hi, i am trying to made DNS simulations in natural convection by fluent,can i do it ? thank you

I'm sorry but Fluent has not direct numerical simulation.

Maybe using LES with a grid on the Kolmogorov size and a time step size equivalent with no SBG viscosity via UDF...

Even so there is the problem of the discretization of the equations... try it...

Lourival

You have just to choose the laminar model (so no model)...this is DNS. The convective scheme could also be an upwind (instead of the central one) because the cut of this scheme (in the spectral space) is compatible with the natural cut in the flow so you don't loose so much in using such a scheme.

So the only and one thing you need to do before doing DNS in fluent is the VERY VERY VERY FINE grid.

The question is: is there a real reason to do DNS in Fluent with milions of cells just for simple flows (square cavity) and GBs of memory for few seconds?

I think you wrong. In such case you do not have pulsations on inlet and everywhere in domain.

This is about the inlet boundary condition. But you can always use an UDF. In the square cavity there is no inlet so there is no problem. Activating the LES in fluent just to use the synthetizer in a DNS is at least crazy. But i think that everything about DNS in Fluent is crazy. Maybe with the density based explicit solver there are some chances to do it.

But what about the flow? Are you saying that the turbulence is caused by the turbulent model or what?

DNS means Direct Numerical Simulation; Direct means no model because the grid is fine enough to simulate every scale in the flow, from the biggest ones down to the dissipative scale (kolmogorov). If your grid is fine enough you don't need any model so...just use the laminar model.

Even if the inlet is laminar, the flow can become turbulent, right? Also in a square cavity, if there is a temperature difference strong enough or one of the sides slides fast enough, the flow can become turbulent, right?

The question is: what should i do to correctly simulate this turbulence? There are two ways:

1)With space and time scales small enough to capture all the flow characteristics (small dx and dt)...you can just simulate it as laminar, so no model; if the flow is turbulent you will see it.

2)Due to memory and computing resources, the space and time steps can't be small enough...use a turbulence model. Depending on the amount of resources you choose between LES or URANS.

That's it. But DNS means no model and a fine enough grid.

think you valerio,lourival,paolo bubua, yes ,very very fine grid in DNS ,but the geometry is complex and 3D with different temperature in the walls,how about the inlet boundary conditions?

thank you valerio,lourival,paolo bubua, yes ,very very fine grid in DNS ,but the geometry is complex and 3D with different temperature in the walls,how about the inlet boundary conditions?

"You have just to choose the laminar model (so no model)"...

1st: why would it say laminar MODEL in the first place! You should realy check the gouverning equations on this one (I haven't got the manual right now...)

2nd: every flow can become turbulent depending on sufaces, velocity (mass transfer rate) etc... etc..

anyway: are you combining physics in your model Jenny? or are you just simulating flow conditions? You'll need a very fine grid indeed for DNS. Dependig on the size of the geometry, wheather or not you're simulating heat transfer (for example) and the available computer power, it can be done.

I'm not sure how far you will come when only solving flow conditions, but in my research (validating DNS solvers by measuring flow and temperature in a real scale model and solving a convective flow, combining heat transfer and flow, using DNS on the computer), it is almost inpossible to solve models larger that roughly 0.2x0.15x0.1 5 (i'm using a simple geometry). Because the straight Navier-Strokes equations leave so many valid outcomes to satisfy the equations, models are very/very sensitive to boundry conditions/grid conditions and solver settings.

Dennis,

I think the LES it most right choise to model semi-DNS problems on state-of-the-art PC.

What i really said is simply:

"DNS means no model and a fine enough grid"

How this is achieved in Fluent?

1) Create the very fine grid

2) Define -> Models -> Viscous... -> Laminar

Or, but is more time consuming, use a LES model with Cs=0 and the same grid as above.

The questions were rethoric...i know what turbulence depends on, i was answering to bubua who wrote:

"I think you wrong. In such case you do not have pulsations on inlet and everywhere in domain."

That's all.

The DNS modelling need not only fine mesh and time step. The DNS need special methods of discretization of equations. And maybe much more... i am not deep specialist in this.

If you only refine mesh and time step this is not give right turbulence modelling.

Of course (even if i think that down to the dissipative scale the convective flux discretization is not so important as in LES; that is, the spectral cut of the scheme should be near the dissipative scale).

But in Fluent this is the only thing you can do:

2nd order time advancement (probably the density based explicit scheme) - 2nd order convective flux discretization (upwind - central) or 3rd order convective flux discretization.

Just to be more clear, i'm not saying that performing DNS in fluent is simple (instead i'm saying it's difficult and crazy, insane, there is no sense at all in performing DNS in Fluent).

What i'm saying is that performing a DNS means that you have a grid and time step fine enough that you don't need any turbulence model. This in Fluent means Laminar model.

Laminar model doesn't means that there is a particular model that will force the flow to remain laminar. It just means no model.

What's wrong with this?

Hi all,

Im Aravind Rohan currently working in DNS of separation in shear layer. Im running a case using DNS in fluent. I got my grid very fine and I ran the case.

My domain is a rectangulat duct with wall at bottom, top outflow and inlet and outlet.

I ran the case for 2500 time steps to get the steady state and another 2000 time steps to get time averaged values.

The problem I encounter is that the Instantaneous velocity at the wall is not equal to zero which makes it difficult to find the separation point.

What could be the problem??? Is there something wrong with the boundary conditions???

Thank You Aravind Rohan.

[Volker P.]

Originally Posted by Paolo Lampitella
;150742

You have just to choose the laminar model (so no model)...this is DNS. The convective scheme could also be an upwind (instead of the central one) because the cut of this scheme (in the spectral space) is compatible with the natural cut in the flow so you don't loose so much in using such a scheme...

Is this also valid for forced convection flows?