[Jackie Chen]

Hi Foamers

I try to use OF 2.3.0 the tutorial file propeller to simulate the flow around tidal turbine.
When I try to type moveDynamicMesh-checkAMI
It shows

--> FOAM FATAL ERROR: 

    request for volVectorField U from objectRegistry region0 failed
    available objects of type volVectorField are
0()

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField,  Foam::volMesh> const&  Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>,  Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const  in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libdynamicFvMesh.so"
#3  Foam::Q::execute() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libutilityFunctionObjects.so"
#4   Foam::OutputFilterFunctionObject<Foam::Q>::execute(bool) in  "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libutilityFunctionObjects.so"
#5  Foam::functionObjectList::execute(bool) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6  Foam::Time::run() const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7  Foam::Time::loop() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/moveDynamicMesh"
#9  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/moveDynamicMesh"
Aborted (core dumped)

ANyone can figure out this? Thanks in advance

[wyldckat]

Quick answer: The "U" field is not loaded automatically when using the mesh-only solver moveDynamicMesh. You can try using the function object "readFields" to forcefully load the "U" file: http://openfoamwiki.net/index.php/Ti...loading_fields - section "3.3 Force loading fields"

[Jackie Chen]

Hi Bruno Santos

Thanks for you reprly. However, my of is 2.3.0. and the readfield is a separate file under system.The error remains.

[wyldckat]

Hi Jackie Chen,

Sorry for the late reply, but I finally managed to give a quick look into this.

The tutorial "incompressible/pimpleDyMFoam/propeller" has in its "system/controlDict" these lines:

functions
{
    #include "readFields"
    #include "Q"
    #include "surfaces"
    #include "forces"
}

Which means it already does what I said it would do.
I looked better into the error output you got and it states that it was in fact the "Q" utility function that crashed.

In addition, the script "Allrun.pre" has these lines near the end:

# - create the inlet/outlet and AMI patches
runApplication createPatch -overwrite

# - test by running moveDynamicMes
#runApplication moveDynamicMesh -checkAMI

# - set the initial fields
cp -rf 0.org 0

Which I now understand why you're asking this question and why you got this crash.

It takes too long to generate this mesh in my machine, so I haven't tried this yet, but my suggestion is that you place the call for moveDynamicMesh to after the copy is made, namely:

# - create the inlet/outlet and AMI patches
runApplication createPatch -overwrite

# - set the initial fields
cp -rf 0.org 0

# - test by running moveDynamicMesh
runApplication moveDynamicMesh -checkAMI

This way the "U" file is now present in the folder "0", so that the "readFields" function object will now be able to load the field "U" and the "Q" function object will then be able to use the "U" field.

-----------------

edit: OK, the mesh is now finished generating and I still got the same crash. I managed to get it working if I comment out the line for "Q" in "system/controlDict", namely:

functions
{
    #include "readFields"
//    #include "Q"
    #include "surfaces"
    #include "forces"
}

Best regards,
Bruno

[WernerW]

Hi Bruno,

Thanks for your help, I commented the line for Q and the program seemed to work for the first 10 timesteps (0.1 to 1) but crashed at 1 , at the first writing time with this error:

--> FOAM FATAL ERROR:
Cannot find isosurface field Q in database or directory "/home/werner/OpenFOAM/werner-2.4.0/run/WindTurbine-DyM1/1"

From function sampledIsoSurface::getIsoFields()
in file sampledSurface/isoSurface/sampledIsoSurface.C at line 113.

FOAM exiting

Meanwhile, OpenFOAM created a folder in my case directory called 1

werner@werner-K45VD:~/OpenFOAM/werner-2.4.0/run/WindTurbine-DyM1/1$ tree
.
├── polyMesh
│** └── points
└── uniform
└── time

2 directories, 2 files

Have you got this error?

regards,
Werner

[wyldckat]

Quick answer: You will have to comment out the "surfaces" entry as well:

functions
{
    #include "readFields"
//    #include "Q"
//    #include "surfaces"
    #include "forces"
}

[WernerW]

Thank you Bruno !

Once more that made it work Could you explain what we disabled there disabling Q and Surfaces ?

In each step I could read "Did not find volVectorField U Not updating Uboundary conditions." Is there any way of solving this ?

I think that solving this would be useful becuase when I run the application pimpleDyMFoam a get a floating point exception related to division by 0 in the process of reading speed U. I paste here the error ...

I apreciate very much your help

werner@werner-K45VD:~/OpenFOAM/werner-2.4.0/run/WindTurbine-DyM1$ pimpleDyMFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-dcea1e13ff76
Exec : pimpleDyMFoam
Date : Aug 13 2015
Time : 11:48:49
Host : "werner-K45VD"
PID : 5224
Case : /home/werner/OpenFOAM/werner-2.4.0/run/WindTurbine-DyM1
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function rotatingMotion
Applying solid body motion to cellZone Cylinder

PIMPLE: no residual control data found. Calculations will employ 2 corrector loops

Reading field p

AMI: Creating addressing and weights between 9005 source faces and 8959 target faces
AMI: Patch source sum(weights) min/max/average = 0.254862, 1.1706, 0.995708
AMI: Patch target sum(weights) min/max/average = 0.797915, 1.49352, 1.011
Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}

Reading/calculating face velocity Uf

No finite volume options present

Courant Number mean: 0.023476 max: 0.977293
forces forces:
Not including porosity effects


Starting time loop

Courant Number mean: 0.023476 max: 0.977293
deltaT = 0.111111
Time = 0.111111

solidBodyMotionFunctions::rotatingMotion::transfor mation(): Time = 0.111111 transformation: ((0 0 0) (-0.797896 (0.602796 0 0)))
AMI: Creating addressing and weights between 9005 source faces and 8959 target faces
AMI: Patch source sum(weights) min/max/average = 0, 1.30674, 0.993375
AMI: Patch target sum(weights) min/max/average = 0, 1.49861, 1.00718
PIMPLE: iteration 1
#0 Foam::error:rintStack(Foam::Ostream&) at ~/OpenFOAM/openfoam240/src/OSspecific/POSIX/printStack.C:219
#1 Foam::sigFpe::sigHandler(int) at ~/OpenFOAM/openfoam240/src/OSspecific/POSIX/signals/sigFpe.C:108
#2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ~/OpenFOAM/openfoam240/src/OpenFOAM/fields/Fields/scalarField/scalarField.C:116 (discriminator 2)
#4 void Foam::divide<Foam::fvPatchField>(Foam::FieldField< Foam::fvPatchField, double>&, double const&, Foam::FieldField<Foam::fvPatchField, double> const&) at ~/OpenFOAM/openfoam240/src/OpenFOAM/lnInclude/scalarFieldField.C:91 (discriminator 2)
#5 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::dimensioned<double> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ~/OpenFOAM/openfoam240/src/OpenFOAM/lnInclude/GeometricScalarField.C:116
#6 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::dimensioned<double> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ~/OpenFOAM/openfoam240/src/OpenFOAM/lnInclude/GeometricScalarField.C:116 (discriminator 1)
#7 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(double const&, Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ~/OpenFOAM/openfoam240/src/OpenFOAM/lnInclude/GeometricScalarField.C:116 (discriminator 1)
#8 ? at ~/OpenFOAM/openfoam240/applications/solvers/incompressible/pimpleFoam/pimpleDyMFoam/../UEqn.H:16 (discriminator 2)
#9 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#10 ? at ??:?
Floating point exception (core dumped)

[wyldckat]

Quick answer:

1. The problem with pimpleDyMFoam occurs at 0.1111..., after rotating I don't know how many degrees... is it something like 90 degrees? If so, that's waaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaaay too much
2. moveDynamicMesh is usually used for helping with diagnosing mesh excessive distortions that may occur with some transformations. It's a lot faster to use this than to use the solver. Therefore, running moveDynamicMesh without the function objects is only worth while for looking at the mesh for each time snapshot. Furthermore, I would suggest saving all time instances, so that you can look at exactly the mesh distortions that the solver will be looking at.

[WernerW]

Hi Bruno,

1. Ok! yeah, you're right , with a speed of 158 rad/s the turbine rotated 90 degrees between each step. Now I set the deltaT to 0.001 for 9 degrees between each step, is that fine. I'm still getting the FPE (Floating point exception). Do you know a current post where I can get further advise for this issue ?
2. In that sense should we enable Q and Surfaces to get the full results when we run the solver ?

[wyldckat]

Quick answers:

Originally Posted by WernerW

1. Ok! yeah, you're right , with a speed of 158 rad/s the turbine rotated 90 degrees between each step. Now I set the deltaT to 0.001 for 9 degrees between each step, is that fine. I'm still getting the FPE (Floating point exception). Do you know a current post where I can get further advise for this issue ?

9 degrees is still too much. You should do a quick study with a simple geometry, for diagnosing what can and can't be done. If you jump directly into trying to solve your final geometry/case, it will take you considerably a lot longer to solve all of the problems you will likely face.

I can't remember any specific threads on this topic.

Originally Posted by WernerW

2. In that sense should we enable Q and Surfaces to get the full results when we run the solver ?

I believe those two entries are mostly demonstrations of features that OpenFOAM provides for co-processing which the solver is running, i.e. post-processing on-the-fly.

[WernerW]

Hi Bruno,

I set deltaT to 1e-5 , as it was in the propeller tutorial, and the issue was solved :P Thanks a lot once more