Convegence problems while increasing the mesh resolution
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 steadystate 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! 
What does your mesh look like?
Can you post an image? 
5 Attachment(s)
Hi Sebastian,
thank You for Your quck anwser. Here are the images of both meshes: Mesh with 250000 elements: Attachment 293 Attachment 294 Mesh with 800000 elements: Attachment 295 Attachment 296 This is how it converge with the smaller mesh calculated wit kepsilon turbulence model. Attachment 297 I tried also to calculate it with komega model, but it dosen't seems to work even with the smaller mesh. I would be pleased, if You could help me. Best regards! 
2 Attachment(s)
The quality is not good enough, but i hope it will help You!

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? 
Hi,
What is your y+? You'll need it to be > 30 for kepsilon turbulence model. Regards, Jose Santos 
1 Attachment(s)
Hi!
Here is a closer image of the region, or did You mind some other? Attachment 301 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((rhoA(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 komega 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. 
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 
Quote:
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? 
Quote:
I'm rather new to turbulent simulations, but aren't second order schemes preferred? Or does this only apply to LES? 
I would try to:
1  Coarsen the mesh until obtaining y+>30 and use standard kepsilon model; 2  Refine the mesh until obtaining y+<1 and use any lowRe 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 
Quote:
Best, Thomas 
Thank You for all the posts!
Best Regards, Marcin. 
All times are GMT 4. The time now is 07:41. 