|
[Sponsors] |
December 17, 2012, 03:17 |
Difference between ANSYS CFX and Fluent?
|
#1 |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
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. |
|
December 17, 2012, 05:40 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144 |
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. |
|
December 17, 2012, 07:39 |
|
#3 |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
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)? |
|
December 17, 2012, 08:20 |
|
#4 |
Senior Member
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 414
Rep Power: 18 |
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. |
|
December 17, 2012, 09:28 |
|
#5 | |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
Thanks Chris DeGroot for taking time to answer my question.
I was bale to understand the most of your answer, except Quote:
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. |
||
December 17, 2012, 10:18 |
|
#6 |
Senior Member
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 414
Rep Power: 18 |
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. |
|
December 18, 2012, 20:48 |
|
#7 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,188
Rep Power: 23 |
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.
|
|
December 18, 2012, 20:53 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144 |
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.
|
|
December 19, 2012, 00:31 |
|
#9 |
Senior Member
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 414
Rep Power: 18 |
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.
|
|
December 19, 2012, 02:20 |
|
#10 |
Senior Member
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 1,188
Rep Power: 23 |
Right, I don't mind doing the planar 2D models either, but trying to do an axisymmetric "wedge" just sucks.
|
|
December 19, 2012, 03:22 |
|
#11 | |
Member
Join Date: Nov 2011
Location: Czech Republic
Posts: 97
Rep Power: 15 |
Quote:
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). |
||
December 19, 2012, 07:01 |
|
#12 | |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144 |
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:
|
||
December 19, 2012, 07:54 |
|
#13 |
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 277
Rep Power: 21 |
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.
|
|
December 19, 2012, 09:08 |
|
#14 | |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
Quote:
Thanks for the insight Eric. I was looking for the difference like these, which make some sense to beginners like me. |
||
December 19, 2012, 09:10 |
|
#15 | |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
Quote:
|
||
December 19, 2012, 09:24 |
|
#16 | |
New Member
Keerthivasan R
Join Date: Dec 2012
Posts: 12
Rep Power: 14 |
Hi Chris DeGroot,
Quote:
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. |
||
December 19, 2012, 09:26 |
|
#17 |
Senior Member
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 277
Rep Power: 21 |
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.
|
|
December 19, 2012, 12:22 |
|
#18 |
Senior Member
Chris DeGroot
Join Date: Nov 2011
Location: Canada
Posts: 414
Rep Power: 18 |
||
March 23, 2014, 20:54 |
Cfx or fluent???
|
#19 |
Member
Ndong-Mefane Stephane Boris
Join Date: Nov 2013
Location: Kawasaki (JAPAN)
Posts: 53
Rep Power: 13 |
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 ? |
|
March 23, 2014, 21:05 |
|
#20 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,871
Rep Power: 144 |
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 . |
|
Tags |
cfx & fluent |
|
|
LinkBacks (?)
LinkBack to this Thread: https://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 | 17 | February 3, 2020 08:29 |
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 05:16 |
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 |