# Re: Segregated Solver option in FLUENT 13

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 1, 2013, 06:40 Re: Segregated Solver option in FLUENT 13 #1 Member   Yash Ganatra Join Date: Mar 2013 Posts: 67 Rep Power: 6 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: 13 The default algorithm for FLUENT is segregated. OJ rgd likes this.

 June 1, 2013, 12:52 Re: Segregated Solver Option in FLUENT 13 #3 Member   Yash Ganatra Join Date: Mar 2013 Posts: 67 Rep Power: 6 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: 13 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   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,399 Blog Entries: 6 Rep Power: 45 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 300-400 iterations for segregated to 25-30 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: rgd, sargordan, lizard_asl and 1 others like this. 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: 6 Thank you very much

July 12, 2016, 00:47
#7
New Member

Senthilkumar
Join Date: Oct 2012
Posts: 19
Rep Power: 7
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:
 Originally Posted by Far 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 300-400 iterations for segregated to 25-30 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:

July 12, 2016, 06:30
#8
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 2,008
Rep Power: 27
Quote:
 Originally Posted by aero.senthilkumar 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
Just take them as guidelines. Both can work, but the density based algorithm handles strong coupling much better than the pressure based solver.

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 P-V 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: 19
Rep Power: 7
Thank you very much, Lucky Tran.

Quote:
 Originally Posted by LuckyTran Just take them as guidelines. Both can work, but the density based algorithm handles strong coupling much better than the pressure based solver. 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 P-V 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.

 Tags fluent 13.0, natural convection, segregated solver, solvers

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post HMR CFX 5 October 10, 2016 05:57 hadi.iraji CFX 1 May 7, 2013 04:03 EtaEta CFX 7 December 8, 2011 18:15 Sas CFX 15 July 13, 2010 08:56 saii CFX 2 September 18, 2009 08:07

All times are GMT -4. The time now is 17:52.