calculation of time for CFD simulation
 

I am learning to use CFD using Ansys CFX. I know that The length of time required to complete a CFD simulation depends on the length of the simulation, the number of grid cells (assuming that you are doing a numerical simulation) and the time-step of calculations. The numerical integration scheme, the implementation of the software and the details of the hardware also make a difference.
But is there is any way to calculate total time required to complete a simulation?

Thank You

The answer to your question is generally no. But there are some instances where you can perhaps generate some estimates.

For steady-state solutions (pressure and density based), you generally have no idea how many iterations/pseudo-timesteps it will take to reach your convergence tolerance. You cannot reliably generate estimates based on rates of convergence, because initial residuals tend to drop quickly and then stall later. Some simple flow cases may seem to be predictable, but for any complicated flow at all, this won't be the case in my experience. The only way you can really find out is to run the job and see. But, if you are running similar geometries with similar operating conditions on a similar computer, your time for your new jobs will likely be close to those of your initial job. Generally, you cannot think that doubling the number of cells will double your solution time...it may well MORE than double solution time. Just like doubling the number of CPU cores you use will half the solution time. This is true for all steady-state approaches, AFAIK.

For transient simulations, the situation is a little better--at least if you are using fixed timesteps and fixed spatial grids. If you start your solution and you time the execution of some relevant interval of timesteps. If your simulations contains some significant temporally varying phenomena (vortex shedding, bubble bursting, flame oscillation, etc), your timing interval should contain at least one of those phenomena. Then, you can likely use that estimate how long the rest of the simulation time will take. It should be reasonably accurate as long as no huge flow changes occur later in the simulation. For simulations like, say, simulation of internal combustion engines, that moving flame front will make the compute time very unpredictable (in my experience anyway). This will also be the case with adaptive time stepping or adaptive meshing schemes (though you often use adaptive time stepping/meshing is these problems anyway).

There is a small class of CFD solvers that do have fairly predicable runtimes. These are explicit time integration scheme...usually density based. Again, without adaptive time stepping and fixed resolution grids, these solvers have (more or less) a fixed amount of work they do per timestep. In this case, you can average the time required for just a few timesteps and scale that up to the full solution time.

Finally, some CFD solvers offer a time estimate for when the solution will complete. These are generally inaccurate (often laughably so!). This is for all of the reasons above. But they tend to average over the whole of the simulation time processed, so they generally get more accurate, the longer the simulation goes, so they can offer some indication. I just hesitate to call any of these "predictive" except maybe for the explicit CFD solvers with fixed timesteps and grids.

Just to say that for laminar steady flow problems, the time-dependent alghoritm has a characteristic steady time of the order of the Reynolds number. More complex is the case of fully unsteady flows where often one runs the code for many time units to accumulate several fields.

Comparison between RANS and LES for fluidic oscillator
 

I want to do a comparative study of flow field in fluidic oscillator using both RANS and LES. My computaitonal domain in 10 * 4 * 2.5 cm across. I am working with flow range between 25 m/s to 100 m/s or (0.075 m2/s to 0.3 m2/s) which falls in the Reynolds number range between 10000-60000.

I have done URANS simulation using CFX and moving into LES simulations. What are the meshing rules for LES ? What considerations I have to make for such calculation?

How to get rough estimation of computational time required between a URANS simulation and LES simulation using CFX ? Hardware I am using is intel i7 @3.40 GHZ with 32 GB RAM.

Thank You

The two formulations are very different, therefore you have to consider that LES requires a very fine grid for inhomogeneous flow directions (e.g. walls where you need 3-4 nodes within y+<=1). You have also to consider that after the LES solutions reached a fully developped flow condition (that is after the numerical transient has ended) you need further computation time to cumulate several fields in time for computing the statistics.

Meshing requirements for LES
 

I am using Ansys CFX for LES simulations of internal flow field of fluidic oscillator. I am working with velocity range 25m/s to 100 m/s i.e reynolds no. 10000 to 60000. My computational domain is 25 cm* 15 cm * 25 mm. What would be the meshing requirements for LES simulation ? what are the considerations for LES simulations

Thank you

In general, you need to have such a mesh that is able to capture the large scale eddies while only small eddies need to be modeled. The larger Re, the smaller mesh size is required. The rule is that the mesh size should be in the inertial range of turbulence. There are some formulas that allow you to approximate the turbulence length scales based on turbulence quantities. These give you an idea about the order of the turbulence length scales (representative value). What you should do is to test how your results change when you change the mesh size - although this has two catches. One is that LES simulations are computationally expensive and so it is a pain to run several test cases. The second catch is that as you decrease the mesh size, more and more eddies should be resolved and less modeled. So one cannot talk about grid-independency like in case of the RANS simulations.

A separate chapter is how to resolve the boundary layer. The turbulence length scales near the walls are extremely small and that's why you need to refine your mesh here. That is usually unfeasible. There are methods that can alleviate this issue, such as WMLES or DES. I personally use LES only for cases where I am not interested in boundary layer else it would become too expensive.

LES modeling is an extensive topic. If you want to know more, you should seek for a dedicated literature.