# Convegence problems while increasing the mesh resolution

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

 May 13, 2009, 08:42 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: 10 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!

 May 13, 2009, 10:50 #2 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 13 What does your mesh look like? Can you post an image? __________________ Schrödingers wife: "What did you do to the cat? It's half dead!"

 May 14, 2009, 02:54 #3 New Member   Marcin Hinz Join Date: May 2009 Location: Monheim am Rhein, Germany Posts: 24 Rep Power: 10 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!

May 14, 2009, 02:58
#4
New Member

Marcin Hinz
Join Date: May 2009
Location: Monheim am Rhein, Germany
Posts: 24
Rep Power: 10
The quality is not good enough, but i hope it will help You!
Attached Images
 Netz2.jpg (94.2 KB, 18 views) Netz_fein2.jpg (98.9 KB, 19 views)

 May 14, 2009, 03:32 #5 Senior Member     Sebastian Gatzka Join Date: Mar 2009 Location: Frankfurt, Germany Posts: 729 Rep Power: 13 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!"

 May 14, 2009, 05:20 #6 Senior Member     Jose Luis Santos Join Date: Mar 2009 Location: Portugal Posts: 215 Rep Power: 11 Hi, What is your y+? You'll need it to be > 30 for k-epsilon turbulence model. Regards, Jose Santos

 May 14, 2009, 08:51 #7 New Member   Marcin Hinz Join Date: May 2009 Location: Monheim am Rhein, Germany Posts: 24 Rep Power: 10 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.

 May 14, 2009, 09:23 #8 Member   Thomas Wolfanger Join Date: Mar 2009 Location: South West Germany Posts: 60 Rep Power: 10 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

May 14, 2009, 13:17
#9
Senior Member

Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 13
Quote:
 Originally Posted by anger 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!"

May 14, 2009, 13:26
#10
Senior Member

Sebastian Gatzka
Join Date: Mar 2009
Location: Frankfurt, Germany
Posts: 729
Rep Power: 13
Quote:
 Originally Posted by Marcin 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!"

 May 14, 2009, 13:39 #11 Senior Member     Jose Luis Santos Join Date: Mar 2009 Location: Portugal Posts: 215 Rep Power: 11 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

May 15, 2009, 07:35
#12
Member

Thomas Wolfanger
Join Date: Mar 2009
Location: South West Germany
Posts: 60
Rep Power: 10
Quote:
 Originally Posted by sega 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?

Best,
-Thomas

 May 20, 2009, 02:05 #13 New Member   Marcin Hinz Join Date: May 2009 Location: Monheim am Rhein, Germany Posts: 24 Rep Power: 10 Thank You for all the posts! Best Regards, Marcin.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Harmeet FLUENT 8 May 13, 2010 21:59 arya CFX 4 June 19, 2007 12:21 Vidya Raja FLUENT 1 October 13, 2005 13:52 hung FLUENT 7 April 18, 2005 09:38 Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09

All times are GMT -4. The time now is 04:50.