[gfilip]

Hello,

I'd like to take advantage of the new lowWeightCorrection feature in OF2.3.x. I modified the AMI patches in polyMesh/boundary to include the lowWeightCorrection keyword:

    AMI1
    {
        type            cyclicAMI;
        inGroups
        2
        (
        cyclicAMI
        baffleFaces
        )
        ;
        nFaces          54328;
        startFace       6857788;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI2;
        lowWeightCorrection 0.2;
    }
    AMI2
    {
        type            cyclicAMI;
        inGroups
        2
        (
        cyclicAMI
        baffleFaces
        )
        ;
        nFaces          54328;
        startFace       6912116;
        matchTolerance  0.0001;
        transform       noOrdering;
        neighbourPatch  AMI1;
        lowWeightCorrection 0.2;
    }

Once I run interDyMFoam with the modified boundary file, I get the following error:

--> FOAM FATAL ERROR: 
Employing default values when sum of weights falls below 0.2 but supplied default field size is not equal to target patch size
    default values = 0
    source patch   = 54328

but right before this error, I get the following information indicating that the source and target patch sizes are matched:

AMI: Creating addressing and weights between 54328 source faces and 54328 target faces
AMI: Patch source sum(weights) min/max/average = 1, 1.0847458, 1.0000261
AMI: Patch target sum(weights) min/max/average = 1, 1.0847458, 1.0000261

I also get the same error after regenerating the grid with the OF2.3.x snappyHexMesh. Is this related to the modification of the propeller tutorial (using cell and face sets in 2.2.x versus patches for AMI generation in 2.3.x)?

Thanks for your help.

[PorscheGTIII]

I'm getting this error as well. I was able to run potentialFoam without problems, but when I tried to run simpleFoam I get the same error after displaying the AMI information and Selecting the turbulence model.

[gfilip]

I can confirm as well that when running my case without turbulence modeling (laminar), the error goes away.

[gfilip]

Chris, are you trying to use kOmegaSST by any chance? I tried switching to kOmega and kEpsilon and both of those turbulence models work without producing that error.

I submitted a bug on the tracker.

[PorscheGTIII]

Yes, I was using the kOmegaSST model. I can confirm that there is no problem using the laminar model or using the kOmega model.

I've ran this case case using OpenFOAM 1.6-ext and their GGI implementation and have had great success. It's a little frustrating why this grid interpolation method is having problems with the interpolation weights when the extended version is doing it without any problems.

[PorscheGTIII]

gfilip, do you get this same error when you try to post-process results with the yPlusRAS command if you used another turbulence model?

[gfilip]

Just tested that, and yes yPlusRANS fails with the same error even though the simulation ran with kOmega.

[gfilip]

FYI: the issue is now resolved by commit 8fa487c

[PorscheGTIII]

Just a quick question. If I installed through the apt package management tool, do I have to do anything to get this new commit?