# estimate time step?

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 9, 2005, 08:28 estimate time step? #1 CFD Student 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 Mani 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 semi-empirical 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 CFD Student Guest   Posts: n/a Dear Mani, Thanks a lot for your help. I am about to finish implementing 5-stage explicit dual time-stepping Runge-Kutta scheme into my 2-D finite volume Navier-Stokes solver employing central differencing scheme of JST and Roe FDS together with Baldwin-Lomax turbulence model. Actually, I am completely new to unsteady flow simulation and I don't know what is the best validation case for 2-D 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 ag 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 second-order time differencing over first-order 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 amol Guest   Posts: n/a You can have unsteady inviscid simulations. Richtmyer-Meshkov 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 Mani 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 Mani 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 40-60 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 (dual-time 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 CFD Student Guest   Posts: n/a Nice suggestions for me. Please accept my best regards... CFD Student

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post pUl| FLUENT 31 August 21, 2015 04:46 nileshjrane OpenFOAM Running, Solving & CFD 4 February 25, 2013 05:13 nileshjrane OpenFOAM Running, Solving & CFD 8 August 26, 2010 12:50 m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58

All times are GMT -4. The time now is 10:45.

 Contact Us - CFD Online - Top