# No. of time step / convergence

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 February 19, 2002, 04:07 No. of time step / convergence #1 Jens 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 non-isothermal cases. Regards Jens

 February 20, 2002, 03:07 Re: No. of time step / convergence #2 Neale Guest   Posts: n/a Seems to me that the number of timesteps to convergence, especially with the coupled solver in CFX-5 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 Robin 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 Astrid 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 Neale 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 Robin 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 Astrid 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 (400-500 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 Robin 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 Astrid 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 Robin 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 1e-4 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 Astrid 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 Robin 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 Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post nileshjrane OpenFOAM Running, Solving & CFD 4 February 25, 2013 05:13 colopolo CFX 13 October 4, 2011 22:03 jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24 m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36 msrinath80 OpenFOAM Running, Solving & CFD 2 November 7, 2006 16:15

All times are GMT -4. The time now is 17:39.

 Contact Us - CFD Online - Top