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

Difference between ANSYS CFX and Fluent?

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

Like Tree55Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 18, 2016, 07:05
Default
  #41
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,474
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The Navier Stokes equations have momentum equations and a pressure/mass equation. But the momentum equation is only loosely coupled (in a mathematical sense) to the pressure/mass equation so you need to do some special numerical techniques to simultaneously solve them. There are several methods to do this, and they are known as pressure-velocity coupling or PV coupling. It is the fundamental method used by the CFD solver.
ghorrocks is offline   Reply With Quote

Old   October 8, 2016, 21:30
Default
  #42
AST
New Member
 
no name
Join Date: Oct 2016
Posts: 1
Rep Power: 0
AST is on a distinguished road
The Navier Stokes equations have momentum equations and a pressure/mass equation. But the momentum equation is only loosely coupled (in a mathematical sense) to the pressure/mass equation so you need to do some special numerical techniques to simultaneously solve them. There are several methods to do this, and they are known as pressure-velocity coupling or PV coupling. It is the fundamental method used by the CFD solver.
AST is offline   Reply With Quote

Old   November 5, 2016, 23:11
Default
  #43
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 8
swm is on a distinguished road
In my opinion, CFX is more robust and easier for new users than Fluent. However, it is more convenient to alter turbulent parameters and numerical parameters in fluent. In terms with the performance, fluent is more accurate with lower scheme dissipation.
swm is offline   Reply With Quote

Old   November 6, 2016, 05:43
Default
  #44
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,474
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
In terms with the performance, fluent is more accurate with lower scheme dissipation.
On what basis do you say that? In my experience CFX is more accurate with lower dissipation that fluent for most cases.

My justification is:
* CFX has second order differencing as default, fluent has first
* CFX has a coupled solver (the only solver options), the Fluent default solver is a very old technology uncoupled solver

You can configure Fluent to run in a CFX-like mode and then it will have similar dissipation to CFX. But the default Fluent setup is highly dissipative.
ghorrocks is offline   Reply With Quote

Old   November 6, 2016, 06:44
Default
  #45
Member
 
Join Date: Jan 2015
Posts: 63
Rep Power: 7
highorder_cfd is on a distinguished road
Just an observation. Actually they are developing an unified CFD solver under the name of ANSYS Flux. This is currently implemented in the product AIM. However this is still at the early stages of the development (single species and phase, compressible and incompressible, includes pressure loss and porous domains with these last ones as beta feature, no rotating zones and transient still beta feature).

Quote:
Originally Posted by ghorrocks View Post
ANSYS bought CFX, then it still had some spare cash so it bought Fluent as well. If you got the cash the easiest way to get market share is to buy it.

So ANSYS has 2 codes due to its history of buying established CFD codes. And it has not released a unified code with the best of both codes yet.
highorder_cfd is offline   Reply With Quote

Old   November 6, 2016, 09:28
Default
  #46
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 8
swm is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
On what basis do you say that? In my experience CFX is more accurate with lower dissipation that fluent for most cases.

My justification is:
* CFX has second order differencing as default, fluent has first
* CFX has a coupled solver (the only solver options), the Fluent default solver is a very old technology uncoupled solver

You can configure Fluent to run in a CFX-like mode and then it will have similar dissipation to CFX. But the default Fluent setup is highly dissipative.
1.One of my colleagues compared results of airfoils and found that the Cp distribution predicted by cfx near shock was not as sharp as that in fluent.
2. I found that CFX can always 'give' a result no matter how bad your mesh is. So, I guess it is because of relatively large numerical viscosity in cfx.
swm is offline   Reply With Quote

Old   November 6, 2016, 18:36
Default
  #47
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,474
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
1.One of my colleagues compared results of airfoils and found that the Cp distribution predicted by cfx near shock was not as sharp as that in fluent.
Was the CFX simulation correctly set up? Properly validated/verified?

CFX probably would have a hard time being as good as the Fluent density based solver for shock wave flows. Was the Fluent simulation done on the density based solver?

Quote:
2. I found that CFX can always 'give' a result no matter how bad your mesh is. So, I guess it is because of relatively large numerical viscosity in cfx.
CFX is pretty reliable for converging most of the time. This can also be due to the coupled solver allowing resolution of small coupling effects which uncoupled sovlers have problems with. So I do not agree that blaming it on higher dissipation is a good explanation in general.
ghorrocks is offline   Reply With Quote

Old   November 6, 2016, 20:13
Default
  #48
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 8
swm is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Was the CFX simulation correctly set up? Properly validated/verified?

CFX probably would have a hard time being as good as the Fluent density based solver for shock wave flows. Was the Fluent simulation done on the density based solver?
I didn't ask him about these details.



Quote:
Originally Posted by ghorrocks View Post
CFX is pretty reliable for converging most of the time. This can also be due to the coupled solver allowing resolution of small coupling effects which uncoupled sovlers have problems with. So I do not agree that blaming it on higher dissipation is a good explanation in general.
Could you please explain your 'This can also be due to the coupled solver allowing resolution of small coupling effects which uncoupled sovlers have problems with' for me? It's a general saying that is hard to understand. BTW, my colleagues simulated a lot of airplane projects with CFX successfully which proves that robustness of this software is awesome!
swm is offline   Reply With Quote

Old   November 6, 2016, 20:23
Default
  #49
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,474
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Most CFD solvers including Fluent are based on a SIMPLE algorithm (or its derivatives, such as SIMPLEC, PISO). That solves the equations as a single matrix per variable. So you solve the linearised U momentum, then V, then W, then you do a pressure correction step, and you iterate over this whole process to obtain convergence. As it is done sequentially it can take many iterations for the non-linear effects to work its way through the other equations.

CFX uses a coupled solver which solves the UVW moment and pressure equation in a single matrix. This means that a solution to the entire linearised equation set is obtained in one go. This means you do not need to iterate as much to get the weaker coupling effects transmitted to all equations. But the down side of this is the solver requires more memory as the matrix for the linear solver is much larger.

As the coupled solver handles weak coupling better, if effects contained in weak coupling are important then a coupled solver would be expected to converge better than an uncoupled solver.
swm and liucheng8602 like this.
ghorrocks is offline   Reply With Quote

Old   November 6, 2016, 21:24
Default
  #50
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 8
swm is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Most CFD solvers including Fluent are based on a SIMPLE algorithm (or its derivatives, such as SIMPLEC, PISO). That solves the equations as a single matrix per variable. So you solve the linearised U momentum, then V, then W, then you do a pressure correction step, and you iterate over this whole process to obtain convergence. As it is done sequentially it can take many iterations for the non-linear effects to work its way through the other equations.

CFX uses a coupled solver which solves the UVW moment and pressure equation in a single matrix. This means that a solution to the entire linearised equation set is obtained in one go. This means you do not need to iterate as much to get the weaker coupling effects transmitted to all equations. But the down side of this is the solver requires more memory as the matrix for the linear solver is much larger.

As the coupled solver handles weak coupling better, if effects contained in weak coupling are important then a coupled solver would be expected to converge better than an uncoupled solver.
Thank you for brief introduction about the basic concepts relating with couple solver. According to this, classical FV methods (reconstruction, riemann solver and time marching) belong to the coupled ones, right? But I have not noticed that there is an option to change Riemann solver types in CFX.
swm is offline   Reply With Quote

Old   November 6, 2016, 22:14
Default
  #51
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,474
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I am not familiar with the reconstruction approach. I know the godunov scheme has been effectively superseded by more schemes like SIMPLE and the coupled solver for general CFD but I am not familiar enough with the Godunov scheme to say exactly why.

The time marching scheme is an explicit scheme which has no linear equation set to solve, rather the PV coupling is done as part of the algebraic calculation of the next time step. While the PV coupling is inherent in these sort of solvers the extremely tight time step restriction of explicit solvers means that these approaches are only useful in flows like shock wave flows where the CFL=1 time step size is appropriate. For general CFD it is restricted to such tiny time steps that simulations take forever - and they are problematic to get to steady state simulations as well.

In CFX the coupled solver is hard-coded in there. So you don't get any option about which solver to choose. But you also do not loose simulation time with the overhead of choosing a solver type.
swm likes this.
ghorrocks is offline   Reply With Quote

Old   November 6, 2016, 22:18
Default
  #52
swm
Member
 
swm's Avatar
 
Join Date: Dec 2013
Posts: 47
Rep Power: 8
swm is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
I am not familiar with the reconstruction approach. I know the godunov scheme has been effectively superseded by more schemes like SIMPLE and the coupled solver for general CFD but I am not familiar enough with the Godunov scheme to say exactly why.

The time marching scheme is an explicit scheme which has no linear equation set to solve, rather the PV coupling is done as part of the algebraic calculation of the next time step. While the PV coupling is inherent in these sort of solvers the extremely tight time step restriction of explicit solvers means that these approaches are only useful in flows like shock wave flows where the CFL=1 time step size is appropriate. For general CFD it is restricted to such tiny time steps that simulations take forever - and they are problematic to get to steady state simulations as well.

In CFX the coupled solver is hard-coded in there. So you don't get any option about which solver to choose. But you also do not loose simulation time with the overhead of choosing a solver type.
Thanks a lot.
swm is offline   Reply With Quote

Reply

Tags
cfx & fluent

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


LinkBacks (?)
LinkBack to this Thread: https://www.cfd-online.com/Forums/cfx/110640-difference-between-ansys-cfx-fluent.html
Posted By For Type Date
Ingenieurthread [19] - mods.de - Forum This thread Refback November 22, 2014 07:57

Similar Threads
Thread Thread Starter Forum Replies Last Post
difference between CFX and fluent rashmi FLUENT 17 February 3, 2020 08:29
Difference of result betn Fluent & CFX simulation for S2S radiation njundale Fluent UDF and Scheme Programming 0 November 6, 2012 01:35
Difference between Fluent and CFX safikhani_hamed FLUENT 1 October 1, 2012 05:16
Difference between CFX and FLUENT TypeSpeed CFX 3 January 6, 2010 16:55
Converting ANSYS CFX files to Fluent files Martin S. Rasmussen FLUENT 3 January 30, 2007 16:08


All times are GMT -4. The time now is 01:35.