CFX/OF results comparison
 

Hello everyone,

I am realizing a external aerodynamic study of a building with OpenFOAM and CFX at the same time.
I use :
- Quite the same mesh
- Same material definition
- Same turbulence model
- Same order of discretization
- I use simpleFOAM solver with OpenFOAM

But i have some problems with the results of OpenFOAM.

With CFX, convergence time is quick, around 300 iterations.
With OpenFOAM, the convergence time (all residual values less than 10^-5) is longer. Moreoever, even if the residuals are very low, when I calculate the force in the building with "forces" tools of OF, the value always decrease very slowly.

So, with CFX, the final value is fixed : Fx = 1.91e+07 N, and don't move after, even if i continue the calculation.
with OpenFOAM : The value arrive around Fx = 1.84e+07 N in 2000 iterations, and continue to always decrease very very slowly after. I stopped around Fx = 1.2e+07 N.

I don't understand how it could be possible.
Have you got some ideas ?

Don't hesitate to ask me some questions if I am not clear
Regards,

m_f

Dear m_f,

In principle there should not be a difference but heard/read it already a few times that it is often observed.
* Concerning your case, "quite the same mesh" could be a possible cause.
Did you perform a grid sensitivity study (see how Fx changes with increasing grid resolution)? If not, I would start with that.
* Regarding the convergence time. It is easy to compare residuals that are given by CFX and OF but make sure they are defined in the same way. Else you would be comparing apples and oranges.
* To speed up the simulation, you can try to switch to piso or pimpleFoam and use localEuler as scheme for the time derivative (the time derivative is then used in a sense of "false time stepping"). It wouldn't surprise me if CFX does something similar.

Cheers,

L

First, thank to answered so quickly,

- .When i wrote quite the same that's mean the size of the same is quite the same, and i tried to design the refinement zone in the same way (same cell refinement zone, with the same cell size).
Do you know a way to export the mesh OpenFOAM to CFX (Ansys Workbench Student Edition) ?

- I totally agree. I compared yet, the evolution of two one are quite "normal", just OF seems slower than CFX (I would like to plot them but I use the blueCAPE windows version, so I can't use gnuplot to plot them. . . I am wrong I no :/ (Linux computer stayed in my country)

- I will try that and give you some news as soon as possible !

Thanks for all

m_f

Hi m_f,
I think it would be interesting to compare the flow in both computations. I suggest that you draw the streamlines at a chosen height above the ground. It is possible that the recirculation region is different in the two simulations. I've seen some CFX results that have an unsymmetrical recirculation, in spite of the building being symmetrical and the wind incidence being 90 degrees in relation to the walls. On the other hand, to converge a symmetrical simulation might be difficult, if the flow has a natural tendency to become unsymmetrical, this tends to destabilize the symmetrical the flow.
Best Regards,
Paulo

on the speed of convergence:

since it wasn't already mentioned (but you probably know already), CFX uses coupled solvers (i.e. pressure and velocity are coupled through the continuity equation and solved in a single matrix) while simpleFoam is a segregated solver (i.e. Ux, Uy, Uz, and p are solved separately and coupled explicitly between eachother). Coupled solvers converge faster i.e. in less iterations (in general :)).