CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Difference between ANSYS CFX and Fluent?

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree38Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 17, 2012, 03:17
Question Difference between ANSYS CFX and Fluent?
  #1
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
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 !

Last edited by keerthivasan; December 19, 2012 at 09:05.
keerthivasan is offline   Reply With Quote

Old   December 17, 2012, 05:40
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 17, 2012, 07:39
Default
  #3
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
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)?
keerthivasan is offline   Reply With Quote

Old   December 17, 2012, 08:20
Default
  #4
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
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.
amod_kumar and keerthivasan like this.
cdegroot is offline   Reply With Quote

Old   December 17, 2012, 09:28
Default
  #5
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
Thanks Chris DeGroot for taking time to answer my question.

I was bale to understand the most of your answer, except
Quote:
"....it can solve the volume fractions coupled. And the general grid interfaces are very useful."
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.
keerthivasan is offline   Reply With Quote

Old   December 17, 2012, 10:18
Default
  #6
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
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.
cdegroot is offline   Reply With Quote

Old   December 18, 2012, 20:48
Default
  #7
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
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.
keerthivasan and 6863523 like this.
evcelica is offline   Reply With Quote

Old   December 18, 2012, 20:53
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
keerthivasan likes this.
ghorrocks is offline   Reply With Quote

Old   December 19, 2012, 00:31
Default
  #9
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
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.
Mfaizan likes this.
cdegroot is offline   Reply With Quote

Old   December 19, 2012, 02:20
Default
  #10
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
Right, I don't mind doing the planar 2D models either, but trying to do an axisymmetric "wedge" just sucks.
evcelica is offline   Reply With Quote

Old   December 19, 2012, 03:22
Default
  #11
Member
 
Join Date: Nov 2011
Location: Czech Republic
Posts: 95
Rep Power: 5
Sixkillers is on a distinguished road
Quote:
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).
Yes it can



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).

Sixkillers is offline   Reply With Quote

Old   December 19, 2012, 07:01
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.

Quote:
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.
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.
ghorrocks is offline   Reply With Quote

Old   December 19, 2012, 07:54
Default
  #13
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
Quote:
Originally Posted by Sixkillers View Post
On the other hand due to this approach the CFX can't handle exotic type of meshes (e.g. cut-cell , polyhedral).
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.
Sixkillers likes this.
brunoc is offline   Reply With Quote

Old   December 19, 2012, 09:08
Default
  #14
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
Quote:
Originally Posted by evcelica View Post
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.

Thanks for the insight Eric. I was looking for the difference like these, which make some sense to beginners like me.
vinayender and 6863523 like this.
keerthivasan is offline   Reply With Quote

Old   December 19, 2012, 09:10
Default
  #15
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
Quote:
Originally Posted by Sixkillers View Post
Yes it can



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).

Thanks a lot for including the diagrams. Otherwise it would have been a mystery to me.
vinayender and 6863523 like this.
keerthivasan is offline   Reply With Quote

Old   December 19, 2012, 09:24
Default
  #16
New Member
 
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 4
keerthivasan is on a distinguished road
Hi Chris DeGroot,

Quote:
By coupled (more accurately I should say "fully-coupled"), I mean they are solved in the same matrix system simultaneously.
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.
6863523 likes this.
keerthivasan is offline   Reply With Quote

Old   December 19, 2012, 09:26
Default
  #17
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 236
Rep Power: 12
brunoc is on a distinguished road
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.
brunoc is offline   Reply With Quote

Old   December 19, 2012, 12:22
Default
  #18
Senior Member
 
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 387
Rep Power: 6
cdegroot is on a distinguished road
Quote:
Originally Posted by Sixkillers View Post
Yes it can


I stand corrected!
cdegroot is offline   Reply With Quote

Old   March 23, 2014, 20:54
Default Cfx or fluent???
  #19
New Member
 
Ndong-Mefane Stephane Boris
Join Date: Nov 2013
Location: Kawasaki (JAPAN)
Posts: 14
Rep Power: 3
S_teph_2000 is on a distinguished road
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 ?
S_teph_2000 is offline   Reply With Quote

Old   March 23, 2014, 21:05
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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 .
ghorrocks is offline   Reply With Quote

Reply

Tags
cfx & fluent

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


LinkBacks (?)
LinkBack to this Thread: http://www.cfd-online.com/Forums/cfx/110640-difference-between-ansys-cfx-fluent.html
Posted By For Type Date
Ingenieurthread [19] - mods.de - Forum This thread Refback November 22, 2014 07:57

Similar Threads
Thread Thread Starter Forum Replies Last Post
difference between CFX and fluent rashmi FLUENT 8 March 5, 2014 23:50
Difference of result betn Fluent & CFX simulation for S2S radiation njundale Fluent UDF and Scheme Programming 0 November 6, 2012 01:35
Difference between Fluent and CFX safikhani_hamed FLUENT 1 October 1, 2012 04:16
Difference between CFX and FLUENT TypeSpeed CFX 3 January 6, 2010 16:55
Converting ANSYS CFX files to Fluent files Martin S. Rasmussen FLUENT 3 January 30, 2007 16:08


All times are GMT -4. The time now is 03:35.