
[Sponsors] 
February 19, 2002, 04:07 
No. of time step / convergence

#1 
Guest
Posts: n/a

Hi,
Does anyone have some idea or rule of tumb about how many accum. timestep (steady state)are nesseary in order to achieve convergence as a function of number of elements ? Like for isothermal and nonisothermal cases. Regards Jens 

February 20, 2002, 03:07 
Re: No. of time step / convergence

#2 
Guest
Posts: n/a

Seems to me that the number of timesteps to convergence, especially with the coupled solver in CFX5 should roughly be constant with the number of elements, or at least have a very weak dependence. I bet if you took one hex grid, ran it, and it converges in n iterations, then double the resolution in each direction by simply cutting all the cells into 8, that grid would converge in something close to n iterations as well.
This of course will be grid quality dependent. Neale 

February 24, 2002, 00:35 
Re: No. of time step / convergence

#3 
Guest
Posts: n/a

Hi Jens,
You should be able to converge within 200 iterations, regardless of the number of nodes. Robin 

February 24, 2002, 10:46 
Re: No. of time step / convergence

#4 
Guest
Posts: n/a

With Autotimestepping I agree. But, if you use 'Physical Timestepping' with a very small time step, you might require 1000 iterations. Thus, it depends on your time step relative to the dimensions of your problem and the specific velocity. I know, Autostepping is the preferred default selection but we sometimes have to use 'Physical Timestepping' when the Autotimestepping does not give desired behavior.
Astrid 

February 24, 2002, 19:28 
Re: No. of time step / convergence

#5 
Guest
Posts: n/a

Personally I'd never use the automatic timestep calculation. Generally, it's far too conservative.
Why would you use physical timescale with a small timestep anyways. That seems pointless. You can always estimate a decent timescale simply using 1/3 to 1/5 L/V, maybe 0.1 if your problem has some initially fast transients that need to be resolved. Neale 

February 24, 2002, 19:38 
Re: No. of time step / convergence

#6 
Guest
Posts: n/a

Astrid,
Of course your simulation will take forever if you use a small timestep! Once you are past the initial transient, after 10 to 20 timesteps, you should increase the physical timestep up to at least the resident time of your model. Basically, use as big a timestep as you can get away with. Robin 

February 25, 2002, 03:11 
Re: No. of time step / convergence

#7 
Guest
Posts: n/a

Neal and Robin,
We run cases with a large geometry but with difficult physics in a small region (shocks, Ma>1.5 etc). Then, a large time step does not always give the desired behavior. To prevent the 100th FINMES we take a small timestep and run it overnight or in the weekend (400500 iterations). Monday is usually a nice day to start the week because I start the week with a solution! Astrid 

February 25, 2002, 21:52 
Re: No. of time step / convergence

#8 
Guest
Posts: n/a

Astrid,
Which advection scheme are you running? Do you use mesh adaptation to help resolve the shocks? Robin 

February 26, 2002, 07:42 
Re: No. of time step / convergence

#9 
Guest
Posts: n/a

 Upwind and High Resolution.
 No. I already have to many elements (>5M). Astrid 

February 26, 2002, 20:49 
Re: No. of time step / convergence

#10 
Guest
Posts: n/a

Hi Astrid,
Stick to High Resolution for your converged solution. Upwind is just bad, bad, bad. I highly recommend using mesh adaption when you have a highly compressible flow. It will allow you to make better use of the nodes you can afford your problem. Start with fewer nodes, 1 Million for instance. Use the mesh adaptation to add the additional nodes by setting a node budget of 5 Million for the final mesh. For resolving shock waves, adapt the solution based on Pressure. In this way, you will use the nodes where you need them, rather than spreading them throughout the domain. You should also choose the "variation*edge length" option, this will prevent the adaption algorithm from favoring the shock for adaption. Skew the node addition to add the maximum number of nodes at the first adaption step, a node allocation parameter of 2.0 will do this. Lastly, set the adaption criteria to adapt at a convergence of 1e4 MAX residual or a maximum of 100 timesteps. Make sure you use a reasonably large timestep (no less than 1/100th of the advection time, preferably 1/10th to 1/5th. Let her rip... Regards, Robin 

February 27, 2002, 17:37 
Re: No. of time step / convergence

#11 
Guest
Posts: n/a

Indeed, I use for Upwind for start up and High Resolution for the Final solution.
Thank you for your advices on Mesh adaption. I will give it a try. Unfortunately live is not so simple as the solution is very unsteady: the shocks don't have a fixed position. Actually I should perform transient calculations. Is it possible to use mesh adaption in transient calculations. In other words, is it possible to get rid of a refined grid in positions were it is not required anymore? Astrid 

February 27, 2002, 20:52 
Re: No. of time step / convergence

#12 
Guest
Posts: n/a

Hi Astrid,
Mesh adaption too expensive a process to do at each timestep of a transient simulation, better to refine the mesh in the area of the shock before you begin. Robin 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
SLTS+rhoPisoFoam: what is rDeltaT???  nileshjrane  OpenFOAM Running, Solving & CFD  4  February 25, 2013 05:13 
Force can not converge  colopolo  CFX  13  October 4, 2011 22:03 
Orifice Plate with a fully developed flow  Problems with convergence  jonmec  OpenFOAM Running, Solving & CFD  3  July 28, 2011 05:24 
Modeling in micron scale using icoFoam  m9819348  OpenFOAM Running, Solving & CFD  7  October 27, 2007 00:36 
AMG versus ICCG  msrinath80  OpenFOAM Running, Solving & CFD  2  November 7, 2006 16:15 