CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Convegence problems while increasing the mesh resolution (http://www.cfd-online.com/Forums/openfoam/64503-convegence-problems-while-increasing-mesh-resolution.html)

Marcin May 13, 2009 08:42

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 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!

sega May 13, 2009 10:50

What does your mesh look like?
Can you post an image?

Marcin May 14, 2009 02:54

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 k-epsilon turbulence model.

Attachment 297

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 May 14, 2009 02:58

2 Attachment(s)
The quality is not good enough, but i hope it will help You!

sega May 14, 2009 03:32

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?

santos May 14, 2009 05:20

Hi,

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

Regards,
Jose Santos

Marcin May 14, 2009 08:51

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((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.

anger May 14, 2009 09:23

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

sega May 14, 2009 13:17

Quote:

Originally Posted by anger (Post 216088)
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?

sega May 14, 2009 13:26

Quote:

Originally Posted by Marcin (Post 216082)
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?

santos May 14, 2009 13:39

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

anger May 15, 2009 07:35

Quote:

Originally Posted by sega (Post 216115)
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

Marcin May 20, 2009 02:05

Thank You for all the posts!

Best Regards, Marcin.


All times are GMT -4. The time now is 09:45.