
[Sponsors] 
November 26, 2009, 22:34 
Laminar model in Fluent

#1 
Senior Member
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 16 
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 

December 3, 2009, 19:02 

#2 
Senior Member

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. 

December 3, 2009, 22:24 

#3 
Member
Ivan
Join Date: May 2009
Posts: 85
Rep Power: 17 
I had the same confusion. in my understanding, sbaffini meant to say the grid should be finer for more complex flow. is it right?


December 4, 2009, 01:09 

#4 
Senior Member
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 16 
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... 

December 4, 2009, 04:52 

#5 
Senior Member

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 NavierStokes 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. 

December 4, 2009, 12:25 

#6 
Senior Member
karine
Join Date: Nov 2009
Posts: 158
Rep Power: 16 
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 

January 5, 2016, 15:12 
Laminar model  application

#7 
New Member
daniel
Join Date: Sep 2014
Posts: 17
Rep Power: 11 
I have a simulation of interior pipe flow where the Re ranges from 3002000. There are recirculation regions in the geometry. Would utilizing Fluents laminar model yield a useful solution? I am not sure if the turbulent zones will be modeled correctly.


January 6, 2016, 15:33 

#8 
Senior Member
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,712
Rep Power: 66 
Re < 2300 is generally laminar so yes. Of course assuming you are using the same definition of Re.


February 8, 2016, 13:42 

#9 
New Member
daniel
Join Date: Sep 2014
Posts: 17
Rep Power: 11 
Thank you. After some more reading it makes sense. . .
However, now I am facing the issue of finding the documentation of the laminar model and its implementation in Fluent. I am looking for what equation in what form it specifically solves. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Seeking Macroscopic Particle Model in Fluent  bzhang7  FLUENT  3  June 25, 2022 17:54 
How to model "chimney effect" using Fluent?  Feidao Li  FLUENT  10  January 14, 2010 09:43 
Need Help on Fluent Modelling Laminar on BluffBody  ary  Main CFD Forum  1  May 19, 2005 05:59 
Mixing length models and zerohvac model in fluent  sarah_ron  FLUENT  0  November 27, 2004 23:29 
Covert StarCD model to FLUENT  Lam  Siemens  6  June 24, 2003 20:21 