[mohammad]

Dear all,
I want to know some information about CFX11 software. Is it CFX solver a Pressure-based,a Density_based or a Combined solver?

Please also do me a favor and kindly give me a reference for your reply this question.

Regards,

[ghorrocks]

Pressure based, reference: The CFX documentation.

ps: I do not know what a "combined solver" is, in terms of the p-v coupling.

[Far]

coupled pressure based, finite element finite volume

[mohammad]

Originally Posted by ghorrocks

Pressure based, reference: The CFX documentation.

ps: I do not know what a "combined solver" is, in terms of the p-v coupling.

Originally Posted by Far

Far: coupled pressure based, finite element finite volume

Dear Far, Dear Glenn Horrocks

According to my experience,
1-FLUNET has sensitivity problem to aspect ratio. Does this coupling solves that problem in CFX?
2-Some other CFD codes (e.g. ONERA project) need some "Low Mach Preconditioning " for low speed flows to solve the error resulting from compressiblity problem in N-S. Does the above coupling in CFX help for this matter?
3- Deos CFX considers incompressible flow when using "subsonic" option for inlet velocity?

Regards,

[ghorrocks]

1) All solvers have degraded performance on high aspect ratio elements. I have heard rumours that Fluent is especially suseptible to this, I have no idea. I suspect CFX is better than Fluent here but that is only a guess.
2) CFX is a pressure based solver which needs no special correction at low Mach number. It is the density based solver which need help at low Mach number as there is not sufficient density variation to be resolved adequately.
3) CFX uses incompressible flow when you set it to constant density fluid and compressible flow when you select a compressible fluid. The subsonic inlet option is only available when you have selected a compressible flow option.

[mohammad]

Originally Posted by ghorrocks

1) All solvers have degraded performance on high aspect ratio elements. I have heard rumours that Fluent is especially suseptible to this, I have no idea. I suspect CFX is better than Fluent here but that is only a guess.

Dear Glenn Horrocks;
I have some experiences about this....this is true. I solved several 2-D and 3D models with different aspect ratios in both CFX and Fluent.
Fluent is more sensitive and even this matter causes divergences or very inaccurate results.

[ghorrocks]

Recent versions of Fluent have a coupled solver which is very close to the CFX solver. Did you use this, or the default SIMPLE based solvers?

[mohammad]

Originally Posted by ghorrocks

Recent versions of Fluent have a coupled solver which is very close to the CFX solver. Did you use this, or the default SIMPLE based solvers?

I meant Fluent 6.3 [SIMPLE].
Plus, I read the same thing , as you said, in Ansys 14 "User Guide". You are right. But as it is written there still CFX is better.

[Far]

Well, recently I have (my friend as well) used the Fluent 13 and 14 for Mach from 0.6 to 6.5 and didn't find any problem, comparable to NPARC results in high Mach no regime. Grids used had Yplus from 1 to 8000 (different cases, e.g. for drag prediction yplus was kept at 1). Solver was density based. Previously in Fluent 6.3, we had difficutly in getting converged solution and even after 60000-80000 iteration we achieved 1e-02 residual level and now in latest release we are getting solution within 2000-5000 iteration with residual level of 1e-5.

This is due to improvements in solver, which is obvious from the above description. One improvement which is obvious is the introduction of automatic wall treatment for the k-w based model and scalable wall functions for k-epsilon based models. These improvements were introduced in CFX long ago (as Menter discovered them in 2002-2003). Now ANSYS is improving the both solvers by combining the strong points of both solvers and Fluent has improved a lot in solver technology as compared to V 6.3.

You must have also noted that ANSYS is not supporting GAMBIT and they have replaced GAMBIT with ANSYS Meshing and now GAMBIT team is working very hard on it. But they are still releasing the new versions of Fluent!!! Why?This is due to fact that both solvers have strong points. For example CFX does not support the polyhederal cells and hanging node meshes. CFX does not have the Far field boundary condition. But on the other hand ANSYS is keep on improving the turbomachinery module in CFX. Why? Why not they are improving the turbo machinery module in Fluent? You know ANSYS has introduced the Assembly meshing option for very complex geometries (cut cell) and these meshes can only run in Fluent!! Why they not improving CFX to accept these latest type of grids? The answer is very much clear both have their strong points and as well as weak sides.

[mohammad]

Dear Far and Glenn Horrocks,
Thank you for your comprehensive and informative answers. I am really happy that some knowledgeable guys like you are in this forum.

Regards,