Courant Number
Hello all:
Is there a way in CFX (using v5.6) to specify a value for the courant number so that the solver will adjust the timestep accordingly to maintain the value? Thanks, Aaron 
Re: Courant Number
CFX5 is fully implicit, why would you want to do this?
Robin 
Re: Courant Number
Robin, Could you please explain your comment a bit more detailed. I did beleive that when doing a transient calculation that the Courant number was important (less or equal to 1 or 5 depending on time scheme) Regards Jan

Re: Courant Number
Even though a scheme might be implicit, if you are doing a transient calculation, the courant number will be important within a given time step. Otherwise, you won't capture the transient behaviour between the timesteps.
Aaron 
Re: Courant Number
This is true of explicit methods, but is not the case for a fully implicit code. Since CFX5 solves the mass and momentum equations in a coupledimplicit manor, you are not restricted by the Courant Number.
Rather, you need to ensure that the equations are converging within your timestep. You should choose a timestep that is small enough to converge within 3 to 5 coefficient loops in order to accurately resolve the transient physics. Robin 
Re: Courant Number
Yes, but, as Robin pointed out already in the other post, since CFX5 is fully implicit, if you take a timestep small enough and converge the solution within a timestep (i.e. global balances and RMS residuals are low enought that you have "solved" the equations) then you do not need to worry about the Courant number.
Furthermore, if the convergence condition within a timestep is achieved then it basically means that you are taking a timestep which is adequately resolving the transient physics. If your timestep is too big then you will not converge within a timestep. Given it's "linear" scheme nature, the Courant number on it's own can never be an adequate measure of how well you are solving an inherently nonlinear problem. Neale. 
Re: Courant Number
Thanks for your reply Robin, I am happy with your answer, cause normally I just calculate the Courant number just to get an idea about the size of if. It is other parameters that determine the size of the time step. I guess the confusion comes from, as I understand it, that the Courant number rather is a stability criteria more than a measure for the transient behaviour of the flow.

what is Courant Number
What exactly is this courant number, can someone throw some light in this regard?
thanks henry 
Quote:
If so, how does this implicit method work? All I know is that backward (or implicit) Euler for example, tends to reverse the energy development of a signal that is being transported (since it's working backwards) if ideally the energy development would be zero. So for example if normal Euler is unstable and will make the energy of the signal exponentially increase, as in an UPWIND scheme with a Courant number > 1, backward Euler would reverse the energy development and instread exponentially decrease it, and tend to lowpass filter the signal that is transported. But for a Courant number < 1, UPWIND is stable and will lowpass filter the signal, thus making the energy exponentially decrease, so wouldn't an implicit method in this case make the energy exponentially increase and thus be unstable? 
Explicit methods take gradients at the current time step and extraplote that forward in time to get the next time step. So the fundamental solution procedure is algebraic. This approach is limited to a Courant number (of CFL number if compressible) of 1.0.
Implicit methods solve the next time step as a set of simultaneous equations, with gradients calculated back to the previous time step. This means a matrix solution is required, but also means the Courant number/CFL number limit does not apply. If you want a more detailed explanation than that I will refer you to any reasonable CFD textbook. The difference between implicit and explicit methods is basic numerical methods. 
Quote:
I needed to know whether the comment regarding the selection of appropriate time steps to allow convergence within 35 iterations is verified and widely accepted. I have been trying to analyse flow over a ramp geometry which induces separation and would like to capture any resulting vortex shedding. Currently using transient simulation, pressurebased, SIMPLE pressurevelocity correction algorithm with all transport and turbulence scalar equations set to secondorder upwind. I started to use the timesteps which allows the streamwise, freestream velocity to traverse the smallest cell size in step. This resulted in 0.002s steps and I have iterations at 40 max/timestep. I did this as a maximal value and there are many timesteps which do not really converge even after 40 iterations. Even after very long runs of 100 timesteps, the residuals for all the transport equations and scalars are all oscillating at a constant frequency. Is there a way to identify what I could be doing wrong here? Should I alter the timestep size to follow the 35 iteration convergence guideline? 
Quote:
Quote:
Quote:
Quote:
You will probably find 35 coeff loops approach give you much smaller time steps, but very fast and reliable convegence in each time step. This is faster, more accurate and more reliable than larger time steps with longer convergence per time step. If you do not believe me then do a simple benchmark simulation where you play with the number of coeff loops and look at the final result. Best do this on a benchmark where you have good reliable benchmark data to compare to  maybe vortex shedding off a cylinder or something like that. Then you can explore this for yourself and I suspect you will too will believe. 
Quote:
I will basically need to perform convergence/sensitivity analysis for this rather than blindly using the timestep suggested by the CFL criteria of 1 (as per my previous attempt). The only problem I imagine is the long lead times involved in trying to identify an appropriate timestep by trial and error. Do you use a general guideline or ratio that is suitable for the refinement or coarsening of the timesteps in such a case, when trying to identify suitable timesteps? I currently don't have access to multiple computers or a cluster so I am stuck with a single workstation so the turnaround for something like this is important. I currently have 4 levels of mesh refinement which relate to each of the steps in my grid convergence and independence study. Should I include all of these in my attempts to find the appropriate timesteps or choose the one deemed 'fine enough'? I am not too sure about this however, I imagine we should use a grid which would completely isolate any convergence issues to the timestep changes rather than due to lack of resolution/discretisation. Comments are greatly appreciated everyone. 
If you are using Fluent then my comments are not applicable. SIMPLE is very different to the coupled solver in CFX and requires a different approach. You might get similar behaviour using the coupled solver in Fluent but I cannot guarantee it.
But your comment is totally right  blindly applying Courant number =1 is not useful. Best to do a sensitivity analysis and determine for yourself what time step it needs. Between mesh sizes you can use Curant number to give you a starting point but it is preferable to repeat the sensitivyt analysis. For general comments on CFD accuracy see "Computational Fluid Mechanics" by Roache, or the excellent summary which has become the Journal of Fluids Engineering Editorial policy: http://journaltool.asme.org/Template...umAccuracy.pdf 
Quote:
The prospect of having to repeat the timestep sensitivity study for each of the meshes is quite daunting though, as previously mentioned. Ultimately the objective of the gridindependence study was to settle on a mesh to use for the simulation so that reliable results could be quoted. I may do this only if the convergent timestep is quite similar to the initial value used with CFL=1, otherwise I will have study the finest mesh and use it's timestep for the others. I already read through the Journal's policy, guidelines and the paper by Roache. Most of his work is very fundamental and given his reputation, they are definitely important to consider however, I am just concerned whether or not it is worth trying to achieve this level of verification given the time limitations of my undergraduate research topic? 
The CFX coupled solver should solve to a defined convergence level much faster than the SIMPLE based methods, but each coeff loop will take much longer. In the end you generally get steady state flows converging considerably faster with a coupled solver, but results are variable with transient simulations  some are faster and some are slower.
Yes, the time step sensitivity study for each mesh level is daunting, that's why in CFX you use 35 coeff loops per iteration and then the solver automatically takes care of it. Very nice, removes a degree of freedom, so to speak. But yes, if you take the fine mesh time step and apply that to everything you will probably be OK  just watch out for roundoff errors causing convergence difficulties. If you use even a few of Roache/Celik's techniques to validate your code that would be impressive for an undergraduate project. The Richardson extrapolation technique is a very nice one which is simple in concept and powerful  check it out. 
Quote:
Last night, I used another mesh which is slightly coarser than the previous with ~1.3M cells. This used the same timestep of 0.002 s and this finally converged within 45 iterations on each timestep. Another interesting technique I have been using is that the steady state solver was used to initialise the URANS simulations. Hence, the URANS was initiated after 1000 steadystate iterations. I am happy with the progress so far and now I will seriously explore my validation options. Thanks for all your guidance everyone. 
All times are GMT 4. The time now is 08:31. 