[crizpi21]

Hi Cagatayemre, this is the output running "checkMesh". Do you see anything wrong with it?

Checking geometry...
    Overall domain bounding box (0 0 0) (8 5.5 2.5)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-5.70422e-16 -3.12442e-16 -1.73464e-15) OK.
    Max cell openness = 2.63594e-15 OK.
    Max aspect ratio = 68.8 OK.
    Minimum face area = 4.95e-07. Maximum face area = 0.0545054.  Face area magnitudes OK.
    Min volume = 3.31031e-09. Max volume = 0.00843175.  Total volume = 109.878.  Cell volumes OK.
    Mesh non-orthogonality Max: 52.1642 average: 4.80993
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.67389 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

Originally Posted by Cagatayemre

You can play with included angle setting in surfaceFeatureExtractDict. Resolve feature angle in SnappyHexMeshDict works with includedAngle setting in terms of curvature (edge) refinement.

In surfaceFeatureExtractDict I have "includedAngle 180" so all the edges should be selected. [/QUOTE]How is your stl geometry quality ?[/QUOTE] How can I check this?

As to the divSchemes, I am already using bounded Gauss upwind schemes. I have seen that cell limited Gauss linear is suggested for poor quality meshes, do you consider my mesh to be like this? Anyway, I'll give it a go.

Moreover, I am not sure about the relation between all these parameters you suggested changing and the fact that the solver is not converging, could you explain this a bit more?

Thanks in advance for your help.


UPDATE: I have tried with grad schemes cell limited Gauss linear and still no convergence.

[Cagatayemre]

Hey Kristina, If I can see your geometry I may help you efficiently. Is your geometry complicated? Please try following schemes. Mesh quality results seems good but still it might lead to problems. It is hard to say something for me in terms of this results.

laplacianSchemes
{
default Gauss linear uncorrected;
}

snGradSchemes
{
default uncorrected;
}

Where do you have problem field ? Is the problem at outlet or stl surface? What is the refinement level there? You should visualize the mesh at that location for me. You should refine and coarsen the mesh and see the results at that specific location.

you can decrease the resolve Feature Angle in snappyHexMeshDict step by step. (if you set it to 0 degrees, you will have maximum refinement level everywhere.If you set it to 60 degrees, you can not gonna extra refine edges and curves that make angle between 0-60)

Example snappyHexMeshDict
refinementSurfaces -------------------------------------------------- level (4 6)
maximum refinement level 6 (curvatures and edges)
you can use this maximum refinement to refine curvatures, edges, etc.

I have experienced that after volume mesh generation process, at the boundary patches of the geometry some zero or negative area faces occur and velocity values at that specific cell can blows up(Solution is not converged).

Did you visualise the problem field (velocity field for example) and select that specific cell in paraview and add mesh quality filter. You might have a quadratic, hexahedral or different type of cell. You will see numbers corresponds to mesh quality in mesh quality filter. For instance, skew = 0.5 or edge ratio = 2.34 . Compare properties of the problem cell with the regular cells. You should split render view ; click spread sheet view button and click "show only selected elements" button

I have coarsen the surface with meshlab (decimal edge collapser without texture tool). (if you have 10 million faces on stl surface and only 4 cores to generate mesh with snappyHexMesh) I got some bad faces (looks weird) after coarsening process. Weighted coarsening in meshLab might solve this issue but it is too slow. Maybe we should run parallel with multiple cores.

surfaceCheck utility gives information about the stl geometry (or obj whatever) and also generates several patches from the geometry. Maybe you can split your geometry file with this utility and remesh locally. (Surface remesher and surface wrapper tool in Star CCM+ can do it with multiple cores.) We can use snappyHexMesh in order to generate volume mesh and extract remeshed surface with surfaceMeshTriangulate tool (you should search for openfoam.com/modules/utilities/surface. There are lots of interesting utilities in order to process surfaces.)

try to increase nSmoothScale in terms of meshQuality

[Himanshu_Shrivastava]

Hello,

sorry to open an old thread...


But can anyone please explain me what is the difference between sum local ,global and cumulative in continuity error.
Eg.: "time step continuity errors : sum local = 0.043, global = 1.13e-007, cumulative = 1.33e-007"

and Which one we have to check for deciding convergence?

P.S.: I come from fluent background where we see only one continuity residue.

Thank You

[qutadah.r]

Originally Posted by pierre

Hi Philippose,

I'll try to help, the code goes:

volScalarField contErr = fvc::div(phi);

scalar sumLocalContErr = runTime.deltaT().value()*
mag(contErr)().weightedAverage(mesh.V()).value();


Info<< "time step continuity errors : sum local = " << sumLocalContErr


since typically runTime.deltaT().value() = 1 for simpleFoam calculations (i.e. iteration counter), div(phi) is your face flux (interpolated velocity field) divergence and ideally is zero (if continuity is something you're looking for). The magnitude of div(phi) volume averaged over each cell should hence also tend to zero. If you want you can normalise it further to give you an idea of magnitude (maybe by dividing by average inlet face flux).

Hope this helps

Pierre

this is only for steady state incompressible flow as i believe and understand, and that is where it comes from. Do you think it is also needed in nonsteady calculations, ofcourse not in the same formulation but in other say pimpleFoam solver? Is it being calculated? an why do we even need this error? arent our residuals the thing we always look for?

thanks!

[efalpha]

Dear crizpi21,

Did you manage to solve the problem? If yes, i would ask you to post the solution if possible.