volPointInterpolation fails on a subMesh, when the baseMesh contains cyclicAMIs and the subMesh doesn't.

Summary

If a mesh contains cyclicAMIs, a subset of that mesh is created and then an interpolation is attempted from cell values to points on the subMesh (such as in a VTK export of a mesh subset) then the process fails when it tries to process AMI boundaries during volPointInterpolated::addSeparated from the volPointInterpolated constructor.

• It fails in both parallel and serial.
• If the interpolation switch is turned off in the function object, no error happens and the process proceeds as expected.
• For a similar test-case to that described below, if the submesh contains faces on the cyclicAMI boundaries then it appears to run OK.
• The latest version of OF for which this export works appears to be v1912.
• (In v2312 and earlier the error messages are different.)
• (I've not tested other similar boundary conditions such as cyclicsACMI and cyclicPeriodicAMI.)

Steps to reproduce

Add the following function-object to the standard v2412 pimpleFoam "mixerVesselAMI2D" tutorial case and run.

functions 
{ 
    vtkWrite
    {
        type vtkWrite;
        libs (utilityFunctionObjects);
        writeControl timeStep;
        writeInterval 1;
        interpolate true;
        boundary false;
        fields  (U p);
        selection
        {
            sphere
            {
                action use;
                source  sphere;
                origin  (0.045 0 0);
                radius  0.01;
            }
        }
    }
}

What is the current bug behaviour?

Running the aforementioned modified tutorial in serial in v2406 in Debug mode (and with volPointOptimisation Debug switch set to 1), yields the following error message at the end of the first time-step:

vtkWrite output Time: 0.00120482
    Internal  : "postProcessing/vtkWrite/mixerVesselAMI2D_00000001/internal.vtu"
volPointInterpolation::makeWeights() : constructing weighting factors
volPointInterpolation::calcBoundaryAddressing() : constructing boundary addressing
boundary:
    faces :96
    of which on proper patch:10
    points:98
    of which on proper patch:22
volPointInterpolation::makeInternalWeights() : constructing weighting factors for internal and non-coupled points.
volPointInterpolation::makeBoundaryWeights() : constructing weighting factors for boundary points.
volPointInterpolation::addSeparated
AMI: Creating AMI for source:AMI1 and target:AMI2
AMI: Patch source sum(weights) min:25469.3 max:25469.3 average:25469.3
AMI: Patch target sum(weights) min:25469.3 max:25469.3 average:25469.3


--> FOAM FATAL ERROR: (openfoam-2406)
Supplied field size is not equal to target patch size
    source patch = 96
    target patch = 96
    supplied field = 0

From void Foam::AMIInterpolation::interpolateToSource(const Foam::UList<T>&, const CombineOp&, Foam::List<T>&, const Foam::UList<T>&) const [with Type = double; CombineOp = Foam::multiplyWeightedOp<double, Foam::plusEqOp<double> >]
in file ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/AMIInterpolationTemplates.C at line 179.

FOAM aborting
[stack trace]
=============
#1  Foam::error::simpleExit(int, bool) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:313
#2  Foam::error::exiting(int, bool) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:271
#3  Foam::error::abort() at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/error.C:375
#4  Foam::Ostream& Foam::operator<< Foam::error(Foam::Ostream&, Foam::errorManipFoam::error) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/lnInclude/errorManip.H:93 (discriminator 4)
#5  void Foam::AMIInterpolation::interpolateToSource<double, Foam::multiplyWeightedOp<double, Foam::plusEqOp > >(Foam::UList const&, Foam::multiplyWeightedOp<double, Foam::plusEqOp > const&, Foam::List&, Foam::UList const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/AMIInterpolationTemplates.C:184 (discriminator 10)
#6  Foam::tmp<Foam::Field > Foam::AMIInterpolation::interpolateToSource<double, Foam::plusEqOp >(Foam::Field const&, Foam::plusEqOp const&, Foam::UList const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/AMIInterpolationTemplates.C:244
#7  Foam::tmp<Foam::Field > Foam::AMIInterpolation::interpolateToSource(Foam::Field const&, Foam::UList const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/AMIInterpolationTemplates.C:302
#8  Foam::tmp<Foam::Field > Foam::cyclicAMIPolyPatch::interpolateUntransformed(Foam::Field const&, Foam::UList const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/cyclicAMIPolyPatchTemplates.C:40
#9  Foam::tmp<Foam::Field > Foam::cyclicAMIPolyPatch::interpolate(Foam::Field const&, Foam::UList const&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/lnInclude/cyclicAMIPolyPatchTemplates.C:68
#10  Foam::cyclicAMIPointPatchField::swapAddSeparated(Foam::UPstream::commsTypes, Foam::Field&) const at ~/OpenFOAM/OpenFOAM-v2406/src/meshTools/AMIInterpolation/patches/cyclicAMI/cyclicAMIPointPatchField/cyclicAMIPointPatchField.C:183 (discriminator 2)
#11  void Foam::volPointInterpolation::addSeparated(Foam::GeometricField<double, Foam::pointPatchField, Foam::pointMesh>&) const at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/lnInclude/volPointInterpolate.C:113 (discriminator 2)
#12  Foam::volPointInterpolation::makeWeights() at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/interpolation/volPointInterpolation/volPointInterpolation.C:411
#13  Foam::volPointInterpolation::volPointInterpolation(Foam::fvMesh const&) at ~/OpenFOAM/OpenFOAM-v2406/src/finiteVolume/interpolation/volPointInterpolation/volPointInterpolation.C:480
#14  Foam::functionObjects::vtkWrite::write() at ~/OpenFOAM/OpenFOAM-v2406/src/functionObjects/utilities/vtkWrite/vtkWrite.C:423 (discriminator 3)
#15  Foam::functionObjects::timeControl::write() at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/db/functionObjects/timeControl/timeControlFunctionObject.C:545
#16  Foam::functionObjectList::execute(bool) at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/db/functionObjects/functionObjectList/functionObjectList.C:770 (discriminator 7)
#17  Foam::Time::run() const at ~/OpenFOAM/OpenFOAM-v2406/src/OpenFOAM/db/Time/Time.C:824
#18  ? at ~/OpenFOAM/OpenFOAM-v2406/applications/solvers/incompressible/pimpleFoam/pimpleFoam.C:122
#19  ? in /lib64/libc.so.6
#20  __libc_start_main in /lib64/libc.so.6 #21 (closed) ? in ~/OpenFOAM/OpenFOAM-v2406A/platforms/linux64Gcc85DPInt32Debug/bin/pimpleFoam
=============
Abort (core dumped)

Note that v2412 gives a very similar error message - the example is in v2406 as a debug compilation of that was already available.

What is the expected correct behavior?

The export should complete OK!

Relevant logs and/or images

Environment information

• OpenFOAM version : v2006 through v2412
• Operating system : Centos7.9/Rocky9.3
• Hardware info :
• Compiler : gcc various

Possible fixes

The submesh/volPointInterpolation/cyclicAMI needs to recognise that there are no non-"empty" cyclicAMI patches remaining and process accordingly.

At first sight:

• volPointInterpolation gets constructed on the sub fvMesh (as it should)
• but then looks up the pointMesh from the original mesh database:

    const pointMesh& pMesh = pointMesh::New(mesh());

• this returns the pointMesh of the original mesh and not the pointMesh of the sub mesh so all the patch faces counts are wrong.
• checked the sub mesh and the number of faces on the cyclicAMI is indeed 0 so the field size is correct, it is the patch sizes that are incorrect:

--> FOAM FATAL ERROR: (openfoam-2412)
Supplied field size is not equal to target patch size
    source patch   = 96
    target patch   = 96
    supplied field = 0

mentioned in commit a77aaa75

Thanks David for reporting. The problem was all the additional addressing was not cleared out. This is generally not a problem since it gets calculated but there was a special exit for 0 overall faces. Please re-open if there is still a problem.

closed

reopened

        if (tgtPatch.size())
        {
            tgtMagSf_.resize_nocopy(tgtPatch.size());
        }

Thanks for looking at this, I haven't tested the new code, but just wondered after looking at the new code, if this check is correct? The other 3 occurrences check for size of the current object (i.e. tgtMagSf_), whereas this one checks for the size on the patch.

You are right. Am just trying to detect the optional data. Too much copy&paste.

Will still give a problem if going from 0 to non-zero but can't think of any occurrence.

mentioned in commit 6dd8804a

Having tested the new code on a couple of cases, I can confirm that the issue appears fixed. Thanks Mattijs.

closed

added community label