Question about meshing / solution scheme of CFX
I have some questions about the functionalities of CFX 5.6/5.7:
1) Is it still able to create the rectangular grid used in the finite volume method? 2) Is it possible to use relaxation method (for the individual variables) to control the convergent rate? 3) Is it possible to choose or define the solution scheme such as SIMPLE, SIMPLEC, QUICK etc. I have defined a domain and solution method in my study. It is basically the convention finite volume method. I have to show that the software being used actually use these methods. From the CFX website, I've noticed that most of the sample meshes are not rectangular and more resemble the finite element mesh. In that case, there will be serious problems (or even impossible) in applying the finite volume method. If anyone has experience about this area, please give me some advices. 
Re: Question about meshing / solution scheme of CF
Of course CFX5 uses finite volume method, just slightly other formulation. Generaly CFX5 uses unstructured aproach and coupled scheme (not SIMPLE...).

Re: Question about meshing / solution scheme of CF
Hi Coriolius,
SIMPLE and SIMPLEC are segregated solution methods, whereas CFX5 uses a coupled solution method. QUICK is an advection scheme, which is available in CFX5 as an expert option, but not terribly useful. You can use whatever elements you like. The formulation is a hybrid between finite element method and finite volume, commmonly referred to as an Element Based Finite Volume Method. For a description of the numerics, refer to the CFX5 theory. For a more thorough review, you can download the CFXTASCflow theory documentation from the CFX Community site. CFX5 and CFXTASCflow share very similar numerics, so much of the theory applies. Regards, Robin 
Re: Question about meshing / solution scheme of CF
Thanks for the info. If I am going to employ the classic SIMPLEtype solution scheme and working on a rectangular mesh only, CFX may be too advance for this purpose.
Anyone can suggest a program (an outdated one is also acceptable) which can do the job? 
Re: Question about meshing / solution scheme of CF
Hi Coriolius,
CFX4 uses a SIMPLE based solver, and works on simple rectangular grids. It might be suitable for your purposes. Glenn 
Re: Question about meshing / solution scheme of CF
Hi Coriolius
In addition to what Glenn said in his Reply, you might consider the ff too: :>1) Is it still able to create the rectangular grid used in the finite volume method? Yes! On the other hand are you using CFXBuild to generate the grid or what? From your question, I presumed that you're using that, then you have to be careful since CFXBuild 5 does not generate structure grid by default. You can change it so that you get the structure grid for the solver. CFX5 accepts both structure and nonstructure grids. >>2) Is it possible to use relaxation method (for the individual variables) to control the convergent rate? I'm sure about this but there is a feature in the CFXpre environment where you specify the convergeance rate. You can also have a user define routine which CFX5 has capability of accepting it. This is somehow difficult though!!!:) >>3) Is it possible to choose or define the solution scheme such as SIMPLE, SIMPLEC, QUICK etc. Yes!! It is already embeded in the solver. is SIMPLE. Remember CFX uses FV but based on FE approached. PS: Refer to the USER MANUAL for full documentations including the theories employed in CFX5. It is available online by clicking HELP on your CFX environment. All the best!!! 
Re: Question about meshing / solution scheme of CF
Thank for the comment and answer

Re: Question about meshing / solution scheme of CF
Thanks for the valuable advices.

Re: Question about meshing / solution scheme of CF
Hi KKA,
Your answer to point 3 is incorrect. You wrote: ">>3) Is it possible to choose or define the solution scheme such as SIMPLE, SIMPLEC, QUICK etc. Yes!! It is already embeded in the solver. is SIMPLE. Remember CFX uses FV but based on FE approached. " CFX5 does not use the SIMPLE algorithm. SIMPLE is an uncoupled solution procedure where each variable is solved in turn. As robin said in his posting, CFX5 uses a unique coupled solution technique where the 3 velocity and pressure equations are solved simultaneously (hence a "coupled" solver). You will find that the CFX solver solves almost all CFD simulations in far less iterations than an uncoupled solver. This is due to the tighter coupling between the equations. Additionally, the relaxation factors available in CFX5 do not work the same as for the SIMPLE algorithm, however they will have similar effects, that is changing the solver speed to solver stability balance. When using SIMPLE CFD solvers you often have to tweak the under relaxation factors to get convergence. CFX5's coupled solver is far more robust and rarely requires these factors to be changed. The relaxation factors can be easily changed in CFX5 with expert parameters. Regards, Glenn 
All times are GMT 4. The time now is 21:26. 