[yashganatra]

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

[oj.bulmer]

The default algorithm for FLUENT is segregated.

OJ

[yashganatra]

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

[oj.bulmer]

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

[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:

[yashganatra]

Thank you very much

[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

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:

[LuckyTran]

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.

[aero.senthilkumar]

Thank you very much, Lucky Tran.

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.