Difference between ANSYS CFX and Fluent?
 

Hi all.


I came to have a look at ANSYS CFX and Fluent. I think, both are for fluid flow modelling and analysis.

If that is so, why do we have 2 different packages from the same company?

If not, it would be very kind of you to correct my understanding.

Thanks in advance !

ANSYS bought CFX, then it still had some spare cash so it bought Fluent as well. If you got the cash the easiest way to get market share is to buy it.

So ANSYS has 2 codes due to its history of buying established CFD codes. And it has not released a unified code with the best of both codes yet.

HI ghorrocks.

Thanks for the insight.

But could you (or anyone else) say what difference do they exhibit from an end user perspective (assuming the end user is not an expert)?

In my opinion, CFX is more user friendly, although Fluent users tend to debate that :)

Fluent uses a classical finite volume method and has many options for PV coupling (segregated and coupled). CFX uses the control volume finite element method is only a coupled solver. They have similar models implemented and probably similar accuracy overall. I've heard Fluent is a bit faster on average.

CFX is particularly good for turbomachinery and stiff multiphase problems since it can solve the volume fractions coupled. And the general grid interfaces are very useful.

Thanks Chris DeGroot for taking time to answer my question.

I was bale to understand the most of your answer, except
Doubts:
1. What do you mean by coupling (I am new to CFD :)) & what is the significance of the capability to solve coupled volume fractions ?

2. In what perspective is the grid interface useful ?

Thanks.

By coupled (more accurately I should say "fully-coupled"), I mean they are solved in the same matrix system simultaneously. The other option is called "segregated", meaning you solve one thing and then the other and iterate back and forth to convergence. For velocity and pressure an example of a segregated method is SIMPLE, where you solve pressure and velocity in separate steps and have some method for adjusting in between to conserve mass. A fully-coupled method solves for velocity and pressure in a single step.

The advantage of fully-coupled method is that it will generally converge in fewer iterations, although each iteration will take longer. For problems that don't like to converge it can be helpful to use a fully-coupled method since it is less likely to blow up. Since multiphase problems are notoriously difficult to converge it is helpful that CFX can solve the volume fractions coupled (I don't think Fluent has this; could be wrong though).

The general grid interface (GGI) allows you to intersect non-matching grids. This is useful if you have a bunch of parts meshed separately and you want to combine them. One reason you might have different parts (or domains as it would be called in CFX) is that you can apply different physics to each domain. This is useful for turbomachinery which will have both rotating and stationary parts. CFX can take care of multiple frames of reference easily. You might also have a situation where you want a fluid domain and a porous domain, which GGI will take care of as well.

The difference that bothers me the most is CFX is only a 3D solver, whereas Fluent has 2D and axisymmetric solvers. If I would have known this before I started learning CFD I would have chosen Fluent for sure.

Agreed, it is the most glaring missing feature in CFX. When I moaned about it to the developers a while back they replied to generate a 2D version would be a complete rewrite of the solver code, and it was not worth it given you can do a pseudo-2D with the current solver by modelling a thin wedge. A dissappointing response, and I am sure it is loosing them sales.

Yeah, I suppose that could be a downside. I have never minded just running a single layer in the third dimension when I need to solve a 2D problem, but I guess I'm just used to it. Before getting involved with CFX I used my own code which worked the same way. As a CFD coder I can attest to the fact it would be a real pain to create a 2D code from a 3D one.

Right, I don't mind doing the planar 2D models either, but trying to do an axisymmetric "wedge" just sucks.

Yes it can :)

http://i.imgur.com/ZgVrW.png

Moreover CFX is vertex-centered solver, which means that every variable is stored in a mesh vertex (node) instead of a cell centroid (Fluent's technique). Therefore the CFX should be able to obtain the "same" results as Fluent on a coarser grid. On the other hand due to this approach the CFX can't handle exotic type of meshes (e.g. cut-cell , polyhedral).

http://i.imgur.com/eM5qT.png

My main problem with the lack of a true 2D solver is that the solver runs an order of magnitude slower than it should. That is, a true 2D solver would run about 10 times faster than a 3D extruded 1 deep mesh. (That 10x speed up is just a guess, but it would be something like that.)

It is far easier to achieve grid independance with 2D models, and 2D models are really good for optimisation and parameter sweeps. So it is a major bummer they run far slower than they have to.

Sure, but ANSYS has dozens (hundreds?) of programmers all adding features to the software. ANSYS has decided that the new features they are adding elsewhere in the software is of more value to customers (ie sales) than developing a 2D model. I find this quite amazing - 90% of new features added in the last few releases I will never use, but if CFX had a 2D model I would use it frequently. A real 2D model would be really valuable to me. It just does not make sense to me.

Not entirely true. You're right that it can't handle cut-cell meshes, but if you look at how CFX works with the mesh and how its control volumes are created, I think it's safe to assume that every mesh is a polyhedral mesh in CFX.

Thanks for the insight Eric. I was looking for the difference like these, which make some sense to beginners like me. :)

Thanks a lot for including the diagrams. Otherwise it would have been a mystery to me.

Hi Chris DeGroot,

This is an awesome insight for me. In my classes, I remember my Professor talking about the coupling phenomenon. But all I could remember was coupling means combining different entities

But the fact that coupling means solving the entities in the same matrix system simultaneously is the one which I would like to remember (I used to sleep in few CFD classes. May be, I missed this, there) for the rest of my time. .

Also, the explanation given for CGI is easy to understand.

Thanks DeGroot & all others, for speaking in a language that a beginner could understand.

As already pointed by someone else, please notice that both CFX and FLUENT now support that. It is not the default option in neither of them, though.

I stand corrected!

Cfx or fluent???
 

Hello,

I just attended a seminar on ANSYS 15.0 release, just like the one I attended last year for ANSYS 14.5. I don't know if it's only me, but I have the strong feeling that little by little, CFX is left behind. every year, Fluent gets new capabilities, while CFX only gets a few updates here and there. As a CFX user it is really frustrating, especially when you're not doing much turbomachinery analysis... Is there still something, a good thing that is exclusive to CFX except the turbo machinery friendly part? because even if that's the case, I have the feeling it won't last.
Any thoughts ?

My guess is development is focussed on reinforcing CFX's strengths in turbomachinery, multiphase and that sort of thing. I agree that there are few new features out of that area, and CFX's new features look very thin compared to Fluent's new features.

A reasonable number of the new features in Fluent is porting existing features in CFX to Fluent. Also when ANSYS bought Fluent remember it came with many more developers than the CFX purchase did - so the Fluent development should be quicker.

I had a discussion with an ANSYS senior developer in 2009 where I vividly recall him stating that if ANSYS has not released a unified CFD code within 5 years they have failed. They have 8 months left and the signs are not looking good :(.

I know exactly what you mean, and I feel the same way sitting through the ANSYS "Fluid Dynamics Update" Webinars, it seems all they talk about is FLUENT, and CFX hardly gets mentioned.
I also heard of the Unified code about a year ago, and was kind of expecting it for the 15.0 release, but nothing yet.

From what I heard a couple of years ago, a preview/first version should have been released with R15, but as we know, it wasn't.

R16, maybe? It will still be (kind of) within your 5 year range, Glenn.

Many years ago I heard v14 would have a unified solver, then it became v15, then v16, and so on... apparently a working name was (is?) FLUX (FLUent+cfX) :)

But I wonder if we will ever see it.

Got an e-mail from an ANSYS representative today. He's saying that a beta of a CFX/FLUENT unified code MIGHT BE available with the release of 16.0...They have to keep the dream alive right?!:D

Stephane

I've heard that ANSYS is working on unified CFD code now, but it won't appear even in 16 release. Also I heard that head of CFD line is fluent-guy, therefore fluent gets more attention.

I'd also like to see Ansys Meshing and ICEM merge.

I'd love the ease of use of Meshing, combined with the power of ICEM.

I know you can do something similar by going into meshing, create a new method and select "External ICEM solver" or something along those lines. However in my experience it's quite buggy. I want one unified meshing program.

I think that one of the differences are chemical reactions (combustion, etc.) which can be solved in the FLUENT solver.

CFX can model chemical reactions. I have not done a detailed comparison of reactions both of them can solve, but I suspect they can both handle most reactions you are likely to come across.

Seems like they're going to fail.

since there are even for Ansys v16 two completely independent "What's new guides" for fluent and cfx,
the "united version" of both to Ansys CFD seems to be in the far future...
or will it never happen??

find by google:

cfx:
http://dl.ptecgroup.ir/virtual_educa..._Tools_R16.pdf

fluent:
http://dl.ptecgroup.ir/virtual_educa...Fluent_R16.pdf

Those exist for every software in the ANSYS portfolio. There is also one for Polyflow (another ANSYS CFD tool), and different ones for ANSYS Mechanical and ANSYS APDL (former ANSYS Classical), even though both are based on the same solver.

BTW, even if/when a combined tool is announced, they can't just discontinue CFX and/or FLUENT, since a LOT of customers depend on them, many of which have custom tools built around those software.

You should expect CFX and FLUENT to keep going (and being supported/enhanced) for many years, even if this new thing is coming.

yes exactly -this is the point.
When starting to build some new "software environment/addons" today -which tool to choose if both would meet the requirements?
When educating people in cfd software usage which one to use?
etc. ...
Announcing something like a rough roadmap/timeline for this topic would be helpful...

Regarding building tools, my guess is that talking to ANSYS would be the best choice.

But on education, any CFD tool should do. If the person that is learning understands what the software is doing behind the curtains (equations being solved, what the models do, what the solver settings mean) they will be able to use any CFD application available.

Beginning of the end for CFX???
 

Have you seen the Ansys Customer Portal lately. In the "Online Documentation" for Ansys 16, in the Fluid "Dynamic" Section there is no more "CFX" section; only "Fluent" and "CFD-Post"...Is it just an omission? did they really merge both applications???? the suspense is unbearable!!!! :eek:

Edit:

Ok, nothing to get excited about. I just checked the "Product variable Table" for ansys 16, and nothing is changed: same old licenses, same old CFX on one side and Fluent on the other...

very useful comment .special tnx to Chris DeGroot

Hi
 

I am simulating mixing of two fluids ( both of them are water with identical physical properties) in a 3D T-shaped micromixer. which software do you recommend for this simulation (CFX or Fluent)?

Best regard

hi
 

I am simulating mixing of two fluids ( both of them are water with identical physical properties) in a 3D T-shaped micromixer. which software do you recommend for this simulation (CFX or Fluent)?

Best regard

Which ever one you are most familiar with. Both software can do this sort of simulation, so choose the one you prefer to use.

The most important thing is to use the software correctly and validate and verify thoroughly. Which software you use is of secondary importance.

I'm a newbie to CFD. May I ask what is PV coupling? Thanks!