# CFX/OF results comparison

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

 March 15, 2013, 05:43 CFX/OF results comparison #1 Member   M Join Date: Jul 2012 Posts: 33 Rep Power: 7 Sponsored Links 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

 March 15, 2013, 06:07 #2 Senior Member   Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 297 Rep Power: 15 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

March 15, 2013, 10:15
#3
Member

M
Join Date: Jul 2012
Posts: 33
Rep Power: 7
First, thank to answered so quickly,

-
Quote:
 Originally Posted by Lieven Concerning your case, "quite the same mesh" could be a possible cause.
.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) ?

-
Quote:
 Originally Posted by Lieven 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.
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)

-
Quote:
 Originally Posted by Lieven 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")
I will try that and give you some news as soon as possible !

Thanks for all

m_f

 March 16, 2013, 09:50 #4 Senior Member   Paulo Vatavuk Join Date: Mar 2009 Location: Campinas, Brasil Posts: 158 Rep Power: 10 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

 March 17, 2013, 10:05 #5 Senior Member     Daniel P. Combest Join Date: Mar 2009 Location: St. Louis, USA Posts: 612 Rep Power: 22 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 ). linnemann, wyldckat, sharonyue and 1 others like this. __________________ Dan Find me on twitter @dancombest and LinkedIn Last edited by chegdan; March 21, 2013 at 10:48.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Shawn_A CFX 16 April 12, 2016 20:49 Fugacity Autodesk Simulation CFD 1 February 24, 2012 11:48 dancfd OpenFOAM Post-Processing 3 November 14, 2011 20:11 Mohit Gupta Main CFD Forum 0 September 29, 2008 13:04 Lee Siemens 4 May 26, 2006 03:39