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

Convegence problems while increasing the mesh resolution

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 13, 2009, 08:42
Default Convegence problems while increasing the mesh resolution
  #1
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hello everyone!

I am a new member and a new OpenFoam user. My first exersise is to simulate an example quite simmilar to the AngledDuct (rhoPimpleFoam) from the tutorials with some small changes:
- it has to be a steady-state simulation (i've repleaced the PIMPLE with the SIMPLE algorithm)
- the boudary conditions are: total pressure (12 bar) in inlet, temperature ( 400 K ) also in inlet and a static pressure (11 bar) in outlet

The tutorial mesh seams to converge, however while importing meshes from gambit wit higher resolution i have some problems with convergence (250000 elements converges , 800000 elements dosen't)

I'm even not quite sure, if my boundary conditions for k and epsilon are ok (they were also transfered from the tutorial)

Mayby someone of You have any sugestions?

Best regards!
Marcin is offline   Reply With Quote

Old   May 13, 2009, 10:50
Default
  #2
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
What does your mesh look like?
Can you post an image?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   May 14, 2009, 02:54
Default
  #3
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hi Sebastian,

thank You for Your quck anwser. Here are the images of both meshes:

Mesh with 250000 elements:

Netz_forum.jpg

Netz2_forum.jpg

Mesh with 800000 elements:

Netz_fein2_forum.jpg

Netz_fein_forum.jpg

This is how it converge with the smaller mesh calculated wit k-epsilon turbulence model.

residuals_forum.jpg

I tried also to calculate it with k-omega model, but it dosen't seems to work even with the smaller mesh.

I would be pleased, if You could help me.

Best regards!
Marcin is offline   Reply With Quote

Old   May 14, 2009, 02:58
Default
  #4
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
The quality is not good enough, but i hope it will help You!
Attached Images
File Type: jpg Netz2.jpg (94.2 KB, 17 views)
File Type: jpg Netz_fein2.jpg (98.9 KB, 19 views)
Marcin is offline   Reply With Quote

Old   May 14, 2009, 03:32
Default
  #5
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Dear Marcin.

I'm just brainstorming, but a possible cause for the problem may be in the connecting region of the two straight pipes. As I have experienced OpenFOAM has sometimes problems dealing with such 'skewed' elements.

Do you have a closer image of the region?
Are you using corrected flux schemes? Maybe you can post your fvSchemes dictionary?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   May 14, 2009, 05:20
Default
  #6
Senior Member
 
santos's Avatar
 
Jose Luis Santos
Join Date: Mar 2009
Location: Portugal
Posts: 213
Rep Power: 9
santos is on a distinguished road
Send a message via Skype™ to santos
Hi,

What is your y+? You'll need it to be > 30 for k-epsilon turbulence model.

Regards,
Jose Santos
santos is offline   Reply With Quote

Old   May 14, 2009, 08:51
Default
  #7
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Hi!

Here is a closer image of the region, or did You mind some other?

connecting_region.jpg

My fvSchemes file looks like that:

ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phid,p) Gauss upwind;
div(phiU,p) Gauss linear;
div(phi,h) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(phi,omega) Gauss upwind;
div((rho*R)) Gauss linear;
div(R) Gauss linear;
div(U) Gauss linear;
div((muEff*dev2(grad(U).T()))) Gauss linear;
}
laplacianSchemes
{
default none;
laplacian(muEff,U) Gauss linear corrected;
laplacian(mut,U) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DomegaEff,omega) Gauss linear corrected;
laplacian((rho|A(U)),p) Gauss linear corrected;
laplacian(alphaEff,h) Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p;
}

What would be the cause, that the SST k-omega model dosen't coverg? Also with the finer mesh. Mayby the BC are bad adjusted?

Dear Santos, my y+ is < 30 in the smaller mesh, so this could be the reason for it. I have started the same simulation with CFX, but it takes a lot of time to get an achivement of this simulation. Isn't it so, that in the case with small mesh the SST model schould converg?

Thanks a lot for Your anwsers!

Regards, Marcin.
Marcin is offline   Reply With Quote

Old   May 14, 2009, 09:23
Default
  #8
Member
 
Thomas Wolfanger
Join Date: Mar 2009
Location: South West Germany
Posts: 60
Rep Power: 8
anger is on a distinguished road
Hi Marcin,

it may be the case that unsteadiness in the flow which does not affect the solution for the coarse mesh will prevent the solution from converging when using a finer mesh. You can check whether this is the case by simply doing a transient run and check convergence there.

Best,
-Thomas
anger is offline   Reply With Quote

Old   May 14, 2009, 13:17
Default
  #9
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Quote:
Originally Posted by anger View Post
it may be the case that unsteadiness in the flow which does not affect the solution for the coarse mesh will prevent the solution from converging when using a finer mesh.
How can unsteadiness be a problem in a turbulent simulation, as it is the prominent feature of the flow?
Why should this be a problem on a finer grid, as the fluctuations are present even on the coarse mesh?

By the way, how can a turbulent flow be calculated in steady state?
Is the result one snapshot of the flow? There is not averaging involved?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   May 14, 2009, 13:26
Default
  #10
Senior Member
 
sega's Avatar
 
Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 11
sega is on a distinguished road
Quote:
Originally Posted by Marcin View Post
Here is a closer image of the region, or did You mind some other?
These elements look very 'elongated'. Can this cause any problems in combination with the upwind-scheme for div(phi,U)?

I'm rather new to turbulent simulations, but aren't second order schemes preferred? Or does this only apply to LES?
__________________
Schrödingers wife: "What did you do to the cat? It's half dead!"
sega is offline   Reply With Quote

Old   May 14, 2009, 13:39
Default
  #11
Senior Member
 
santos's Avatar
 
Jose Luis Santos
Join Date: Mar 2009
Location: Portugal
Posts: 213
Rep Power: 9
santos is on a distinguished road
Send a message via Skype™ to santos
I would try to:

1 - Coarsen the mesh until obtaining y+>30 and use standard k-epsilon model;

2 - Refine the mesh until obtaining y+<1 and use any low-Re model;

3 - Repeat 1 and 2 in transient mode.

Sebastian: The upwind scheme has the opposite effect, it normally damps instabilities that may build up on your flow. 2nd order schemes are in general less dissipative, and more prone to give you convergence problems.

Regards,
Jose Santos
santos is offline   Reply With Quote

Old   May 15, 2009, 07:35
Default
  #12
Member
 
Thomas Wolfanger
Join Date: Mar 2009
Location: South West Germany
Posts: 60
Rep Power: 8
anger is on a distinguished road
Quote:
Originally Posted by sega View Post
How can unsteadiness be a problem in a turbulent simulation, as it is the prominent feature of the flow?
Why should this be a problem on a finer grid, as the fluctuations are present even on the coarse mesh?

By the way, how can a turbulent flow be calculated in steady state?
Is the result one snapshot of the flow? There is not averaging involved?
Noone can prevent you from calculating turbulent flow steady state by doing some mathematical operations on the equations of motion. Keeping in mind that this does not correspond to the nature of the flow however is your task. You often do get meaningful results, but in cases where large sacle unsteadiness exists you may have bad convergence behaviour. This is where mesh resolution comes into play. If the mesh is coarse, for example flow separation which causes unsteadiness may not be detected and convergence will occur. In other words, the problem is linked to the scales of turbulence present in the flow. But how does unsteadiness come into a steady state simulation? The unsteadiness enters the simulation due to its iterative nature. As a consequence, if you perform a steady state simulation on a flow with large scale turbulence, you will not reach a converged solution and depending on the iteration number you get different pictures of the flow.

Best,
-Thomas
anger is offline   Reply With Quote

Old   May 20, 2009, 02:05
Default
  #13
New Member
 
Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 8
Marcin is on a distinguished road
Thank You for all the posts!

Best Regards, Marcin.
Marcin 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
STL File - Mesh Surface Problems Harmeet FLUENT 8 May 13, 2010 21:59
basic of mesh refinement arya CFX 4 June 19, 2007 12:21
Improving mesh resolution Vidya Raja FLUENT 1 October 13, 2005 13:52
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 14:15.