CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   Laminar model in Fluent (http://www.cfd-online.com/Forums/fluent/70537-laminar-model-fluent.html)

thecfduser November 26, 2009 23:34

Laminar model in Fluent
 
Hi all,

the laminar model in Fluent, is it the same than a DNS????
In fact this model resolves the NS equations so with an unsteady solver and unsteady boundary conditions, it must be a DNS no?

thanks and regards

sbaffini December 3, 2009 20:02

Hi,

roughly speaking yes, a DNS is necessarily a simulation without any model, a "laminar" one in the parlance of the available viscous models in Fluent.

However a correct DNS also requires that all the relevant flow scales are CORRECTLY resolved, not just resolved, on the grid. Hence, according to the discretization method it requires different grid resolutions.

ivanbuz December 3, 2009 23:24

I had the same confusion. in my understanding, sbaffini meant to say the grid should be finer for more complex flow. is it right?

thecfduser December 4, 2009 02:09

hi
as far as i know, they call it laminar because this model will never converge for a turbulent flow....u will need a very fine mesh : y+=0.1
and an unsteady solver to perform a DNS
Fluent user manual is not so clear anyway...

sbaffini December 4, 2009 05:52

Let me put it in this way:

1) Direct Numerical Simulation means that you directly simulate all the relevant scales of the flow, hence without any additional turbulent model.

2) The Navier-Stokes equations do not change form between laminar and turbulent flows

3) The minimum lenght which need to be correctly resolved in DNS, say for homogeneous isotropic turbulence in a box of side L0, is:

L= L0*O(Re^-3/4)

4)Now, for the given Re, if you just use a grid with dx=L without concern about the numerical method used for the simulation than you are probably committing a mistake. Indeed, for a given grid, nearly all the numerical methods introduce some error which, for consistency reasons, is concentrated around the smallest scales resolvable on the grid

5) Say, for example, that the numerical method used correctly resolve only half of the scales resolvable on the grid, that is:

SCALES RESOLVABLE ON THE GRID

Largest = L0
Smallest = 2dx

SCALES CORRECTLY RESOLVED BY THE METHOD

Largest = L0
Smallest = 4dx

In this case, to have a DNS you have to ensure that 4dx=L, that is dx=L/4.

6) Say, for example, that the numerical method used correctly resolve only 1/5 of the scales resolvable on the grid, that is:

SCALES RESOLVABLE ON THE GRID

Largest = L0
Smallest = 2dx

SCALES CORRECTLY RESOLVED BY THE METHOD

Largest = L0
Smallest = 10dx

In this case, to have a DNS you have to ensure that 10dx=L, that is dx=L/10. And so forth.

7) Whatever the method used and the Re are, there is certainly a grid fine enough to properly perform a DNS, you have only to ensure that the error of the method is concentrated well inside the dissipative range of the spectra (say, where the energy per wavelenght is O(10^-12 - 10^-14))

8) Is any numerical method suitable for DNS? It goes without saying that i would never use a method such that i need dx=L/10 but i'd prefer something like dx=L/4 or even larger. It is usually performed with spectral methods.

9) In any case, DNS is necessarily 3D and unsteady but nothing different from a laminar computation. You have to understand that the laminar mode in fluent does not mean that there is something forcing the solution to be laminar. It is just a simulation without any model.

thecfduser December 4, 2009 13:25

Hi Paolo,
u are always here for help:)
in fact like i said be4 (after a small research), the laminar model in FLUENT is DNS and they call it laminar because if u want to perform it for a highly turbulent flow, u will need years to converge.... But anyway, the laminar model in FLUENT suffers from a problem, and is that u cant specify turbulence (random fluctuations) at an inlet. You can do this only with LES....There is sometimes some small asumptions also (since u have some options in this model)

I have a question Paolo not on DNS (sorry for bothering all time):
i have read that unseatdy RANS can perform unsteady calculations. I tried several cases and thes result was always steady.......So is is true that URANS can perform as unsteady models for a single phase flow????? (in multiphase, it can give unseadt results)

Thanks again


All times are GMT -4. The time now is 08:53.