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.

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.

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.

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.

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).

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.

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?

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.

I didn't ask him about these details.



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!

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.

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.