
[Sponsors] 
August 9, 2005, 08:28 
estimate time step?

#1 
Guest
Posts: n/a

Dear CFD People,
How do we estimate time step for time accurate computations? Is there any algebraic formula as in the case of estimating the location of first grid point next to the wall. Best regards. 

August 9, 2005, 14:20 
Re: estimate time step?

#2 
Guest
Posts: n/a

If you're looking for a general formula for all time accurate computations... there is none. There can't be one, because the time step you need depends on the time scales that you would like to resolve, and that depends on a number of things: a) the type of flow you're studying, b) the desired accuracy, c) the computational scheme... In addition, the temporal resolution may be limited by the spatial resolution of your grid. Knowing all those parameters, you can assess an apropriate (preliminary) time step. A time (and grid) resolution study will then reveal if you need to decrease the time step, or if you can choose a larger one. Let us know some details of your study and we can give you some concrete hints.
By the way, any "algebraic" formula to locate the first grid point off a wall for viscous flow cannot be general, either. Most likely you would use semiempirical similarity relations for a flat plate to get a first estimate... but only by examination of your CFD result will you see if the resolution was chosen high enough (unless you actually run a flat plate). The general problem with determining the required resolution (both temporal and spatial) is that you would need to know the flow beforehand Since that's not the case, you have to apply some educated guess, the quality of which must be verified by examining your CFD result. Without the latter you cannot claim to have achieved the accuracy you were aiming for. 

August 10, 2005, 02:33 
Re: estimate time step?

#3 
Guest
Posts: n/a

Dear Mani,
Thanks a lot for your help. I am about to finish implementing 5stage explicit dual timestepping RungeKutta scheme into my 2D finite volume NavierStokes solver employing central differencing scheme of JST and Roe FDS together with BaldwinLomax turbulence model. Actually, I am completely new to unsteady flow simulation and I don't know what is the best validation case for 2D unsteady flows. Can you please give me any suggestion? Also, can we simulate inviscid unsteady flows? Is it physically possible that we can have an unsteady inviscid flow? Best regards. CFD student 

August 10, 2005, 08:49 
Re: estimate time step?

#4 
Guest
Posts: n/a

A fairly simple 2D unsteady case is flow around a cylinder. Make comparison to lift and drag coefficients and Strouhal number. A simple shock tube problem is a good case for determining the unsteady behavior of the code also. You should be able to compute the proper shock speed. A third case is inviscid convection of a vortex  this is a good case for quantifying how dispersive/dissipative the scheme is. Can the code maintain the core vorticity, and does the vortex drift off the path it should follow? It also demonstrates the benefits of secondorder time differencing over firstorder time.
Yes you can simulate unsteady inviscid flows. Unsteady inviscid flows are as physically possible as steady inviscid flows (which is not very). 

August 10, 2005, 22:16 
Re: estimate time step?

#5 
Guest
Posts: n/a

You can have unsteady inviscid simulations. RichtmyerMeshkov instability (RMI)is a very popular example of it. You will get tons of paper on the subject (RMI) and is very good code validation problem.


August 11, 2005, 14:20 
Re: estimate time step?

#6 
Guest
Posts: n/a

Incompressible, laminar flow (Reynolds number between 47 and 180) over a cylinder would be a good case, as previously suggested. That should be your first choice, considering the ease of implementation and the availability of experimental data.
Yes, you may start with inviscid flow. Besides the cases suggested in previous posts you can always create unsteadiness by applying unsteady boundary conditions. These cases are often easier to study and handle than the cases where unsteadiness is caused by flow instability (as with the cylinder). Examples for unsteady boundary conditions could be a nozzle (internal flow) with oscillating exit pressure. Another popular case is the oscillating airfoil. There are a lot of data available, experimental and numerical, for the viscous or inviscid flow over a harmonically oscillating airfoil. However, you would need to implement grid motion and include the effect of grid motion on the fluxes. 

August 11, 2005, 14:43 
Re: estimate time step?

#7 
Guest
Posts: n/a

To answer your original question: Taking the cylinder as an example you would choose the time step small enough to resolve the vortex shedding. This is an easy validation case because you know what to expect (from experimental data). The oscillation period of laminar flow is a known function of the Reynolds number. You would choose about 4060 time steps per oscillation period (which defines the time step size) to get a good temporal resolution, while making sure that your spatial resolution is also adequate. For other harmonically oscillating flows you would do the same, starting from an estimate of the oscillation period. If nothing is known about the unsteadiness, it's a lot more difficult to get it right.
This is all under the assumption that you use an implicit scheme (dualtime stepping, in your case). If it's explicit you have additional constraints due to stability issues, so your time step may have to be smaller to make the scheme stable, regardless of the intrinsic time scales of the flow. I recommend you use an implicit scheme. 

August 12, 2005, 01:16 
Re: estimate time step?

#8 
Guest
Posts: n/a

Nice suggestions for me. Please accept my best regards...
CFD Student 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Time step size and max iterations per time step  pUl  FLUENT  31  August 21, 2015 04:46 
SLTS+rhoPisoFoam: what is rDeltaT???  nileshjrane  OpenFOAM Running, Solving & CFD  4  February 25, 2013 05:13 
Error while running rhoPisoFoam..  nileshjrane  OpenFOAM Running, Solving & CFD  8  August 26, 2010 12:50 
Modeling in micron scale using icoFoam  m9819348  OpenFOAM Running, Solving & CFD  7  October 27, 2007 00:36 
IcoFoam parallel woes  msrinath80  OpenFOAM Running, Solving & CFD  9  July 22, 2007 02:58 