CFX vs. FLUENT
 

This topic never stops showing up in the forum. Let me help you make it clear.

1. By CFD Code

• FLUENT : UK college > Creare (US) > Fluent (US) > Ansys
• CFX : UK Nuclear Research > AEA Technology (UK) > ASC (Canada, CFX-TASCflow) > Ansys
• STAR-CD : UK college > CD-Adapco
• FineTurbo : Brussel college (Prof. Hirsch) > NUMECA

2. By Solver Type

• Segregated : Pressure-based Method of FVM : FLUENT, STAR-CD

- Continuity, momentum and energy equations are solved sequentially.
- Pressure is later corrected by Pressure-Velocity Coupling (like SIMPLE, SIMPLEC or PISO)
- Originally for incompressible flow, but extended to compressible flow

• Coupled : Time Marching of FVM : FLUENT (RAMPANT), FineTurbo

- Conservative vector forms in time and space
- Explicit (FineTurbo, FLUENT RAMPANT) or implicit (FLUENT) solver with multigrid
- Originally for compressible flow, but extended to incompressible using pseudo-compressibility factor
- Better accuracy in highly compressible flows (maybe controversial)

3. CFX is kind of unique

• CFX is a coupled solver, but needs the pressure-velocity coupling, too. It belongs to the Pressure-based group.
• CFX is fully implicit, relatively faster than FLUENT, but requiring much storage.
• CFX is a cell-vertex code, while FLUENT a cell-centered.
• CFX has a shape function borrowed from FEM to evaluate gradients, but FLUENT uses the staggered grid concept.

4. CFX vs. FLUENT

• CFX has more friendly GUI for turbomachinery users (that was a kind of business strategy for CFX-TASCflow to survive competing with FLUENT).
• FLUENT has traditionally more users in more general applications.
• Both are now good enough !

5. My recommendations

• If you simulate combustion, multi-phase or chemically-reacting flows, I'd go with FLUENT segregated.
• If you simulate a single phase turbomachinery flow, two options are recommended : CFX or FineTurbo. In this area, they are totally different animals. Try out both in your model through a comparison with reliable test data before making a decision.
• NUMECA FineTurbo grid generation package (Autogrid) has been frequently agreed more powerful and of higher quality, but the Post still looks not easy to love.

Thanks for that.

So Fluent uses the FVM and CFX uses the FVM with Finite elements? I've heard it described that way.

I also posted on whether this has anything to do with Fluent being able to handle 3D meshes but CFX not being able to?

CFX and Fluent can both handle 3d meshes just fine.

You are probably getting confused with 2d meshes: Fluent has a pure 2D solver, but CFX does not have a 2d solver and you need to make a 1 element thick model and ignore the third dimension. This is messier to set up, much slower to solve and uses more memory. This was done simply because CFX did not want to do the development effort to make and validate a 2d solver, they thought the market was going to full 3d so a 2d solver was not worth the effort in their opinion. I have always disagreed with this logic and think this is one of CFX's greatest weaknesses.

No. Both Fluent and CFX use Finite Volume Methods to solve the equations. I.e., they are FVM-packages. However, Fluent takes the meshes as generated and stores the calculated values in the center of the cells. It is therefore called a cell-based solver. CFX does not take the meshes as generated. It creates a background mesh around the nodes (corners of the elements). Calculated values are stored in these nodes. Therefore it is called a node-based-solver.

In fact, if CFX converts a tet mesh in the background, it converts this into a polyhedra mesh. Therefore, a solution with a tet mesh in CFX is somewhat comparable to a solution with a polyhedra mesh in Fluent. Solutions with tet-meshes are uncomparable.

So, what you see is that Fluent can read almost every mesh like hex, tets, pyramids, prisms, polyhedra and Hex meshes with hanging nodes (cutcell-technology).
CFX can only handle hex, tet, pyramids, and prisms. It cannot read polyhedra and hex-meshes with hanging nodes, because CFX cannot convert them in its background process to a polyhedra mesh.

Just for clarification, ANSYS CFX never converts the original mesh into a polyhedral mesh explicitly, i.e. it discretizes the equation on each element sector around a node, and creates discrete equations around a node of the original mesh. The equations are very close to those obtained by explicitly computing the dual mesh, i.e. polyhedral mesh, but they are not identical for all situations.

Otherwise, the description is spot on.