[tschenkel]

Hi,


I am in the process of migrating my FSI simulations from the old FSI toolbox to the new solids4foams.


I am currently running

Using: foam-extend-4.1 (see www.foam-extend.org)
Build: 4.1-5832cfe256a5



When I try to run the 3dTube/linearElastic3dTube tutorial case the case runs fine, however, paraview can't read the solid region:

...Error reading line 11260 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D: Found duplicated entries with keyword value


...Error reading line 8052 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D_0: Found duplicated entries with keyword value


...Error reading line 44 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D_0_0: Found duplicated entries with keyword value




Paraview is V5.6.0


What am I missing?

Best
Torsten

[tschenkel]

Update:

There seems to be a problem/bug in foam-extend-4.1 (MPI error in the pressure GAMG solver), which was a showstopper for me, so I reverted back to fe40, and recompiled solids4foam on fe40.

This problem does not show up then. So it seems to be caused by a change from fe40 to fe41.

Best
T

[Daniel_Khazaei]

Originally Posted by tschenkel

Update:

There seems to be a problem/bug in foam-extend-4.1 (MPI error in the pressure GAMG solver), which was a showstopper for me, so I reverted back to fe40, and recompiled solids4foam on fe40.

This problem does not show up then. So it seems to be caused by a change from fe40 to fe41.

Best
T

facing the exact same problem on fe41

[bigphil]

Originally Posted by tschenkel

Hi,


I am in the process of migrating my FSI simulations from the old FSI toolbox to the new solids4foams.


I am currently running

Using: foam-extend-4.1 (see www.foam-extend.org)
Build: 4.1-5832cfe256a5



When I try to run the 3dTube/linearElastic3dTube tutorial case the case runs fine, however, paraview can't read the solid region:

...Error reading line 11260 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D: Found duplicated entries with keyword value


...Error reading line 8052 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D_0: Found duplicated entries with keyword value


...Error reading line 44 of /home/acests3/foam/acests3-4.1/run/3dTube/linearElastic3dTube/0.0002/solid/D_0_0: Found duplicated entries with keyword value




Paraview is V5.6.0


What am I missing?

Best
Torsten

Hi Torsten,

I have checked this on my system (case run on Ubuntu 16.04 LTS with foam-extend-4.1, build 4.1-e01e16c94382, and the latest master branch of solids4Foam, with ParaView 5.6.0 on macOS) but am not getting an error.

One solution is to use foam-extend-4.0.

To try to determine where the problem is, I suggest you move all of the solid fields out of the time sub-directory and see if you can now read the solid region in ParaView. If this works, then move back in the fields one-by-one until you find the one that ParaView complains about. If you find the problem, hopefully, it may become clear how to fix it.

Philip

[tschenkel]

Hi Philip

I have not tested again with fe41 after upgrading to the master branch of solids4foam. Will try to do that next week.


The fields that are causing the problems are the D fields (D, D_0, D_0_0). If I disable them (unchecking them in the dialog in paraview, no need to move the files), the case reads fine and I can use the pointD field to warp the mesh to match the mesh motion of the fluid region.

I'll have to double check the MPI bug in fe41 as well, and open another thread on that (does your fe41 work in parallel with GAMG for p?).

Which compiler is recommended for fe41 and solids4foam?

I compiled both with gcc 4.8.5 on CentOS 7.6 for foam-extend 4.0, but fe41 doesn't seem to like gcc 4.8.5, so I used the gcc7 toolchain for that.

[tschenkel]

This has been resolved.

After a bugfix update in foam-extend 4.1 I


- pulled the current sources for both foam-extend-4.1 and solids4Foam-release
- recompiled both with the gcc7 toolchain on CentOS (Ubuntu 18.04 still compiling)


and the testcase is working fine now.

How do I change the thread title to include "SOLVED"?

[bigphil]

Great.

Done.

[Michael@UW]

Originally Posted by tschenkel

This has been resolved.

After a bugfix update in foam-extend 4.1 I


- pulled the current sources for both foam-extend-4.1 and solids4Foam-release
- recompiled both with the gcc7 toolchain on CentOS (Ubuntu 18.04 still compiling)


and the testcase is working fine now.

How do I change the thread title to include "SOLVED"?

I just recompiled foam-extedn 4.1 and solids4Foam on Ubuntu 18.04, but the issue is still the same. D, D_0, D_0_0, DD, DD_0 can not be loaded into Paraview due to duplicated entries.
This bug was fixed in OpenFOAM foundation version stated at https://bugs.openfoam.org/view.php?id=2737.

I wonder if it is fixed in foam-extend.

[Michael@UW]

It seems the values on "solidTraction boundary" are written twice.
Here is the output of linearElastic3dTube/0.0001/solid/D:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | foam-extend: Open Source CFD                    |
|  \\    /   O peration     | Version:     4.1                                |
|   \\  /    A nd           | Web:         http://www.foam-extend.org         |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0.0001";
    object      D;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 0 0 0 0 0];

internalField   nonuniform List<vector> 
6400
(

;

boundaryField
{
    inlet
    {
        type            fixedDisplacement;
        value           uniform (0 0 0);
    }
    outlet
    {
        type            fixedDisplacement;
        value           uniform (0 0 0);
    }
    inner-wall
    {
        type            solidTraction;
        gradient        nonuniform List<vector> 
1600
(
First time
)
;
        pressure        uniform 0;
        secondOrder     false;
        limitCoeff      1;
        relaxationFactor 1;
        value           nonuniform List<vector> 
1600
(
Second time!
)
;
    }
    symmetry-x
    {
        type            solidSymmetry;
        patchType       symmetryPlane;
        secondOrder     false;
        value           nonuniform List<vector> 
320
(

)
;
    }
    symmetry-y
    {
        type            solidSymmetry;
        patchType       symmetryPlane;
        secondOrder     false;
        value           nonuniform List<vector> 
320
(

)
;
    }
}


// ************************************************************************* //

[Michael@UW]

fvPatchVectorField::write(os) does the work.

void solidTractionFvPatchVectorField::write(Ostream& os) const
{
    //fixedGradientFvPatchVectorField::write(os);
    fvPatchVectorField::write(os);

    if (tractionSeries_.size())
    {
        os.writeKeyword("tractionSeries") << nl;
        os << token::BEGIN_BLOCK << nl;
        tractionSeries_.write(os);
        os << token::END_BLOCK << nl;
    }
    else
    {
#ifdef OPENFOAMFOUNDATION
        writeEntry(os, "traction", traction_);
#else
        traction_.writeEntry("traction", os);
#endif
    }

    if (pressureSeries_.size())
    {
        os.writeKeyword("pressureSeries") << nl;
        os << token::BEGIN_BLOCK << nl;
        pressureSeries_.write(os);
        os << token::END_BLOCK << nl;
    }
    else
    {
#ifdef OPENFOAMFOUNDATION
        writeEntry(os, "pressure", pressure_);
#else
        pressure_.writeEntry("pressure", os);
#endif
    }
    os.writeKeyword("secondOrder")
        << secondOrder_ << token::END_STATEMENT << nl;
    os.writeKeyword("limitCoeff")
        << limitCoeff_ << token::END_STATEMENT << nl;
    os.writeKeyword("relaxationFactor")
        << relaxFac_ << token::END_STATEMENT << nl;

#ifdef OPENFOAMFOUNDATION
    writeEntry(os, "value", *this);
#else
    writeEntry("value", os);
#endif
}

[Michael@UW]

It worked after I recompiled the solids4Foam!

[bigphil]

Thanks Michael@UW,

I will push this change to the development branch.
I guess this is a result of something changing in foam-extend-4.1.

Philip