Thanks.

The Froude number of the jet is around 2.8e5. I will take a look at the paper.

EDIT: Sorry, it was the square value of Fr... It actually is around 530!

Hi Jonathan,

A Froude number of 530 seems still high for triggering strong buoyant instabilities, given the length of the simulated domain is not especially long, I would assume it is inertia which destabilizes your jet. Refer "Vertical Turbulent Buoyant Jets: A review of experimental data" by Chen and Rodi (1980) and citing articles for details and backing by references.

A specific formula for such a rather numerical matter is not known to me, but from experience jets get quickly, almost instantly, destabilized if the driving instability is strong enough.

For numerical simulations it is important not to introduce too much numerical dissipation in order to quickly progress to a turbulent state quickly; The cross-section of the jet should be resolved with at least ~25 gridpoints, especially in the shear layer, so that the strong shear at jet exit can effectively develop strong eddies, breaking the jet's symmetry.

Also the initial conditions do matter a lot. You can initialize your jet either using a moving column of fluid, or start by inject into a quiescent fluid. The latter tends to be more turbulent right from the start due to a stronger perturbation, but may lead to spurious effects when leaving the domain at the outflow boundary.

Some researchers added random initial perturbations. They should destabilize the jet quickly but decay such that after the usual few flow-through times where the analysis is discarded there should be no remainder of the same found in your simulation.

Also, when using an eddy viscosity model in the case of LES make sure to check how much additional viscosity it adds. Switching the turbulence model off in the initial period will destabilize your jet more quickly.

Thanks for the help.

But reading your answers, I worry that my question is not clear enough. Maybe I did not used the appropriate terms: I don't want to estimate the duration of my simulation (CPU time), I want to know the time I have to simulate the jet to be fully developed, i.e. 10 seconds? 15 seconds?

Here is some more details about my simulation. I am performing and LES simulation of an air jet of an initial diameter of 4 mm and 105 m/s, injected in a volume of 100 times the diameter. Regarding the initialization, I use the SEM method to introduce some perturbations in the quiescent volume where the flow will develop itself. I simulated around 0.16 seconds of the jet and see some perturbation on the jet, and qualitatively, the results make sense. But I am not able to reproduce velocity profiles, which explains why I would like to estimate this duration.

Using DNS/LES you always need some time to wait for the flow developing, the memory of the initial condition causes a numerical transition that cannot be estimated by a formula as it depends on many factors.

In case you have a statistical energy equilibrium in your problem, the best way is to compute the total energy in the domain and use this integral quantity as a check. You will see that, after several non dimensional time-units, the energy reaches an average level. From that time you can sample the field to compute the statistics you need

In fluent use the unsteady/time-dependent solver and examine velocity or Re against various time, you will get the answer.

Jonathan, I don't think such a formula exists, because each code has each proper convergence scheme. means, for the same code (accelerated or not) the time/ way followed will not be the same even the time step delta_t is the same. Such a case is the with/without multigrid accelerattion. & look more.

Is the flow in the jet relativistic? That can make a huge difference.

The real question here is what are you trying to answer with your simulation? Are you trying to determine the time to reach a fully developed jet flow or are you interested in the structure of the flow is once it is fully developed? If you are doing the latter you might want to start with a coarse domain and run a quick solution to get a flow filed that can be used to initialize your refined domain. And then iterate until you have a converged solution (speed up computational time). However, if you want to simulate time dependent flow evolution you will want to start with the flow field in the domain initialized to zero, run a time dependent simulation and continue until the flow field is converged. I would expect that convergence in real time would be on the order of a few seconds. From my experience with jet flow 15 seconds seems long to me, but the answer lies in whether or not the solver has converged. I am not aware of an analytical answer to the question you pose.

Filippo Maria Denaro has it - in LES/DNS it's all about energy.  The essence of the methods is to resolve (all for DNS, most for LES) the turbulent kinetic energy is it not?  So the evolution of the global amount of kinetic energy is as good as it gets.

In your case - jet entering a large container - could take a really long time.  So prepare good scripts for re-submitting your jobs on the cluster and take a holiday.

To answer to Robert Haehnel, I am actually interested in the fully developed phase of the jet. But, as I am running a LES unsteady solution, I wanted to know the time I need to run to obtain the fully developed state of the jet to see if it is actually matching with my deadline...

I still have to check the energy in my domain to see if my jet is fully developed or not.

PS: Thanks for all the answer!

Even with LES, if you can initialize the flow field with a fully developed flow from a coarse mesh, and then iterate to the solution on the finely resolved mesh you will save yourself a lot of computation time. I have found I can save several days of computation time by running a couple simulations where I double the mesh refinement (coarsest mesh might take 20 minutes, next level of refinement takes a couple hours, then use that as initial conditions for my final simulation).

Just tricks of the trade if your CFD solver can easily ingest a flow field from a coarser mesh for the initial condition. Most allow you to do that, it is just a matter of figuring out how. The time up front figuring it out will save a lot of time getting to your solution.