CFD Online URL
[Sponsors]
Home > Forums > FLUENT

Coupled solver, computational cost

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 18, 2013, 07:29
Default
  #41
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
This is the post where Re=40 results are posted and mesh file link is also provided. Fluent + flow past cylinder at Re=40

Boundary conditions wre:

Dia = 1 m (necessary for Reynolds number)

Density = 40 Kg/m3

Viscosity = 1

Velocity = 1 m/sec

You can check your self how fast is coupled solver.

Yes you are right memory requirements are high, approximately twice of SIMPLE
Far is offline   Reply With Quote

Old   April 18, 2013, 07:56
Default
  #42
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 10
oj.bulmer will become famous soon enough
I am not suspecting the idea. Personally, am a big fan of CFX's multigrid coupled solver. In one of the cases involving porous interface, for same mesh/physics, CFX converged within 80 iterations while FLUENT had to go till 1000!

I just like to observe things in totality

Cheers
OJ
oj.bulmer is offline   Reply With Quote

Old   April 18, 2013, 07:59
Default
  #43
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,902
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Are you talking about Fluent 14 + versions. One thing should be noted that in CFX CFL is not provided as option to user and it is decided by solver.
Far is offline   Reply With Quote

Old   April 18, 2013, 08:27
Default
  #44
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 10
oj.bulmer will become famous soon enough
Yes, 14.5. Also, given sudden change of properties across the porous interface, I typically use local timescale option instead of auto/physical timescale, which smartly changes the timescales globally (ie, equivalent to variable CFL).

But of course you can always provide aggressive local timescale factor for faster convergence. Some opine that it is necessary to run last few iterations using Physical/auto timescale, while some think running local timescales "enough" is sufficient, ie when we witness flatter monitors and reduced imbalances.

OJ
oj.bulmer is offline   Reply With Quote

Old   April 18, 2013, 16:59
Default
  #45
Senior Member
 
François Grégoire
Join Date: Jan 2010
Location: Laval University, Canada
Posts: 339
Rep Power: 7
macfly is on a distinguished road
Quote:
Originally Posted by oj.bulmer View Post
Oh well, I think there is a bit confusion over the concept of under-relaxation. There are two types:

1) (Explicit) Under-relaxation of variables: For pressure-based coupled algorithm, this would under-relax the individual variables in inner iterations. Notice that the under-relaxation type for momentum and pressure is EXPLICIT!

2) (Implicit) Under-relaxation of equations: For pressure-based coupled algorithm, CFL applied tries to under-relax the equations through full IMPLICIT coupling. The choice of CFL will influence the local timescale and eventually the solution of the equations, as specified in earlier (long) post. Essentially when CFL is used, the separate under-relaxation of flow equations is not needed. But for turbulence equations, URFs still needs to be specified.

Typical values of Explicit URFs (in pressure-based coupled case) for pressure/momentum being 0.75, it can be further increased to accelerate inner iterations. But for higher order schemes for momentum etc, often it needs to be reduced to say 0.5 etc, with very bad meshes requiring further reduction at times. Any divergence in AMG solver should indicate the high CFL value, which needs to be reduced.

OJ
Ok, got it. Sorry to waste your time. Thanks.
macfly is offline   Reply With Quote

Old   August 1, 2013, 05:21
Default
  #46
New Member
 
Daan de Boer
Join Date: Jun 2012
Posts: 6
Rep Power: 4
daandb is on a distinguished road
Quote:
Originally Posted by oj.bulmer View Post
Oh well, I think there is a bit confusion over the concept of under-relaxation. There are two types:

1) (Explicit) Under-relaxation of variables: For pressure-based coupled algorithm, this would under-relax the individual variables in inner iterations. Notice that the under-relaxation type for momentum and pressure is EXPLICIT!

2) (Implicit) Under-relaxation of equations: For pressure-based coupled algorithm, CFL applied tries to under-relax the equations through full IMPLICIT coupling. The choice of CFL will influence the local timescale and eventually the solution of the equations, as specified in earlier (long) post. Essentially when CFL is used, the separate under-relaxation of flow equations is not needed. But for turbulence equations, URFs still needs to be specified.

Typical values of Explicit URFs (in pressure-based coupled case) for pressure/momentum being 0.75, it can be further increased to accelerate inner iterations. But for higher order schemes for momentum etc, often it needs to be reduced to say 0.5 etc, with very bad meshes requiring further reduction at times. Any divergence in AMG solver should indicate the high CFL value, which needs to be reduced.

OJ
Thanks for the great explanation so far! What i still dont really understand is why these two different under-relaxation (implicit/explicit) are not present with the segrated solver (in any casethey cant be changed). I guess this is due to the fact the coupled and segrated solver work differently. Can you explain me what the difference is between them and how this corralates to the difference in the under-relaxations settings?
daandb is offline   Reply With Quote

Old   April 19, 2014, 08:02
Default clarification
  #47
Senior Member
 
Join Date: Mar 2010
Location: Cape Town, SA
Posts: 141
Rep Power: 7
Jonathan is on a distinguished road
Dear OJ,

Thanks very much for this post. It is very helpful

Could i just ask a few additional questions if possible? According to some documentation i found on the web produced by ANSYS, the Courant No. in the context of the PBCS in Fluent affects the diagonal dominance of the coefficient matrix, and therefore the solution stability - and this is clear in the context of linear solver convergence theory etc. Effectively, this does the same thing as the implicit URF's in the segregated solvers ...

However, in one of your posts below, you mention the explicit under-relaxation (relaxation of variables) affects the inner loops of the PBCS? Could i ask you to clarify this further? Do you mean the linear solver loops? i.e. PBiCG solver loops etc? Or where exactly in the algorithm are the explicit URF's applied?

I know in OpenFOAM, for instance, in their SIMPLE implmentation, they use explicit under-relaxation for the pressure equation, but implicit (equation) URF's for MOM, TKE and Eps etc.

I wonder if you would mind explaining this a little further?

Also, in your current (this) post, you use the following nomenclature:

Quote:
\Delta t = CFL * \Delta t^*, where \Delta t^*= \frac{\rho \Delta V}{a_P}.
I was wondering whether you could just explain your nonemclature? obviously \Delta t is time ... is \Delta V cell-volume, i.e. mesh size? Also i am assuming \Delta t^* is some sort of global time step??

Quote:
One of the most important aspect of using this formulation instead of under relaxation factor \alpha is that with CFL you have a wider range of advancement factors. Under relaxation factors of 0.9,0.95 and 0.99 imply CFL values of 9, 19, 99 respectively. Thus use of CFL gives a wider (or refined) range of pace-change than URF..
I never thought of it this way - that is very helpful! thanks!

Finally - could you comment on how the explicit URF's affect the simulation behaviour? As per above, i know Courant No. in this context affects the convergence stability - how then do the explicit URFs participate? Are they related somehow to the need to deal with the governing equation non-linearities?

Again, thanks very much for the post,
best regards
Jonathan

Last edited by Jonathan; April 22, 2014 at 11:56.
Jonathan is offline   Reply With Quote

Reply

Tags
cfl, coupled, courant, under-relaxation factor

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Some confusion about coupled solver for incompressible flow bearcat Main CFD Forum 0 February 14, 2010 21:40
coupled solver (again) lucioantonio FLUENT 0 April 8, 2009 17:15
Coupled solver energy equation problem lucioantonio FLUENT 0 April 3, 2009 11:21
coupled solver wont work in star ccm+ richie CD-adapco 5 November 4, 2008 05:51
Re: Coupled solver + RNG K-e Model JN FLUENT 1 April 22, 2001 17:34


All times are GMT -4. The time now is 09:38.