
[Sponsors] 
April 16, 2012, 23:03 
FLUENT LES Simulation of flow past a cube

#1 
New Member
NGH
Join Date: May 2011
Posts: 15
Rep Power: 6 
Hi
Im simulating the flow past a cube using FLUENT LES model and encountered some issues. The flow is 0.4m/s and the cube is 0.1 m. How many flow through times do I need to get the distinct flow features? After 2 flow through time, the features are still very fuzzy. What could be the problem? Thanks Im using pressure velocity coupling: SIMPLE Gradient:Green Gauss Cell Based Pressure:Standard Momentum:Bounded Central Differencing Transient Formulation:2nd Order Implicit 

April 18, 2012, 02:49 

#2  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 671
Rep Power: 13 
Quote:
For LES, the initialization is VERY important. How did you initialize your case? For LES, typically a RANS solution using your favorite turbulence model is used. Then a random perturbation is slapped onto the solution to force it to transition to turbulence. This random perturbation is very important, if not done properly, the flow will stay laminar! Recall that turbulence is just the amplification and manifestation of small flow instabilities (so for LES you need to provide these instabilities). After the perturbation, you need to run the simulation for enough flow through times for the effect of the perturbation to disappear, I would say 23 flow through times. You can run a few more to be safe. Even if the initial effects are not gone, you should be able to see distinct features by then to know your simulation is proceeding properly. 

April 18, 2012, 22:21 

#3 
New Member
NGH
Join Date: May 2011
Posts: 15
Rep Power: 6 
Hi
Do you mean that I run a RANS solution and then use the case and data file to start LES simulation? How do I introduce the perturbation that you are mentioning in FLUENT Ver 12? Thanks 

April 18, 2012, 22:45 

#4  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 671
Rep Power: 13 
Quote:
Quote:
To my knowledge, this cannot be done in fluent (at least not through any feature in fluent). Maybe you can do some crazy UDF or something. I have always exported my solution data, and then wrote a program to slap random perturbations onto the solution. You can use MATLAB, C, Python, anything programming language that supports reading a text file pretty much. I then import the data into back into fluent and start running. =) The perturbations should not be completely random, since that would add nonphysical velocities. Again, this is all just to give the solver a very good initial guess, so you want very realistic instantaneous velocity distributions to start your LES. A good way is add a gaussianlike perturbation (normal distribution), with standard deviation proportional to the turbulent kinetic energy (or turbulence intensity). Recall the definition of turbulent kinetic energy contains velocity fluctuations. Here is where it really helps to have already solved a RANS case. Using your favorite 2eqn model or otherwise, you would already have solved for the turbulent kinetic energy and can use that for the perturbations. This is my own way of doing it (based on a method originally developed by Jewkes). The perturbation step is not absolutely necessary. In some cases, the flow may become turbulent without the use of perturbations. Even when perturbations are added, in many cases it is very possible for the flow to relaminarize (also very common) if the perturbations are not done well enough. Again, only worry about all this if your flow is not capable of becoming turbulent on its own. Last edited by LuckyTran; April 19, 2012 at 09:34. 

April 19, 2012, 09:25 

#5 
Senior Member

While adding your own fluctuations is what i suggest (i used to do it by a very simple interpreted UDF) as you have more control and sometimes you can avoid the initial RANS computation, you should be aware that, if you have a RANS solution in Fluent you can:
/solve/init/initinstantaneousvel via TUI (or something very similar) and you get your fluctuations in the initial field which, by the way, are based on the spectral synthesizer and are not purely random. However, i don't know the details of your simulation but for a flow over a cube initialization is probably the last problem; if you can't get reasonable istantaneous results after no more than few flow trough times (if you have distinct inflowoutflow boundaries than 1 is just enough) then i would start looking elsewhere (grid size, time step, b.c., etc.). In contrast, if you are talking about average results (after the activation of the flow statistics), then yes, this can be a mess and you could need several tens or hundreds shedding cycles to get proper average results. 

November 12, 2012, 14:00 

#6 
Member
MAZI
Join Date: Oct 2009
Posts: 79
Rep Power: 7 
hi guys
i am running ANSYS 14 to simulate turbulent backward step flow by LES. (http://www.sciencedirect.com/science...07570403001138) in this paper, they plotted fluid velocity in different part of channel. i want to know how can i obtain this velocity profile? after how many seconds should i plot the profiles? i mean how can i find that statistically fluid is steady? and how can i obtain fluctuation and mean velocity component by ANSYS? THANKS 

November 14, 2012, 00:45 

#7  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 671
Rep Power: 13 
Quote:
Fluent can keep track of mean and rms values, you just need to enable "Data sampling for time statistics". fluent keeps a running count of average velocity and rms values starting from the iteration when this option is enabled. It can be reset at any time that you wish to clear the average. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Simulation of steam (CO2 and Water vapor mixture) flow through nozzle using Fluent.  Jimmy  FLUENT  0  March 2, 2011 13:30 
Natural convection  Inlet boundary condition  max91  CFX  1  July 29, 2008 20:28 
Compressible flow simulation using FLUENT  arun  Main CFD Forum  0  February 16, 2004 16:44 
How Fluent treat the pressure term in imcompressible flow  Ray  FLUENT  1  May 24, 2000 16:50 
Simulation of the Flow past a circular cylinder using STARCD  M. S. GUEROUACHE  Main CFD Forum  0  October 1, 1998 10:51 