
[Sponsors] 
June 1, 2013, 06:40 
Re: Segregated Solver option in FLUENT 13

#1 
Member
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 5 
I am working on a natural convection problem and after going through some of the discussions I found that it's better to start with a SEGREGATED solver.
However, I am unable to located that in FLUENT 13. Can someone please tell where is that option? The tutorials I have referred use FLUENT 6 and it's fairly easy to spot the option there. I am able to locate pressure and density based solver though. Thanks in advance, Yash 

June 1, 2013, 12:02 

#2 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12 
The default algorithm for FLUENT is segregated.
OJ 

June 1, 2013, 12:52 
Re: Segregated Solver Option in FLUENT 13

#3 
Member
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 5 
Thank you for your reply. But suppose a plot is plotted, in the bottom right side of the display window it's written FLUENT(2dp,pbs.....) whereas for FLUENT 6 it is clearly written segregated.
Suppose we want to make it Coupled how can we change? Thanks, Yash 

June 1, 2013, 13:05 

#4 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 12 
The by default pressure velocity coupling method is SIMPLE which is segregated method. Use a drop down menu to select coupled instead.
Have a look at FLUENT documentaiton. These are pretty basic questions. OJ 

June 2, 2013, 04:59 

#5 
Super Moderator

There are three type of solvers in Fluent :
1. Pressure based (segregated in older version Fluent 6.3 ) Here transient flows are solved in implicit manner Options available are : SIMPLE, SIMPLER, SIMPLEC 2. Density based (Coupled solver in older version). Here you have two options for transient simulation. Either implicit or explicit. Explicit is recommended when time step is of same order as CFL ~ 1 other implicit is recommended. 3. Pressure based coupled solver (new addition) : It is mix of above two solvers. It is recommended when velocity  pressure coupling is strong and gives you solution in less no of iteration than pressure based segregated solvers (for example 300400 iterations for segregated to 2530 for coupled pressure solver ) How to make choice 1. For higher Mach no flows (higher compressibility effect). Choose density based with implicit option. It is memory pig and may require double RAM as compared to segregated solver. 2. For low Mach no flows if accuracy is more important use pressure based coupled solver. Pressure based coupled solver can also be used for moderate Mach no. 3. For flow where coupling is loose between pressure and velocity field use segregated solver (pressure + SIMPLE type) PS: Last edited by Far; June 2, 2013 at 06:08. 

June 2, 2013, 08:17 
Re: Segregated Solver Option in FLUENT 13

#6 
Member
Yash Ganatra
Join Date: Mar 2013
Posts: 67
Rep Power: 5 
Thank you very much


July 12, 2016, 00:47 

#7  
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 11
Rep Power: 5 
Dear Far,
Thanks for your explanation. But still, I have doubt about Mach number part. Can we consider moderate Mach number as approximately supersonic Mach number less between 1.5 to 2.5. If I am wrong please explain with approximate values about Mach number. Regards, Senthilkumar Or Quote:


July 12, 2016, 06:30 

#8  
Senior Member
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,298
Rep Power: 20 
Quote:
Coupled algorithms are huge memory hogs but they can converge in fewer iterations per simulation at the expense of more memory and longer computational times. But if you could tune the segregated solver so that it converges, generally the segregated solver has a shorter computational time needed at the expense of more iterations. As long as it doesn't diverge, the segregated solver is one of the best places to start. For natural convection problems, the PV coupling is extremely weak and the segregated algorithm is definitely appropriate. You also don't have large changes in enthalpy so the density based solver does not really give you any advantages. Unless... you have a high Mach number natural convection problem which is a very exotic problem. 

July 12, 2016, 08:53 

#9  
New Member
Senthilkumar
Join Date: Oct 2012
Posts: 11
Rep Power: 5 
Thank you very much, Lucky Tran.
Quote:


Tags 
fluent 13.0, natural convection, segregated solver, solvers 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How tensor parameters to be entered in CFXpre?  hadi.iraji  CFX  1  May 7, 2013 04:03 
CFX13 Post Periodic interface  EtaEta  CFX  7  December 8, 2011 18:15 
Domain Imbalance  HMR  CFX  3  March 6, 2011 21:10 
Constant velocity of the material  Sas  CFX  15  July 13, 2010 08:56 
mass flow in is not equal to mass flow out  saii  CFX  2  September 18, 2009 08:07 