
[Sponsors] 
July 18, 2016, 06:05 

#41 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
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 pressurevelocity coupling or PV coupling. It is the fundamental method used by the CFD solver.


October 8, 2016, 20:30 

#42 
New Member
no name
Join Date: Oct 2016
Posts: 1
Rep Power: 0 
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 pressurevelocity coupling or PV coupling. It is the fundamental method used by the CFD solver.


November 5, 2016, 22:11 

#43 
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 10 
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.


November 6, 2016, 04:43 

#44  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
Quote:
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 CFXlike mode and then it will have similar dissipation to CFX. But the default Fluent setup is highly dissipative. 

November 6, 2016, 05:44 

#45  
Member
Join Date: Jan 2015
Posts: 63
Rep Power: 9 
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:


November 6, 2016, 08:28 

#46  
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 10 
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. 

November 6, 2016, 17:36 

#47  
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
Quote:
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:


November 6, 2016, 19:13 

#48  
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 10 
Quote:
Quote:


November 6, 2016, 19:23 

#49 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
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 nonlinear 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. 

November 6, 2016, 20:24 

#50  
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 10 
Quote:


November 6, 2016, 21:14 

#51 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134 
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 hardcoded 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. 

November 6, 2016, 21:18 

#52  
Member
Join Date: Dec 2013
Posts: 47
Rep Power: 10 
Quote:


Tags 
cfx & fluent 
Thread Tools  Search this Thread 
Display Modes  


LinkBacks (?)
LinkBack to this Thread: https://www.cfdonline.com/Forums/cfx/110640differencebetweenansyscfxfluent.html


Posted By  For  Type  Date  
Ingenieurthread [19]  mods.de  Forum  This thread  Refback  November 22, 2014 06:57 
Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
difference between CFX and fluent  rashmi  FLUENT  17  February 3, 2020 07:29 
Difference of result betn Fluent & CFX simulation for S2S radiation  njundale  Fluent UDF and Scheme Programming  0  November 6, 2012 00:35 
Difference between Fluent and CFX  safikhani_hamed  FLUENT  1  October 1, 2012 04:16 
Difference between CFX and FLUENT  TypeSpeed  CFX  3  January 6, 2010 15:55 
Converting ANSYS CFX files to Fluent files  Martin S. Rasmussen  FLUENT  3  January 30, 2007 15:08 