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

Coarser meshes can produce better results?

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

Like Tree1Likes
  • 1 Post By FMDenaro

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 21, 2019, 08:04
Default Coarser meshes can produce better results?
  #1
New Member
 
anonymous
Join Date: Apr 2018
Posts: 26
Rep Power: 6
asda3D is on a distinguished road
Hi everyone,
I am comparing several meshes which utilise coupling CFD and experimental techniques against a fully resolved fine mesh model (19,000 elements using k epsilon model)

The coarse meshes are listed below

CMesh1-630 elements
CMesh2- 960 elements
CMesh3- 2400 elements
CMesh4- 3600 elements

What I have found out is that Cmesh1 produced the most accurate results (temp velocity pressure drop etc) compared to the fine mesh.

I am finding it difficult to explain this phenomenon. What I have learnt from my CFD lectures, is that a denser mesh provides more accurate results because it is more accurately interpolated between two points that are much closer together spatially.

Does anyone know why this could be the case, or point me in the direction of where to look, maybe mesh skewness plays a part.

Thank you in advance
asda3D is offline   Reply With Quote

Old   April 21, 2019, 12:16
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by asda3D View Post
Hi everyone,
I am comparing several meshes which utilise coupling CFD and experimental techniques against a fully resolved fine mesh model (19,000 elements using k epsilon model)

The coarse meshes are listed below

CMesh1-630 elements
CMesh2- 960 elements
CMesh3- 2400 elements
CMesh4- 3600 elements

What I have found out is that Cmesh1 produced the most accurate results (temp velocity pressure drop etc) compared to the fine mesh.

I am finding it difficult to explain this phenomenon. What I have learnt from my CFD lectures, is that a denser mesh provides more accurate results because it is more accurately interpolated between two points that are much closer together spatially.

Does anyone know why this could be the case, or point me in the direction of where to look, maybe mesh skewness plays a part.

Thank you in advance



What you learned is correct when you consider that the local truncation error of a discretization vanishes for vanishing mesh size.
However,

1) the monotonically decreasing slope of the error appears only after a sufficiently small mesh size, before you could see oscillations of the error.
2) You are using a turbulence model, that means you can have some supplementary effect due to the way the model acts.
3) some bug could be always present in the setting ( that is BC.s or some modelling parameter).
4) 19000 elements is still a very coarse mesh for simulating turbulence, in particular if you have wall turbulence
allanZHONG likes this.
FMDenaro is offline   Reply With Quote

Old   April 21, 2019, 12:51
Default
  #3
New Member
 
anonymous
Join Date: Apr 2018
Posts: 26
Rep Power: 6
asda3D is on a distinguished road
Thank you for the informative reply,
Firstly this mesh is modelling a fuel bundle inside a reactor core.
In regards to the mesh being too coarse. Using the k epsilon model a y plus of 30 was needed. I started with a 42,000 elemnt model. Any more elements and the domain would satart displaying a large expansion ration which isn't good.

Additionally,through a sensitvity analysis I lost around 4% of accuracy when reducing the mesh density to 19,000

I have been thinking of maybe trying a low reynolds number model which current possesses 390,000 elements (still working on it) and see if that maybe produces better results.

I must also mention i have accounted for roughness aswell. The CFD package had little information about roughness so this could be an issue maybe too.

I will also investigate aspect ratios, skewness and other mesh quality criteria to see of i can find a relationship explaining this problem.

Thank you.
asda3D is offline   Reply With Quote

Old   April 21, 2019, 12:55
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Do not forget to check the convergence criteria, are they satisfied at the same level on each grid?


Your flow problem requires a mesh-indipendence study, that is you need to refine more and more the grid until the solution does not change anymore.


Of course, it could be also debated if the reference solution you're using is really accurate...
FMDenaro is offline   Reply With Quote

Old   April 21, 2019, 13:00
Smile
  #5
New Member
 
anonymous
Join Date: Apr 2018
Posts: 26
Rep Power: 6
asda3D is on a distinguished road
That was a very quick response that is highly appreciated.

Five lines of interest were created across the domain to ensure mesh convergence was achieved. 18 points of intereest were set for the residual monitoring thay also showed good results.
Even simulating the 42,000 mesh its values lies almost identical to the 19,000 mesh. For example there is a 1.16% difference in pressure gradient values for these two meshes.

I will investigate further to see if i can resolve this.
Thank you FMdenaro for your input
asda3D is offline   Reply With Quote

Old   April 21, 2019, 17:29
Default
  #6
New Member
 
anonymous
Join Date: Apr 2018
Posts: 26
Rep Power: 6
asda3D is on a distinguished road
Just an add on the aspect ration is more than double for the finer meshes compared to the coarser meshes. This may be the reason for the coarser meshes possessing greater accuracy.
asda3D is offline   Reply With Quote

Old   April 21, 2019, 23:00
Default
  #7
Member
 
Steve
Join Date: Mar 2018
Location: South Korea
Posts: 69
Rep Power: 6
steve lee is on a distinguished road
If your reference data is completely correct.
All of your cases are wrong I think.

4 cases can not simulate correctly.
But your first case was converged the correct solution with wrong way.
Maybe the pressure or velocity fields are not the same comparing reference solution.

And.. you should check not only the number of mesh but also y+ or correct usage of tubulence model

As FMdenaro mentioned mesh should be finer when the solution is not changed.
steve lee is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
bad momentum source, vortice direction with twoPhaseEulerFoam and non-ortho meshes cutter OpenFOAM Running, Solving & CFD 7 November 17, 2016 15:17
compare results from two meshes sgr OpenFOAM Post-Processing 4 July 1, 2015 07:38
Different results from similar quality cfx and ICEM meshes Nick R CFX 3 January 17, 2011 08:48
Different Results from Fluent 5.5 and Fluent 6.0 Rajeev Kumar Singh FLUENT 6 December 19, 2010 12:33
Which do you prefer? 6.1 or6.2? Jen FLUENT 9 May 31, 2005 04:21


All times are GMT -4. The time now is 12:03.