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

What is CFX solver? Pressure-based; Density_based; or Combined?

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

Like Tree3Likes
  • 1 Post By ghorrocks
  • 1 Post By Far
  • 1 Post By mohammad

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 16, 2012, 06:38
Smile What is CFX solver? Pressure-based; Density_based; or Combined?
  #1
Senior Member
 
mohammad
Join Date: Dec 2010
Location: UK
Posts: 245
Rep Power: 16
mohammad is on a distinguished road
Dear all,
I want to know some information about CFX11 software. Is it CFX solver a Pressure-based,a Density_based or a Combined solver?

Please also do me a favor and kindly give me a reference for your reply this question.

Regards,
mohammad is offline   Reply With Quote

Old   February 16, 2012, 06:50
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Pressure based, reference: The CFX documentation.

ps: I do not know what a "combined solver" is, in terms of the p-v coupling.
ghorrocks is offline   Reply With Quote

Old   February 16, 2012, 13:53
Default
  #3
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,553
Blog Entries: 6
Rep Power: 54
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
coupled pressure based, finite element finite volume
Far is offline   Reply With Quote

Old   February 16, 2012, 21:18
Default
  #4
Senior Member
 
mohammad
Join Date: Dec 2010
Location: UK
Posts: 245
Rep Power: 16
mohammad is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Pressure based, reference: The CFX documentation.

ps: I do not know what a "combined solver" is, in terms of the p-v coupling.
Quote:
Originally Posted by Far View Post
Far: coupled pressure based, finite element finite volume
Dear Far, Dear Glenn Horrocks

According to my experience,
1-FLUNET has sensitivity problem to aspect ratio. Does this coupling solves that problem in CFX?
2-Some other CFD codes (e.g. ONERA project) need some "Low Mach Preconditioning " for low speed flows to solve the error resulting from compressiblity problem in N-S. Does the above coupling in CFX help for this matter?
3- Deos CFX considers incompressible flow when using "subsonic" option for inlet velocity?

Regards,
mohammad is offline   Reply With Quote

Old   February 17, 2012, 05:19
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
1) All solvers have degraded performance on high aspect ratio elements. I have heard rumours that Fluent is especially suseptible to this, I have no idea. I suspect CFX is better than Fluent here but that is only a guess.
2) CFX is a pressure based solver which needs no special correction at low Mach number. It is the density based solver which need help at low Mach number as there is not sufficient density variation to be resolved adequately.
3) CFX uses incompressible flow when you set it to constant density fluid and compressible flow when you select a compressible fluid. The subsonic inlet option is only available when you have selected a compressible flow option.
marcolovatto likes this.
ghorrocks is offline   Reply With Quote

Old   February 17, 2012, 09:41
Default
  #6
Senior Member
 
mohammad
Join Date: Dec 2010
Location: UK
Posts: 245
Rep Power: 16
mohammad is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
1) All solvers have degraded performance on high aspect ratio elements. I have heard rumours that Fluent is especially suseptible to this, I have no idea. I suspect CFX is better than Fluent here but that is only a guess.
Dear Glenn Horrocks;
I have some experiences about this....this is true. I solved several 2-D and 3D models with different aspect ratios in both CFX and Fluent.
Fluent is more sensitive and even this matter causes divergences or very inaccurate results.
mohammad is offline   Reply With Quote

Old   February 18, 2012, 07:17
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Recent versions of Fluent have a coupled solver which is very close to the CFX solver. Did you use this, or the default SIMPLE based solvers?
ghorrocks is offline   Reply With Quote

Old   February 18, 2012, 11:51
Default
  #8
Senior Member
 
mohammad
Join Date: Dec 2010
Location: UK
Posts: 245
Rep Power: 16
mohammad is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Recent versions of Fluent have a coupled solver which is very close to the CFX solver. Did you use this, or the default SIMPLE based solvers?
I meant Fluent 6.3 [SIMPLE].
Plus, I read the same thing , as you said, in Ansys 14 "User Guide". You are right. But as it is written there still CFX is better.
mohammad is offline   Reply With Quote

Old   February 18, 2012, 12:31
Default
  #9
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,553
Blog Entries: 6
Rep Power: 54
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Well, recently I have (my friend as well) used the Fluent 13 and 14 for Mach from 0.6 to 6.5 and didn't find any problem, comparable to NPARC results in high Mach no regime. Grids used had Yplus from 1 to 8000 (different cases, e.g. for drag prediction yplus was kept at 1). Solver was density based. Previously in Fluent 6.3, we had difficutly in getting converged solution and even after 60000-80000 iteration we achieved 1e-02 residual level and now in latest release we are getting solution within 2000-5000 iteration with residual level of 1e-5.

This is due to improvements in solver, which is obvious from the above description. One improvement which is obvious is the introduction of automatic wall treatment for the k-w based model and scalable wall functions for k-epsilon based models. These improvements were introduced in CFX long ago (as Menter discovered them in 2002-2003). Now ANSYS is improving the both solvers by combining the strong points of both solvers and Fluent has improved a lot in solver technology as compared to V 6.3.

You must have also noted that ANSYS is not supporting GAMBIT and they have replaced GAMBIT with ANSYS Meshing and now GAMBIT team is working very hard on it. But they are still releasing the new versions of Fluent!!! Why?This is due to fact that both solvers have strong points. For example CFX does not support the polyhederal cells and hanging node meshes. CFX does not have the Far field boundary condition. But on the other hand ANSYS is keep on improving the turbomachinery module in CFX. Why? Why not they are improving the turbo machinery module in Fluent? You know ANSYS has introduced the Assembly meshing option for very complex geometries (cut cell) and these meshes can only run in Fluent!! Why they not improving CFX to accept these latest type of grids? The answer is very much clear both have their strong points and as well as weak sides.
AshwaniAssam likes this.

Last edited by Far; February 18, 2012 at 15:19.
Far is offline   Reply With Quote

Old   February 18, 2012, 13:32
Default
  #10
Senior Member
 
mohammad
Join Date: Dec 2010
Location: UK
Posts: 245
Rep Power: 16
mohammad is on a distinguished road
Dear Far and Glenn Horrocks,
Thank you for your comprehensive and informative answers. I am really happy that some knowledgeable guys like you are in this forum.

Regards,
marcolovatto likes this.
mohammad is offline   Reply With Quote

Reply

Tags
cfx solver

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Using Density Gradient C_R_G(c,t), Pressure Based Solver Anirudh_Deodhar Fluent UDF and Scheme Programming 1 October 25, 2013 06:43
Working directory via command line Luiz CFX 4 March 6, 2011 21:02
Pressure and density based solver JOKER FLUENT 0 February 18, 2011 10:58
The correction on pressure equation of SIMPLE algorithm in MRFSimpleFOAM solver renyun0511 OpenFOAM Running, Solving & CFD 0 November 10, 2010 02:47
Pressure based and Density based Solver Xobile Siemens 1 November 30, 2004 22:13


All times are GMT -4. The time now is 17:08.