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

No. of time step / convergence

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 19, 2002, 03:07
Default 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

  Reply With Quote

Old   February 20, 2002, 02:07
Default 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
  Reply With Quote

Old   February 23, 2002, 23:35
Default 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
  Reply With Quote

Old   February 24, 2002, 09:46
Default 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
  Reply With Quote

Old   February 24, 2002, 18:28
Default 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
  Reply With Quote

Old   February 24, 2002, 18:38
Default 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
  Reply With Quote

Old   February 25, 2002, 02:11
Default 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
  Reply With Quote

Old   February 25, 2002, 20:52
Default 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
  Reply With Quote

Old   February 26, 2002, 06:42
Default 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
  Reply With Quote

Old   February 26, 2002, 19:49
Default 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

  Reply With Quote

Old   February 27, 2002, 16:37
Default 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
  Reply With Quote

Old   February 27, 2002, 19:52
Default 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
  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
SLTS+rhoPisoFoam: what is rDeltaT??? nileshjrane OpenFOAM Running, Solving & CFD 4 February 25, 2013 04:13
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 15:15


All times are GMT -4. The time now is 01:43.