CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions > OpenFOAM CC Toolkits for Fluid-Structure Interaction

[solids4Foam] SOLVED: Paraview can't read solids files (duplicate entries with keyword value)

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By bigphil

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   November 4, 2019, 03:26
Default SOLVED: Paraview can't read solids files (duplicate entries with keyword value)
  #1
Member
 
Torsten Schenkel
Join Date: Jan 2014
Posts: 59
Rep Power: 9
tschenkel is on a distinguished road
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 is offline   Reply With Quote

Old   November 5, 2019, 14:20
Default
  #2
Member
 
Torsten Schenkel
Join Date: Jan 2014
Posts: 59
Rep Power: 9
tschenkel is on a distinguished road
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
tschenkel is offline   Reply With Quote

Old   November 7, 2019, 18:29
Default
  #3
Senior Member
 
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 18
Daniel_Khazaei will become famous soon enough
Quote:
Originally Posted by tschenkel View Post
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
Daniel_Khazaei is offline   Reply With Quote

Old   November 8, 2019, 06:57
Default
  #4
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 892
Rep Power: 29
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by tschenkel View Post
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
bigphil is offline   Reply With Quote

Old   November 8, 2019, 12:54
Default
  #5
Member
 
Torsten Schenkel
Join Date: Jan 2014
Posts: 59
Rep Power: 9
tschenkel is on a distinguished road
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 is offline   Reply With Quote

Old   November 21, 2019, 07:18
Default
  #6
Member
 
Torsten Schenkel
Join Date: Jan 2014
Posts: 59
Rep Power: 9
tschenkel is on a distinguished road
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"?
tschenkel is offline   Reply With Quote

Old   November 21, 2019, 07:27
Default
  #7
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 892
Rep Power: 29
bigphil will become famous soon enoughbigphil will become famous soon enough
Great.

Done.
bigphil is offline   Reply With Quote

Old   March 20, 2020, 18:43
Default
  #8
Member
 
Join Date: Jan 2019
Posts: 94
Blog Entries: 1
Rep Power: 4
Michael@UW is on a distinguished road
Quote:
Originally Posted by tschenkel View Post
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 is offline   Reply With Quote

Old   March 20, 2020, 19:03
Default
  #9
Member
 
Join Date: Jan 2019
Posts: 94
Blog Entries: 1
Rep Power: 4
Michael@UW is on a distinguished road
It seems the values on "solidTraction boundary" are written twice.
Here is the output of linearElastic3dTube/0.0001/solid/D:

Code:
/*--------------------------------*- 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 is offline   Reply With Quote

Old   March 20, 2020, 19:14
Default
  #10
Member
 
Join Date: Jan 2019
Posts: 94
Blog Entries: 1
Rep Power: 4
Michael@UW is on a distinguished road
fvPatchVectorField::write(os) does the work.

Code:
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
}

Last edited by Michael@UW; March 20, 2020 at 23:52.
Michael@UW is offline   Reply With Quote

Old   March 20, 2020, 19:25
Default
  #11
Member
 
Join Date: Jan 2019
Posts: 94
Blog Entries: 1
Rep Power: 4
Michael@UW is on a distinguished road
It worked after I recompiled the solids4Foam!
Michael@UW is offline   Reply With Quote

Old   March 23, 2020, 04:48
Default
  #12
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 892
Rep Power: 29
bigphil will become famous soon enoughbigphil will become famous soon enough
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
Daniel_Khazaei likes this.
bigphil is offline   Reply With Quote

Reply

Tags
solids4foam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[OpenFOAM] Paraview: .foam and .OpenFOAM files support redbullah ParaView 2 September 4, 2019 06:49
How can i read mesh files made with ICEM? I want use them for my own code zmester ANSYS Meshing & Geometry 9 October 11, 2009 07:18
Phase locked average in run time panara OpenFOAM 2 February 20, 2008 14:37
[General] Iblanked Plot3d files in Paraview Robert ParaView 0 September 27, 2006 15:45
Results saving in CFD hawk Main CFD Forum 16 July 21, 2005 20:51


All times are GMT -4. The time now is 15:02.