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

Numerical Diffusion in Star and Fluent

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

Like Tree1Likes
  • 1 Post By flotus1

Reply
 
LinkBack Thread Tools Display Modes
Old   November 25, 2013, 18:31
Question Numerical Diffusion in Star and Fluent
  #1
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
So I recently worked on a laminar mixing species transport problem in Star. I had done this problem in Fluent before and gotten good results, so I wanted to see how robust star's solver would be. It was a simply Y connection with two similar species. I noticed that, unless I had the mesh aligned with the flow, I got crazy amounts of numerical diffusion. The same problem in Fluent however was handled (similar mesh size and settings, also unstructured) just fine, with almost no noticeable numerical diffusion.

I have three questions:
1. Has anyone experienced this before?
2. Is this a sign that Star's solver might simply be weaker?
3. Does this mean that their solvers for all other equations might fall to the same weakness? I.e. should I be worried about momentum and turbulence models being too diffuse?
MachZero is offline   Reply With Quote

Old   November 26, 2013, 07:30
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
This might simply be an issue with the default setting for the calculation of convective fluxes.
Did you really use similar schemes in both solvers?
FMDenaro likes this.
flotus1 is offline   Reply With Quote

Old   November 26, 2013, 08:31
Default Numerical diffusion
  #3
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Thanks for your response. To my knowledge the default order for the equation in star is 2nd order. I'll check this today to be sure. I did look through and changed the diffusion model from Schmidt number to an appropriate diffusion coefficient. I using the exact same geometry.

Any other thoughts? I am hopeful there is something silly that I missed and that it doesn't have a ridiculously high numerical diffusion.
MachZero is offline   Reply With Quote

Old   November 27, 2013, 10:25
Default
  #4
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
I noticed you opened the same thread in the CCM+ subforum.
Are we talking about StarCD or about CCM+ ?

For CCM+ and Fluent, I know for a fact that you can obtain accurate results with good control over the numerical diffusion errors.
flotus1 is offline   Reply With Quote

Old   November 27, 2013, 11:18
Default
  #5
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 185
Rep Power: 9
JBeilke is on a distinguished road
ccm+ can read fluent case files. So you can use exactly the same mesh in both codes.

Do you use the same methodology to determine the numerical diffusion in both codes?
JBeilke is offline   Reply With Quote

Old   November 27, 2013, 13:06
Default
  #6
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
I never compared both tools with a methologic approach to cover this specific topic.

But if you really want to do so, I suggest the typical test case for numerical diffusion: the transport of a passive scalar.
flotus1 is offline   Reply With Quote

Old   November 27, 2013, 14:29
Default Same Mesh
  #7
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Hey Guys, thanks for keeping this alive. I am really hopeful I forgot something silly and that CCM doesnt lag behind fluent this noticeably.

Yes, I was referring to CCM+. Sorry about that, I forgot that they have two.

The test I am doing is a simple Y junction with species transport, which I assume is similar to the passive scalar. I have posted two pictures. Both use the same mesh, and have the same fluid properties. To my knowledge, the species transport is 2nd order on both. I have turned the diffusion down to 1e-30, so any mixing seen should be numerical error.

I will attach images showing the results from both Fluent and CCM. While in this case it looks like the numerical diffusion is maybe double in Star CCM, I have a more complicated geometry that I have been working with and it is much more noticeable.

Do you think there is anythign else worth investigating? Gradients or settings or whatnot? I noticed when I made a poly mesh in this geometry the diffusion seemed almost worse. Only when I did a trim mesh asigned with the flow did it give reasonable results.

Thoughts? Thanks in advance for the conversation
Attached Images
File Type: jpg FluentND.jpg (31.8 KB, 29 views)
File Type: jpg ccmND.jpg (31.4 KB, 27 views)
MachZero is offline   Reply With Quote

Old   November 27, 2013, 17:00
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,605
Rep Power: 23
FMDenaro will become famous soon enough
second order means nothing... you can have a central second order as well as an upwind second order...check the exact scheme you are using in time and space
FMDenaro is offline   Reply With Quote

Old   November 28, 2013, 03:13
Default
  #9
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 185
Rep Power: 9
JBeilke is on a distinguished road
Set the gradient method to "Green-Gauss" and the gradient limiter method to "Modified Venkatakrishnan".
JBeilke is offline   Reply With Quote

Old   November 28, 2013, 12:56
Default
  #10
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Thanks again for the comments and suggestions.

I looked into the order of the schemes. In fluent it is a 2nd order upwind. But CCM+ doesnt really state which kind it is. I looked into their documentation regarding the segregated species solver but I didnt see any mention. A bit odd.

I tried changing the suggested gradients, but it didnt make much of a change. I fined the Fluent grid to get an idea of how a finer mesh would help. You can see the attached results. I used the same grid for CCM+. I show results for the default and altered gradient methods.

When I talked to a support engineer, they kinda glossed over this fact and said to try a different trim grid. Sure that works, but I will not always be able to have a grid aligned with the flow, so I do not consider that to be a sufficient answer to this problem.

Any final thoughts as to what else to try? I have 2 more days on my trial license. As always, thanks for all and every idea. I appreciate them.
Attached Images
File Type: jpg ccmND_refined.jpg (37.4 KB, 21 views)
File Type: jpg FluentND_refined.jpg (28.4 KB, 20 views)
MachZero is offline   Reply With Quote

Old   November 28, 2013, 13:08
Default
  #11
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,605
Rep Power: 23
FMDenaro will become famous soon enough
In Fluent you can set the centred second order scheme, avoiding numerical diffusion produced by the upwind discretization
FMDenaro is offline   Reply With Quote

Old   November 28, 2013, 13:32
Default
  #12
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Good to know. Thanks. I don't know of any way to do that in ccm+
MachZero is offline   Reply With Quote

Old   November 28, 2013, 14:40
Default
  #13
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 185
Rep Power: 9
JBeilke is on a distinguished road
@MachZero

I used a temperature test case and the alternative gradient settings improved the solution quite a lot.

Now when using a passive scalar test case the original setup seems to produce slightly better results. Which is what we can also see from your pictures.

But the most impressing result we get by switching between first and second order ;-)
JBeilke is offline   Reply With Quote

Old   November 28, 2013, 15:12
Default
  #14
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Yeah. For comparison I switched to first order (secretly hoping they accidentally
Mislabeled the methods) and it was starkly different. Still surprising how different it was from fluent a results
MachZero is offline   Reply With Quote

Old   November 28, 2013, 22:03
Default
  #15
Senior Member
 
Julien de Charentenay
Join Date: Jun 2009
Location: Australia
Posts: 229
Rep Power: 9
julien.decharentenay is on a distinguished road
Send a message via Skype™ to julien.decharentenay
Interesting thread and question. How is the velocity field behaving? Could it have an impact on the scalar diffusion?

Fluent & Star-CCM+ both uses limiters. The difference may be in the impact of these limiters and implementation of the convective schemes.
__________________
---
Julien de Charentenay
julien.decharentenay is offline   Reply With Quote

Old   November 29, 2013, 06:22
Default
  #16
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 185
Rep Power: 9
JBeilke is on a distinguished road
You can try the "Use TVB Gradient Limiting" and also increase the "Acceptable Field Variation (Factor)" to 0.1

This reduced the numerical diffusion at my passiv scala based test case.
JBeilke is offline   Reply With Quote

Old   November 29, 2013, 07:27
Default
  #17
Senior Member
 
sbaffini's Avatar
 
Paolo Lampitella
Join Date: Mar 2009
Location: Italy
Posts: 531
Blog Entries: 14
Rep Power: 17
sbaffini will become famous soon enough
Consider that you also have rhie-chow and pressure interpolation which also affects the velocity field. I don't think you can be sure of the settings of both codes unless you have definitive information from the manuals. I'm sure about Fluent, while this doesn't seem to be the case for Star.

Also, how are boundary conditions at wall treated in the two solvers?

It is quite obvious, tough, that if the codes were identical you would have obtained the exact same results. There is certainly something different
sbaffini is offline   Reply With Quote

Old   December 2, 2013, 11:05
Default License run out
  #18
Member
 
Join Date: Aug 2011
Posts: 54
Rep Power: 5
MachZero is on a distinguished road
Thanks for the replies. My trial license has run out so I can therefore no longer run these tests. During the trial I ran a variety of tests with fluent and star ccm including low re flow over an ellipse, turbulent flow over a cylinder, and micro fluidic mixing. I was unable to get the low re ellipse drag to be within 40% of experiment (40% low). I was unable to get transient averaged cylinder cd to match within 35% (too high). I worked with an engineer from ccm on those so I assume they have been done correctly.

The concern for me is this numerical diffusion issue. Assuming it isn't a simple setting that needs to be handled, more complex micro fluidic problems show very large diffusion based issues. My question is, should I be concerned with the accuracy and numerical diffusion of this code elsewhere (I.e. In other transport equations)? The differences I am seeing with species transport are simply concerning
MachZero is offline   Reply With Quote

Old   December 2, 2013, 11:21
Default
  #19
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,605
Rep Power: 23
FMDenaro will become famous soon enough
Quote:
Originally Posted by MachZero View Post
Thanks for the replies. My trial license has run out so I can therefore no longer run these tests. During the trial I ran a variety of tests with fluent and star ccm including low re flow over an ellipse, turbulent flow over a cylinder, and micro fluidic mixing. I was unable to get the low re ellipse drag to be within 40% of experiment (40% low). I was unable to get transient averaged cylinder cd to match within 35% (too high). I worked with an engineer from ccm on those so I assume they have been done correctly.

The concern for me is this numerical diffusion issue. Assuming it isn't a simple setting that needs to be handled, more complex micro fluidic problems show very large diffusion based issues. My question is, should I be concerned with the accuracy and numerical diffusion of this code elsewhere (I.e. In other transport equations)? The differences I am seeing with species transport are simply concerning

the problem is not simple...the key of your question is: does the numerical viscosity overwhelms the molecular one in such a way to affect in a relevant way the solution?

The analsysis and the answer depends on a) the type of scheme b) the flow problem.
Laminar flows do not suffer so much but if you want simulate transitional and turbulent flows then the numerical viscosity must be reduced by using high order low-artificial-viscosity discretizations. On the other hand, turbulent flows simulated with statistical models (such as RANS) have solution where the model overwhelms also the numerical viscosity and this problem is less relevant also using low order discretizations.
FMDenaro is offline   Reply With Quote

Reply

Tags
fluent, numerical diffusion, species mixing, star ccm+

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
Fluent Vs Star CCM firda Main CFD Forum 3 February 26, 2011 03:51
Changing from STAR to FLUENT - Solver Troubles BastiL FLUENT 0 February 15, 2008 17:41
How to convert STAR mesh into FLUENT mesh ? Jihwan CD-adapco 8 November 10, 2004 05:11
fluent to star samy CD-adapco 0 January 30, 2003 14:05
Convert FLUENT mesh to some other format for STAR? Jiaying Xu FLUENT 3 December 5, 2002 09:15


All times are GMT -4. The time now is 04:41.