaller they become, the bigger the relative error. In my case, using the biggest possible time-step 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 grid-independance. 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 grid-independant. I only check for the properties I am interested in, like axial dispersion. Then I do the same for the time-step 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 time-step and you let the residuals flat out per time step (in 10-20 iterations). Then you increase the time-step and compare results. From a certain size for the time-step, the result will begin to change: it is no longer time-step independant, the time-step is too big. Once you have chosen a time-step you can start to decrease the number of iterations per time-step 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 1e-5) the diffusion is correct. The rest of the computation till they flat-out (till 1e-16) 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 grid-independant every time. I have a good time step (1e-4s) 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 time-step 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 post-processing of data you need enough data-points: if you want to calculate moments of peaks by example you will need a minimum of data-points per peak, your time-step could be limited by it.

I hope it helps something,

Piran
  Reply With Quote

Old   September 17, 2002, 00:43
Default Re: Important:How many Iterations in each Timestep
  #5
Julie
Guest
 
Posts: n/a
Hey a BIG thank you to u!
  Reply With Quote

Old   September 26, 2002, 01:22
Default Re: Important:How many Iterations in each Timestep
  #6
Alamgir
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 3-5 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
  Reply With Quote

Old   September 30, 2002, 02:44
Default Very Urgent
  #7
Duraivelan.D
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
  Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
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
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM 6 April 12, 2011 11:24
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16
Unknown error sivakumar OpenFOAM Pre-Processing 9 September 9, 2008 12:53


All times are GMT -4. The time now is 04:21.