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

Mesh and Solve Times for CFX, Fluent, CD-adapco

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 4, 2011, 12:48
Default Mesh and Solve Times for CFX, Fluent, CD-adapco
  #1
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
Over a year ago, I was brought into my company to be the CFD specialist. Perviously, I had a long career in writing my own codes with spectral methods, so I am new to the commercial CFD side of things. I made the recommendation for CFX because wer were already using ANSYS products, CFX was fully integrated into Workbench, and the physics that we treat is not complicated. Now that I have some experience with CFX, I am now aware of some other issues and wonder if there is a better choice.

In my (limited) experience, CFX seems to be very time consuming for both meshing and solving. I've been treating relatively simple problems in terms of the physics (forced convection with air) but in complicated geometries (complex fin designs with lots of surfaces, thus lots of inflation). How do mesh and solve times compare between CFX and other products?

Additionally, it seems fairly common that my computer ends up running on vitual memory, crashes and/or corrupts the model. How do these issues compare between CFX and other products? Do other products use more than one processor by default? CFX only uses one processor, requiring a HPC license for more processors.

Thanks in advance for any thoughtful comments. I am very grateful for any advice.
Jade M is offline   Reply With Quote

Old   January 8, 2011, 05:34
Default
  #2
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 372
Rep Power: 10
arjun is on a distinguished road
Quote:
Originally Posted by Jade M View Post

In my (limited) experience, CFX seems to be very time consuming for both meshing and solving. I've been treating relatively simple problems in terms of the physics (forced convection with air) but in complicated geometries (complex fin designs with lots of surfaces, thus lots of inflation). How do mesh and solve times compare between CFX and other products?

The problem and strength both of CFX are its solver. Its major time consuming part is its solver which is based on multigrid preconditioned by BiCGStab (if i remember correctly, i do not use it). Plus it is a coupled algorithm. So in theory and in practice it shall converge very fast. This seems to be true. So what is the problem. The problem is that BiCG takes lots of time compared to gauss seidel of Fluent/Starccm+ .

Why is this a problem. This becomes a neuisence when you try to do unsteady simulation where you are supposed to run some fixed number of sub iterations and have to run simulation for some fixed number of time steps. Then calculations time would be at least 4 times of Fluent.

for steady state problems though it might end up saving time because of coupled algo with powerful matrix solver.

In sum, in CFX they have put best of everything on cost of computation time.

For me Fluent is fastest so far that is commercially available. (But is slower than some of the codes i have written).
arjun is offline   Reply With Quote

Old   January 10, 2011, 11:56
Default
  #3
Senior Member
 
Join Date: Feb 2010
Posts: 145
Rep Power: 8
Jade M is on a distinguished road
Thanks so much, arjun.

I talked with an ANSYS engineer who had some experience with both CFX and Fluent, and nearly 20 years of experience in CFD.

His comment was that CFX and Fluent are similar and that the equivalent settings could be set up in both software to give the same performance. He also commented that there is a trade off between numerical accuracy and model stability (as opposed to numerical stability, because I was having issues with my Workbench file crashing and getting corrupted).

Other general comments were that CFX is better for turbomachinery whiel Fluent is better for shocks and multiphase. CFX is better for general use and also is integrated into the Workbench environment.

These comments are from a particular engineer that I have a great deal of respect for. However, he does work for ANSYS and may not want to make one software sound better than the other.

What are your (and others') thoughts on this?

Originally, I was set on ANSYS products as we use their other software and I believe they have quality products. So then it was a matter of choosing between CFX and Fluent. Since we do have specialized applications, I thought CFX would be better. However, it might be worth reevaluating. I would appreciate any comments from experienced users.
Jade M is offline   Reply With Quote

Old   January 11, 2011, 00:52
Default
  #4
Senior Member
 
Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 372
Rep Power: 10
arjun is on a distinguished road
Quote:
Originally Posted by Jade M View Post
I talked with an ANSYS engineer who had some experience with both CFX and Fluent, and nearly 20 years of experience in CFD.

His comment was that CFX and Fluent are similar and that the equivalent settings could be set up in both software to give the same performance.
Nope. He is completely wrong here.
Fluent,StarCCM+ and to large extent openFOAM are similar solvers.
CFX is very different. There is no chance for same or similar settings.

Here are the major differences:
1. Quote from CFX manual : "CFX uses an element based finite volume method. " Page 363.
Then they explain what they mean by it. On page 364 there is figure 10.1. If you look at it you will understand in one glance that both can never be similar or same.

The thing is in CFX control volume is constructed by centers of mesh elements present in mesh that you load. In a way that each node in mesh that you loaded act as control volume center.
In fluent /starccm/openFOAM control volumes are the control volumes that you load in mesh. (no change).
In other words fluent and cfx do not solve equations at same points.

2. Both use Rhie Chow approach for interpolation but the way velocity is interpolated is completely different. Fluent,starccm+ use the approach explained in peric's book.(or very close to it). Where as cfx uses very different approach.

3. Even when in pressure based coupled solver fluent and cfx construct matrix in different manner. (manual does not say much about this issue but i guess Fluent's approach is much similar to M darvish

http://portal.acm.org/citation.cfm?id=1461314

I can list a lot of small difference but that would take up lots of space here.

Their multigrid solver is though very similar : both are additive corrective multigrid. (starccm+ openFOAM also share this part, not sure about the coupled versions though if they are present in starccm and openFOAM???).

so in theory when you use Fluent as pressure based coupled and set same setting as CFX they both shall be similarly slow :-D


There is one more issue. I think (i can be wrong) that mesh quality plays important role. For good meshes segregated approach may be faster because matrices shall converge without problem. But for poor meshes coupled algorithm and coupled matrix solver MIGHT be better way to go.
(this is just my guess never been tested).




Quote:
Originally Posted by Jade M View Post

Other general comments were that CFX is better for turbomachinery whiel Fluent is better for shocks and multiphase. CFX is better for general use and also is integrated into the Workbench environment.

These comments are from a particular engineer that I have a great deal of respect for. However, he does work for ANSYS and may not want to make one software sound better than the other.

What are your (and others') thoughts on this?

CFX products have reputation for turbomachinary. But one shall be careful. big part of that reputation comes because of CFX-Tascflow.
Tascflow is one that created that reputation and it was present till CFX 5 came along. Tascflow is no longer here but reputation that CFX products good for turbomachinary is continued.
Having said this i still believe for flows with strong swirl CFX may be better choice. (but this is my opinion and again i may be wrong).

Last edited by arjun; January 11, 2011 at 01:13.
arjun is offline   Reply With Quote

Old   August 28, 2012, 02:54
Default
  #5
New Member
 
iman
Join Date: Aug 2012
Location: malaysia
Posts: 10
Rep Power: 5
iman is on a distinguished road
Quote:
Originally Posted by arjun View Post
Nope. He is completely wrong here.
Fluent,StarCCM+ and to large extent openFOAM are similar solvers.
CFX is very different. There is no chance for same or similar settings.

Here are the major differences:
1. Quote from CFX manual : "CFX uses an element based finite volume method. " Page 363.
Then they explain what they mean by it. On page 364 there is figure 10.1. If you look at it you will understand in one glance that both can never be similar or same.

The thing is in CFX control volume is constructed by centers of mesh elements present in mesh that you load. In a way that each node in mesh that you loaded act as control volume center.
In fluent /starccm/openFOAM control volumes are the control volumes that you load in mesh. (no change).
In other words fluent and cfx do not solve equations at same points.

2. Both use Rhie Chow approach for interpolation but the way velocity is interpolated is completely different. Fluent,starccm+ use the approach explained in peric's book.(or very close to it). Where as cfx uses very different approach.

3. Even when in pressure based coupled solver fluent and cfx construct matrix in different manner. (manual does not say much about this issue but i guess Fluent's approach is much similar to M darvish

http://portal.acm.org/citation.cfm?id=1461314

I can list a lot of small difference but that would take up lots of space here.

Their multigrid solver is though very similar : both are additive corrective multigrid. (starccm+ openFOAM also share this part, not sure about the coupled versions though if they are present in starccm and openFOAM???).

so in theory when you use Fluent as pressure based coupled and set same setting as CFX they both shall be similarly slow :-D


There is one more issue. I think (i can be wrong) that mesh quality plays important role. For good meshes segregated approach may be faster because matrices shall converge without problem. But for poor meshes coupled algorithm and coupled matrix solver MIGHT be better way to go.
(this is just my guess never been tested).







CFX products have reputation for turbomachinary. But one shall be careful. big part of that reputation comes because of CFX-Tascflow.
Tascflow is one that created that reputation and it was present till CFX 5 came along. Tascflow is no longer here but reputation that CFX products good for turbomachinary is continued.
Having said this i still believe for flows with strong swirl CFX may be better choice. (but this is my opinion and again i may be wrong).
that was very helpful for me thank you
iman is offline   Reply With Quote

Reply

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


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
Can anybody tell me what does fluent do using MESH MOTION? enry FLUENT 0 October 6, 2010 12:54
Export 2D mesh from ICEM to Fluent BuilttoSpill ANSYS Meshing & Geometry 4 August 28, 2010 08:16
Importing ICEM mesh to Fluent mr_stoked FLUENT 1 June 25, 2010 03:24
mesh for fluent 12 hsn ANSYS Meshing & Geometry 4 September 17, 2009 14:54


All times are GMT -4. The time now is 09:06.