[fusij]

Hello,

When I try to obtain the modelled Reynolds Stress tensor by using the R utility I get the following message

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

Create mesh for time = 0

Time = 0
Reading field U

Reading/calculating face flux field phi

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

Writing R field


--> FOAM FATAL ERROR: 
object of type N4Foam9DataEntryINS_10SymmTensorIdEEEE is not allocated

    From function Foam::autoPtr<T>::operator->()
    in file /home/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/autoPtrI.H at line 176.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::timeVaryingMappedFixedValueFvPatchField<Foam::SymmTensor<double> >::write(Foam::Ostream&) const at ??:?
#3  Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::writeEntry(Foam::word const&, Foam::Ostream&) const at ??:?
#4  Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>::writeData(Foam::Ostream&) const at ??:?
#5  Foam::regIOobject::writeObject(Foam::IOstream::streamFormat, Foam::IOstream::versionNumber, Foam::IOstream::compressionType) const at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 at ??:?
Aborted (core dumped)

This is a 3D simulation. I have tested the utility on another case were I was using the standard k-epsilon model and wall functions accordingly and it worked fine there.

In particular, does anybody know what this means: object of type N4Foam9DataEntryINS_10SymmTensorIdEEEE is not allocated

The R tensor is defined in LaunderSharmaKE.C

[lifeinhand]

I had the same issue. Anyone know the reason?

[alexeym]

Hi,

Though it would be great to have test case with the error, let's try to deduce the reason from backtrace.

Error happened in

Foam::timeVaryingMappedFixedValueFvPatchField<Foam::SymmTensor<double> >::write

Do you have timeVaryingMappedFixedValue boundary condition for TKE (since R tensor uses the same BCs)?

Technically the reason for the error is this part of timeVaryingMappedFixedValueFvPatchField.C (since offset_ is the only property of DataEntry type):

template<class Type>
void timeVaryingMappedFixedValueFvPatchField<Type>::write(Ostream& os) const
{
...
    offset_->writeData(os);
...
}

For some reason offset_ if not initialized properly. So you could submit bug-report using Mantis. Or, since you are using version 2.3.x, enclose the expression into autoPtr validity check:

if (offset_.valid())
{
    offset_->writeData(os);
}

recompile finiteVolume library, check if it helps, and submit a patch.

[lifeinhand]

According to the manager of Bug report website, the timeVaryingMappedFixedValue boundary condition could not use R utility.

"There is no automatic way to convert the timeVaryingMappedFixedValue BC for k into the equivalent for R. It would be possible to simply evaluate R for the current state of all the BCs and output them all as type "calculated" which would be OK for post-processing but not for changing from say a k-epsilon to an R-epsilon turbulence model."

I tried this, it worked. Since I am doing steady state now, it is fine. But for transient problem it seems a little bit trouble to change every time step.

[fusij]

Could you explain to me in little more detail what you did to export the R stress tensor? I thought it was only a postprocessing utility explicitly calculating Reynolds stresses using my eddy viscosity and velocity gradients. Why is the problem related to timeVaryingMappedFixedValue?

[lifeinhand]

Yes, R is only a postprocessing utility. However, based on my understanding, R utility is not compatible with boundary condition "timeVaryingMappedFixedValue". So, what I did was after my calculation is done, I modify the file of the time step that I am going to postprocess, e.g. 1000, I change the U and other vaiables that was "timeVaryingMappedFixedValue" to "calculated". Then R utility will be able to to the job.

[fusij]

Ahh OK, I get it. Thanks for that info. But I am still little bit confused why it is not working for timeVaryingMappedFixedValue since all variables are known for computing the R tensor

[lifeinhand]

I guess it is some bug in the utility or the boundary condition, but I am not capable to find out and fix. :P

[alekhine]

Hey Han Li,
I have now the same issue and cannot make it work. I changed

inlet
{
type timeVaryingMappedFixedValue;
setAverage 0;
offset constant 0;
value nonuniform List<scalar>

to

inlet
{
type calculated;
value nonuniform List<scalar>

but it doesn't work. Can you tell me what you changed in detail please?

UPDATE: I use the kOmegaSST model and adding the k,omega and U files enables the calculation of the Reynolds stress.
Thank you so much for providing the solution!!

Dimitri

[lifeinhand]

Did you change to calculated to all files?

All I did is replace the string "timeVaryingMappedFixedValue" to "calculated" for all variables. For my case U, epsilon and k.

Also, the version I used is OpenFOAM 2.4

[alekhine]

I did the same as you mention, changing only U, epsilon and k to calculated and deleted the setAverage and the offset lines. The delete of the setAverage and offset lines shouldn't make a difference since there are not taken into account by the type calculated, I believe.

Thanks again, you saved me!! :-)

[AhmedSamy]

I am sure the solution to janaf temperature problem is in the mesh. A structured simple mesh using only scripting is the only solution.

I have prepared this procedure to get a good mesh. After gmshtofoam just prepare the bondary file to fit and run checkfoam. Pls check the attached file!