
[Sponsors] 
July 27, 2013, 11:52 

#21 
Member
Harry
Join Date: May 2013
Posts: 68
Rep Power: 4 
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? 

January 16, 2014, 07:10 

#22  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 473
Rep Power: 6 
Quote:
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 

January 16, 2014, 07:18 

#23 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19 
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 steadystate 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. 

January 16, 2014, 07:24 

#24  
Senior Member
Meimei Wang
Join Date: Jul 2012
Posts: 473
Rep Power: 6 
Quote:
__________________
Best regards, Meimei 

January 16, 2014, 07:35 

#25 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,097
Rep Power: 19 
If the flow is really timedependent, 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 timedependent, 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 longtermsolution 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 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 10100 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 100010000 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. 

February 11, 2015, 07:58 
time step size in vof method

#26 
New Member
enass
Join Date: Feb 2015
Location: AlexandriaEgypt
Posts: 3
Rep Power: 2 
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?


April 13, 2015, 04:36 
Global Courant Number in Fluent 15.0

#27 
New Member
Rubegan
Join Date: Apr 2015
Posts: 1
Rep Power: 0 
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. 

May 12, 2015, 20:04 

#28  
Member
John M.
Join Date: Jul 2011
Posts: 57
Rep Power: 6 
Quote:
http://capeforum.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 multistage 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 meshbased 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 timestep, the results should converge to some values (it's like mesh convergence, just refining timestep instead of mesh element size). 

Thread Tools  
Display Modes  


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 