[PHabib]

Hello everyone,

I'm getting an error using reconstructPar. The decomposing works without problems, but reconstructing the volVectorField U leads to an error. I am using OF 2.3 and the Boundary condition "externalCoupled" for U.
Does anyone now how to handle this error? any help will be much appreciated.
Here is the error output:

command:

reconstructPar -fields '(U)'

Create time



Reconstructing fields for mesh region0

Time = 0.0001

Reconstructing FV fields

    Reconstructing volScalarFields


    Reconstructing volVectorFields

        U
externalCoupled: removing lock file
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigSegv::sigHandler(int) in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::externalCoupledMixedFvPatchField<Foam::Vector<double> >::baseDir() const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::externalCoupledMixedFvPatchField<Foam::Vector<double> >::removeLockFile() const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::externalCoupledMixedFvPatchField<Foam::Vector<double> >::~externalCoupledMixedFvPatchField() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6  Foam::externalCoupledMixedFvPatchField<Foam::Vector<double> >::~externalCoupledMixedFvPatchField() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/reconstructPar"
#8  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/reconstructPar"
#9  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/reconstructPar"
#10  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/reconstructPar"
#11  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12  
 in "/opt/openfoam230/platforms/linux64GccDPOpt/bin/reconstructPar"
Segmentation fault (core dumped)

[Dozer_94]

Hi there,

I'm sorry, I don't have an answer to your problem. I am interested however in how you wrote your data input file for the externalCoupled boundary condition for the velocity.

I know that for a scalar field like Temperature it should look like this:

<value1> <gradient1> <valueFraction1>

Could you show me what format is to be used for a vector field like Velocity? I have had no luck digging through the source code...

[Gerry Kan]

Dozer:

Here is the supposed format for externalCoupled for velocities, also by PHabib (response #4).

VectorSpace cmpt

Hope this helps, Gerry.

[Dozer_94]

Gerry,

Great, thanks! Don't know why I couldn't find this thread.

[Gerry Kan]

Hallo PHabib:

I don't know if you have solved the problem already. I encountered the same problem with externalCoupled as well.

Upon looking into the offending function

template<class Type>
Foam::externalCoupledMixedFvPatchField<Type>::
~externalCoupledMixedFvPatchField()
{    removeLockFile();    }

and the corresponding function it calls

template<class Type>
void Foam::externalCoupledMixedFvPatchField<Type>::removeLockFile() const
{
    if (!master_ || !Pstream::master())
    {    return;    }

    if (log_)
    {    Info<< type() << ": removing lock file" << endl;    }

    rm(lockFile());
}

I realize it is asking the head node to remove the lock file.

In my case I modified the the externalCoupled BC so that the lock file never gets created, and the same error you had with reconstructPar appeared. The call to removeLockFile() was then commented out from the destructor and reconstructPar worked fine again.

It could be that the file OpenFOAM.lock was removed between the end of your run and calling reconstructPar. If this is true, the solution would either be preventing this file from being erased, or recreating it prior to calling reconstructPar.

Let me know if you have solved your problem, and how, if your solution is different.

Gerry.