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

Time step size and max iterations per time step

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

Like Tree16Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   July 27, 2013, 11:52
Default
  #21
Member
 
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4
star is on a distinguished road
I will work out with this. Thanks..
In transient flow in the convergence history graph (the coefficient of lift (CL) vs Flow time) the calibrations on CL is very high i.e scale of 100 is used, so CL line looks like straight (but there is some oscillation which i cannot see precisely), how can I change or set the CL scale?
star is offline   Reply With Quote

Old   January 16, 2014, 07:10
Question
  #22
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 473
Rep Power: 6
Anna Tian is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
Again, I doubt that you want to resolve any time-dependent effects in your simulation. Most probably, there are no transient effects in the flow you are simulating.
In this case, it is an unnecessary burden to do a transient simulation because you have to choose more simulation parameters (time step size, number of iterations, transient numerical scheme...).
If the physics are not time-dependent, I would not know how to estimate a suitable time step size.
I have a question related to this for my special case.

For my case, the transient behavior is not significant. The solution of my simulation is not time dependent according to the transient simulation results. But I have to run the transient simulation just because the steady state solution doesn't not converge. In this case, I'm wondering will large time step bring me faster to the steady solution than the small time step (here we assume they converge to the same residual level every time step with the same iteration number)? If I choose the large time step as 0.0001, and the smaller one as 0.00001. Will the large time step transient simulation bring me to the steady solution almost 10 times faster then the small one?
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   January 16, 2014, 07:18
Default
  #23
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
I think so.
With larger time step, the solution evolves faster from the initial conditions towards the final solution.
But since you encountered difficulties with a steady-state solver, dont expect this to hold true for arbitrary time step sizes. The transient solver might have the same difficulties converging the solution when the time step size is too high.
flotus1 is offline   Reply With Quote

Old   January 16, 2014, 07:24
Question
  #24
Senior Member
 
Anna Tian's Avatar
 
Meimei Wang
Join Date: Jul 2012
Posts: 473
Rep Power: 6
Anna Tian is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
I think so.
With larger time step, the solution evolves faster from the initial conditions towards the final solution.
But since you encountered difficulties with a steady-state solver, dont expect this to hold true for arbitrary time step sizes. The transient solver might have the same difficulties converging the solution when the time step size is too high.
But will it be 10 times faster? I also encounter the problem of choosing large time step or small one now. Large time step need more iterations to converge at every time step. But it doesn't seem to evolve much faster from the initial conditions towards the final solution. It seems to me that, for this kind of 'stead' case, large time step can never be better than small one. Maybe it's better to have time step very small?
__________________
Best regards,
Meimei
Anna Tian is offline   Reply With Quote

Old   January 16, 2014, 07:35
Default
  #25
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
If the flow is really time-dependent, you will get to the same point with 10 times less time steps if you choose a time step 10 times larger, provided both time step sizes are able to resolve the relevant transient effects.
Of course with an implicit method you will need more iterations per time step to achieve the same level of convergence.

But since you are using a transient solver as a computational workaround for a flow that might have no transient effects at all or at least we dont know the time scale of the flow, I would not expect the exact same behavior.

Lets have a look at a simple example, the couette flow between two parallel plates initially at rest.
The flow actually is time-dependent, but if the Reynolds number is sufficiently low, it will reach a steady state, a linear velocity profile between the two plates.
So we could simulate the long-term-solution of this flow both with a steady solver or with a transient solver.

But how long will it take for the transient solver? The viscous time scale at which the flow develops is
T_{v} = \frac{L^2}{\nu}
If we choose the time step size of the transient solver to be 1/10th of the viscous time scale, we need an order of 10-100 time steps to reach the steady state.
If we choose a time step size of 1/1000th of the viscous time scale, we need an order of 1000-10000 time steps to reach the same solution, which will obviously take longer.

To conclude: It is not always better to have a small time step size.
Anna Tian likes this.
flotus1 is offline   Reply With Quote

Old   February 11, 2015, 07:58
Default time step size in vof method
  #26
New Member
 
enass
Join Date: Feb 2015
Location: Alexandria-Egypt
Posts: 3
Rep Power: 2
enass massoud is on a distinguished road
I am working on 2 phase flow using vof method and i want to know how to calculate the time step and the number of time steps and how to determine the maximum number of iterations per time step?
enass massoud is offline   Reply With Quote

Old   April 13, 2015, 04:36
Default Global Courant Number in Fluent 15.0
  #27
New Member
 
Rubegan
Join Date: Apr 2015
Posts: 1
Rep Power: 0
ruben91 is on a distinguished road
Hi everyone.

I am currently investigating multiphase flow in a pipe with regards to how it develops. I am currently using a grid size of 2 and the highest input velocity is 0.3m/s. In order to have my Courant number less than 1, I am using a fixed time step of 0.0006s.

However, I am getting a Global Courant number of 5.03. Would this affect the accuracy of my simulation? And if so how do I reduce the Global Courant number and is there even a need to do so?

Thank you.
ruben91 is offline   Reply With Quote

Old   May 12, 2015, 20:04
Post
  #28
Member
 
John M.
Join Date: Jul 2011
Posts: 57
Rep Power: 6
villager is on a distinguished road
Quote:
Originally Posted by ruben91 View Post
...
However, I am getting a Global Courant number of 5.03. Would this affect the accuracy of my simulation?
See this link
http://cape-forum.com/index.php/topi...2.html#msg1392
William provides guidelines for CFL numbers using VOF approach in FLUENT. They are also summarized here.

CFL number greater than some value (generally, 1, 2.5 for multi-stage FLUENT solver) would result in numerical instability when using explicit formulation. It is allowed for implicit solver, however, rising CFL leads to increased numerical error due to the fact that every mesh-based solution becomes less precious when increasing step size (both time step and mesh step, the latter just means coarsening the mesh). However, if you have no transient effects you can use higher CFL.
You can run several calculations refining the time-step, the results should converge to some values (it's like mesh convergence, just refining time-step instead of mesh element size).
villager is offline   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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Time step size, number of time steps and max iterations per time step guido_88 FLUENT 4 August 30, 2012 14:49
icoLagrangianFoam OF1.6 myNewParticleSolver heavy_user OpenFOAM 16 February 11, 2012 06:15
Time step, Number of time step, Maxximum Iterations per time step sandisk FLUENT 0 July 18, 2011 02:57
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48


All times are GMT -4. The time now is 06:32.