CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Pressure-Velocity Coupling in CFX

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

Like Tree9Likes
  • 4 Post By ghorrocks
  • 4 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2009, 07:01
Default Pressure-Velocity Coupling in CFX
  #1
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi,
is Pressure-Velocity Coupling in CFX enabled as default? From Fluent, there is an option to chose SIMPLE or SIMPLEC schemes for the Pressure-Velocity Coupling. So I am wondering does CFX has this option? pls shed some lights. Many thanks
LSC is offline   Reply With Quote

Old   May 29, 2009, 10:30
Default
  #2
New Member
 
Join Date: Mar 2009
Location: Berlin
Posts: 21
Rep Power: 7
Adam S is on a distinguished road
so i know, it isn´t enabled by default. but you can fix it in the expert parameters.
Adam S is offline   Reply With Quote

Old   May 30, 2009, 13:20
Default
  #3
Zef
New Member
 
Join Date: Mar 2009
Posts: 12
Rep Power: 7
Zef is on a distinguished road
Pressure-velocity in CFX is implemented using Rhie-Chow algorithm and is enabled by default.
Zef is offline   Reply With Quote

Old   May 30, 2009, 14:13
Default
  #4
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi,

may I know where the setting is? The help files only briefly mentioned about the theory. Pls advice
LSC is offline   Reply With Quote

Old   May 31, 2009, 04:56
Default
  #5
Zef
New Member
 
Join Date: Mar 2009
Posts: 12
Rep Power: 7
Zef is on a distinguished road
What do you really want to do? Turn it off at all or adjust some settings? Keep in mind that any changes in Rhie-Chow algorithm can change solution and/or convergence and therefore are not recommended.
Zef is offline   Reply With Quote

Old   May 31, 2009, 06:25
Default
  #6
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi Zef,

I am actually doing a study on CFD of airfoils and one of my objective is to see how the results would varies with different settings and parameters. So I am wondering is there any settings for Pressure-Velocity Couplings that I can play around with. In Fluent, there are SIMPLE and SIMPLEC for the P-V couplings so I am wondering CFX would have something like this too. Could you shed some light?
LSC is offline   Reply With Quote

Old   May 31, 2009, 09:16
Default
  #7
Zef
New Member
 
Join Date: Mar 2009
Posts: 12
Rep Power: 7
Zef is on a distinguished road
There are two ways to adjust Rhie-Chow parameters in CFX. If you are using version 11 with SP1 then you can turn beta features on. With this option checkbox "Velocity Pressure Coupling" in Solver Control->Advanced Control will appear. There are several parameters in it, but be aware that it is a beta feature and some of these parameters will not actually work. In CFX version 12 "Velocity Pressure Coupling" is not hidden, but contains much less parameters to adjust.

The second was is to use expert parameters. In order to know which of the expert parameters are dealt with Rhie-Chow algorithm, you should ask technical support.

In my opinion none of these settings actually affects on the converged solution. It may affects only on speed of convergence.
Zef is offline   Reply With Quote

Old   May 31, 2009, 10:05
Default
  #8
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi Zef,

currently I only have access to version 11. Anyway, many thanks for sharing with me.
LSC is offline   Reply With Quote

Old   May 31, 2009, 20:07
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,956
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Sorry to be brutally honest, but all the previous replies don't know what they are talking about.

CFX is a fully coupled solver and so the pressure-velocity coupling is inherent in the solution procedure. SIMPLE, SIMPLEC and PISO are required when you have uncoupled solvers like Fluent.

Adam S - Turning PV coupling off does not make sense. You cannot turn it off.

Zef - Rhie Chow is not PV coupling. It is how the pressure is interolated from the nodes to cell centres. The main thing here is to avoid decoupling of adajcent cells. PV coupling is totally different.

LSC - I strongly recommend you not fiddle with the Rhie-Chow settings unless you know exactly what you are doing. 99% of the time there is something else fundamentally wrong with the simulation and this sort of thing will not help.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   May 31, 2009, 23:08
Default
  #10
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi Glenn,

now I understand how it works. Thanks for sharing!
LSC is offline   Reply With Quote

Old   June 1, 2009, 00:05
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,956
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Just to expand my previous answer a bit:

Uncoupled (or segregated) solvers like Fluent solve the 3 momentum equations (ie velocity) sequentially, then using the updated velocity field they calculate the pressure correction equation for continuity. This is repeated until convergence.

Coupled solvers like CFX have all 3 momentum equations AND the pressure equation in the same matrix so they are solved together. It does not need PV coupling as that is taken care of in the matrix solution.

Coupled solvers take more time per iteration and use more memory as the matrix is bigger, but coupled solvers usually converge much faster as you are only converging on the non-linear terms. Segregated solvers need to converge both the non-linear terms and the PV coupling.

Regards,
Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 1, 2009, 00:26
Default
  #12
LSC
Member
 
LSC
Join Date: May 2009
Posts: 58
Rep Power: 7
LSC is on a distinguished road
Hi Glenn,

the add on was very helpful. Now I understand why each iteration in CFX takes a longer time when compared to Fluent. Again, thanks a lot for sharing
LSC is offline   Reply With Quote

Old   June 2, 2009, 06:44
Default
  #13
Zef
New Member
 
Join Date: Mar 2009
Posts: 12
Rep Power: 7
Zef is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Zef - Rhie Chow is not PV coupling. It is how the pressure is interolated from the nodes to cell centres.
It is how velocity in the mass-carrying term is interpolated, not pressure. Rhie-Chow algorithm avoids velocity-pressure decoupling and oscillating solutions. Maybe it is not PV coupling, but in CFX documentation this algorithm is called "Pressure-Velocity Coupling". Are they wrong?
Zef is offline   Reply With Quote

Old   June 2, 2009, 20:15
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,956
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

As you correctly explain, Rhie Chow is how the PV coupling interpolates the pressure. Therefore it is an interpolation scheme, not a PV coupling mechanism. It is, however, an integral part of a PV coupling mechanism so that is why the options are grouped together.

While Rhie-Chow does act on the mass-carrying terms, it does so by introducing a pressure redistribution term. So my original reply was not totally wrong, but not quite right either

Glenn Horrocks
r.mojtaba likes this.
ghorrocks is offline   Reply With Quote

Old   June 3, 2009, 05:01
Default
  #15
Zef
New Member
 
Join Date: Mar 2009
Posts: 12
Rep Power: 7
Zef is on a distinguished road
Hi Glenn,

I understood. Thank you for explanation.

Best regards,
Zef
Zef is offline   Reply With Quote

Old   June 6, 2009, 19:47
Default
  #16
Member
 
AdidaKK's Avatar
 
Mauricio Caamaño Flores
Join Date: May 2009
Location: Punta Arenas, Chile
Posts: 62
Rep Power: 7
AdidaKK is on a distinguished road
Send a message via MSN to AdidaKK
Hello everyone ,im really new in CFD techniques ,and im actually doin my thesis on a problem of combustion chamber in CFX 10.(its a combustion tubular chamber from a HITACHI turbine).

and if CFX doesnt use algorithm like SIMPLE,SIMPLEC,SIMPLER,where can i find the information of the way this software works with velocity-pressure?

sorry for my english

thanks very much

Mauricio Caamaño.
AdidaKK is offline   Reply With Quote

Old   June 6, 2009, 22:05
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,956
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Hi,

Read the documentation. That is the nest place to start and I can't count the number of times I end up saying it. The documentation also has references to more detailed articles about specific bits of the software so if you want to delve deeper you should chase those up.

But as an overview the discussion on this thread should get you started.

Also you should try to get V12, the current version. V10 is quite old and there has been lots of enhancements since then.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 6, 2009, 22:28
Default student in problem
  #18
Member
 
AdidaKK's Avatar
 
Mauricio Caamaño Flores
Join Date: May 2009
Location: Punta Arenas, Chile
Posts: 62
Rep Power: 7
AdidaKK is on a distinguished road
Send a message via MSN to AdidaKK
i have all the documents of ansys cfx ,theory,modelling,tutorials etc... but..i really didint see this subject.

with Rhie-Chow algorithm can i explain how its cfx solves velocity-pressure coupling?.

but ansys cfx 12 really has a difference with cfx 11 or 10?.

thanks very much for your help.
im full studyng all with a book called "Introduction to computatioanl fluids,Malalasekera" i think its a very good book for starter in this problems.

once again thanks very much for your advise.

Mauricio Caamaño Flores
AdidaKK is offline   Reply With Quote

Old   June 7, 2009, 09:06
Default
  #19
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,956
Rep Power: 78
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
Originally Posted by AdidaKK View Post
i have all the documents of ansys cfx ,theory,modelling,tutorials etc... but..i really didint see this subject.
Well look again. It's in the theory manual.

Quote:
Originally Posted by AdidaKK View Post
with Rhie-Chow algorithm can i explain how its cfx solves velocity-pressure coupling?.
As discussed above, Rhie Chow is just an interpolation method. It is used in the PV coupling but it is not a PV coupling method in itself.

Quote:
Originally Posted by AdidaKK View Post
but ansys cfx 12 really has a difference with cfx 11 or 10?.
No big differences to the fundamental algorithm between any of these versions.

Quote:
Originally Posted by AdidaKK View Post
im full studyng all with a book called "Introduction to computatioanl fluids,Malalasekera" i think its a very good book for starter in this problems.
Yes, that is a good book to introduce segregated solvers. But this book only covers segregated solvers from memory (been almost 10 years since I saw the book so my memory is vague) and does not cover coupled solvers such as CFX. I don't know of any textbook discussing coupled solvers other than the CFX documentation and any references in it.

Also note the CFX coupled solver technology came originally from TASCFlow. You may be able to find some old TASCFlow documentation to help describe the basics.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   June 7, 2009, 18:58
Thumbs up
  #20
Member
 
AdidaKK's Avatar
 
Mauricio Caamaño Flores
Join Date: May 2009
Location: Punta Arenas, Chile
Posts: 62
Rep Power: 7
AdidaKK is on a distinguished road
Send a message via MSN to AdidaKK
thanks very very much for your help Glenn, it was very helpful your comments ,i really apreciate your help.

Mauricio Caamaño Flores.
AdidaKK is offline   Reply With Quote

Reply

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
how to define pressure drop with CFX post alex CFX 0 September 20, 2007 18:31
Pressure jump on supersonic velocity inlet Viktor FLUENT 0 August 9, 2007 01:23
How to set pressure BC with mass Velocity Magnitud arwang FLUENT 2 March 12, 2007 22:04
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13
how to print the results from CFX-4.2 cfd_99 Main CFD Forum 5 June 21, 1999 10:23


All times are GMT -4. The time now is 23:48.