CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   CFX or Fluent (

Confused guy September 26, 2005 05:46

CFX or Fluent
i am intersted in cfd of turbomachinery. I am using fluent for this purpose. But i find it hard to work in gambit. could u people suggest me preprocessor for this purpose.

2ndly i am confused which software is best for turbomachinery. CFX or Fluent ?

James Date September 26, 2005 18:14

Re: CFX or Fluent
Well, all solvers are pretty similar these days but mesh generation is the key!! Have used Gambit/Gridgen/ICEM and now think ICEM is the best by far. The Hex meshing is the the best by far, although hard to learn at first if you're used to bottom up hex grid generation. The tet capabilitly is excellent although i tend not to use it if i can hex mesh a geometry. CFX is very good for the rotating frame of reference turbo machinery simulations. I've done some recent work on tidal turbines and the results seem fine with high quality meshes. Your best bet is to have a 30 trial of CFX and Fluent and see how you get on. From my past experience with Gambit (not the current release) i found it had a tendancy to crash a lot on complex CAD geometries, but this has probably been sorted out now.

zxaar September 26, 2005 21:28

Re: CFX or Fluent
there is general consensus (based on messages on cfd-online) that for turbomachinary cfx is btter than fluent. as far as gambit is concerned, if you geomtery is not too complex its very good mesher and i like it because its very easy to use. in fact i never had to read a single page from tutorial etc to learn it. but for complecated geometries, it sometimes can give you problem, specially when you stumble upon something that it does not have feature to create it.

on windows machine, i have heard that gambit crashes a lot, on my machine it hardly crashes, in fact i prefer to work on windows machine than to linux machine i have for meshing. one thing i have observed that if you are using a two button mouse then it will crash pretty easily, i use a three button mouse and i never saw it crashing (one year on and no problem).

Robin September 26, 2005 23:18

Re: CFX or Fluent
Check out TurboGrid and BladeModeler. Both from ANSYS.


Erich September 27, 2005 10:03

Re: CFX or Fluent
Hey Robin,

Do you ever use CFX-Mesh for blade sections, or do you only use turbogrid? Would you use Hexa over CFX-Mesh for blade sections or is CFX-Mesh more than adequate?



Robin September 27, 2005 12:04

Re: CFX or Fluent
Hi Erich,

I use both. CFX Mesh will produce a high quality mesh with inflation and is particularly useful if you have additional features such as cooling holes, fillets, etc. TurboGrid, on the other hand, is very fast and if you are doing design iterations, has the advantage that you can maintain the same topology from one blade to the next (thus minimizing difference due to grid resolution) and generate the meshes in batch. Hexa is also a very good tool, but requires substantially more work up front. As with TurboGrid, the advantage is that you get a hex mesh and can use the same topology for multiple design iterations. Of course, Hexa can also be applied to any other geometry you wish to hex mesh.

Bladed geometry lends itself well to hex meshes, which allow you to elongate the elements in the passage without comprimizing mesh quality, thus being more efficient on nodes. A hex element also uses less memory per node, since there are fewer connections to neighboring elements. The main drawback is that it is harder to create a quality hex mesh. All the advantages are lost if the mesh is of poor quality. Quality issues include large volume ratio's (the ratio of the volume of neighboring elements), small angles and striping of these features. TurboGrid handles these fairly automatically, whereas it is up to the user to do it in Hexa.

In terms of accuracy, there is no disadvantage to hybrid meshes from CFX Mesh. You will find that you may need more nodes, however, and the tet elements require more RAM, so the computational cost increases. If you have very small features, it is much easier with CFX Mesh to pack the additional nodes in locally and expand the mesh out to the volume size, a key advantage to unstructured grids. Although you cannot guarantee the same mesh topology from one design to the next, you can ensure that the same mesh controls are used and thus keep the grid effects in the same ballpark. CFX Mesh can update to the latest geometry, so if you are linking to your CAD or BladeModeler, remeshing is as easy as pushing a button.

Overall, I highly recommend using TurboGrid if you do a lot of turbomachinery analysis. The extra cost will quickly pay off as it is very easy to use and will speed up the analysis and your overally cycle time.

Best regards, Robin

P.S. My apologies for the name Fred appearing in my posts. Another guy borrowed my computer and I hadn't noticed the change.

Erich September 27, 2005 14:36

Re: CFX or Fluent
Hi Robin,

Thank you. I knew you would be the one to ask. Things are a little better since P-cube.

Best Regards,


Neale October 17, 2005 22:21

Re: CFX or Fluent
From a flow solver standpoint CFX is clearly the Turbo code to use. If you carefully read the Fluent documentation there are significant weaknesses in the treatment Fluent uses at MFR interfaces:

- The "mixing plane model" in Fluent (which called "Stage" in CFX) is not conservative. This is so bad bad bad...

- The "sliding mesh model" in Fluent (which is called Transient Rotor Stator in CFX) cannot not handle partial blade passage simulations with unequal pitch, so you must calculate the full 360 degrees of your stationary and rotating components. This is a massive limitation, especially froma computational resource standpoint.


Bak_Flow October 19, 2005 00:09

Re: CFX or Fluent
Hi Neale,

CFX uses the strong conservation form of the discrete equations for mass, Cartesian momentum components, energy, etc and this is also enforced at the GGI interfaces.

Although for many applications this is a nice property to have, what would be ideal for turbomachinery is strong conservation form for angular momentum.



All times are GMT -4. The time now is 00:30.