[CFDUser_]

Hi All,
Hope everyone is good.
I got the following error while running sprayFoam for kOmegaSST turbulent model.

--> FOAM FATAL ERROR: 

    lookup of turbulenceModel from objectRegistry region0 successful
    but it is not a turbulenceModel, it is a kOmegaSST

    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 181.

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::incompressible::turbulenceModel const& Foam::objectRegistry::lookupObject<Foam::incompressible::turbulenceModel>(Foam::word const&) const in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/liblagrangianTurbulence.so"
#3  Foam::incompressible::omegaWallFunctionFvPatchScalarField::updateCoeffs() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#4  Foam::compressible::RASModels::kOmegaSST::correct() in "/opt/openfoam230/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so"
#5  

#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  

Aborted (core dumped)

Its weird but ya its true. it is saying kOmegaSST is not turbulent model.
Still unable to figure out how to correct it. It is failing to register RASModel (run time constructor for RASModel). I know that PISO is most generic for turbulence models in OpenFOAM and sprayFoam is derived from PISO. So, problem should be some where else (I mean not in constructing RASModel). I am unable to figure it out. Can some body help me?

All I have done to get this error Is replaced aachenBomb geometry with simple square duct then specified proper BCs to run flow problem. Worked well with kEpsilon. Then changed turbulence model to kOmegaSST.

Regards,
CFDUser_

[tomf]

Could you provide the turbulenceProperties and RASProperties files you used? I am guessing from your information something is incorrectly set there. Regards, Tom

[CFDUser_]

Originally Posted by tomf

Could you provide the turbulenceProperties and RASProperties files you used? I am guessing from your information something is incorrectly set there. Regards, Tom

Hi Tom,

Thanks for the reply.
Details you asked are furnished below
RASProperties:
RASModel kOmegaSST;
turbulence on;
printCoeffs on;

turbulenceproperties:
simulationType RASModel;


Regards,
CFDUser_

[tomf]

Maybe there is something in the header above this information that is incorrectly set? So could you just output the entire file contents?

Otherwise it may be a bug in version 2.3.0?

I just changed the turbulence model to kOmegaSST in the copied aachenBomb tutorial for 2.3.x.

It runs fine and is attached:

simply do:

$> blockMesh
$> sprayFoam

Just copied epsilon to omega and kept the values, so maybe it is incorrect, but it runs at least.

[CFDUser_]

Originally Posted by tomf

Maybe there is something in the header above this information that is incorrectly set? So could you just output the entire file contents?

Otherwise it may be a bug in version 2.3.0?

I just changed the turbulence model to kOmegaSST in the copied aachenBomb tutorial for 2.3.x.

It runs fine and is attached:

simply do:

$> blockMesh
$> sprayFoam

Just copied epsilon to omega and kept the values, so maybe it is incorrect, but it runs at least.

I did this already and succeed. problem arrived when tried to change the case to flow problem.
Why don't you change your case to simple flow problem(floe through simple square duct may be) and try the same.

Regards,
CFDUser_

[tomf]

I will not have that amount of time available at the moment I am afraid, maybe some one else has. Probably best if you can provide the case that is troubling you so someone can have a look at it. We do not know what you have in front of you exactly.

[CFDUser_]

Originally Posted by tomf

I will not have that amount of time available at the moment I am afraid, maybe some one else has. Probably best if you can provide the case that is troubling you so someone can have a look at it. We do not know what you have in front of you exactly.

Dear Tom,

Thanks for your support. There was no bug. I gave wrong input for omega.
Now its working.

Thanks a lot.

Regards,
CFDUser_

[appie]

Originally Posted by CFDUser_

Dear Tom,

Thanks for your support. There was no bug. I gave wrong input for omega.
Now its working.

Thanks a lot.

Regards,
CFDUser_

Dear CFDUser,

I'd be interested to know how you saw that the input for omega was incorrect?

And what did you change to solve it?

I'm encountering the same error...

Many thanks in advance!

[CFDUser_]

Originally Posted by appie

Dear CFDUser,

I'd be interested to know how you saw that the input for omega was incorrect?

And what did you change to solve it?

I'm encountering the same error...

Many thanks in advance!

Are you solving for compressible flow and your omega type is just omegaWallFunction??

just change type to compressible:megaWallFunction in omega file.

Your are done.

Regards,
CFDUser_

[appie]

Wow, thanks for the quick reply.

It's a bit different. I'm changing my case from a compressible solver to an incompressible. I'm not sure where the error originates, but I make it till here:

DILUPBiCG: Solving for Ux, Initial residual = 0.999999999998, Final residual = 2.60220350182e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 0.999999999987, Final residual = 3.46113359058e-08, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.999999999999, Final residual = 3.1130707825e-08, No Iterations 4
DILUPBiCG: Solving for H2O, Initial residual = 0.999999891847, Final residual = 5.29106562959e-09, No Iterations 3
DILUPBiCG: Solving for CO2, Initial residual = 5.87534515923e-05, Final residual = 5.55965647659e-08, No Iterations 1


--> FOAM FATAL ERROR:

lookup of turbulenceModel from objectRegistry region0 successful
but it is not a turbulenceModel, it is a realizableKE


The enthalpy(h) is the next equation to be solved, so I would think T so be the source of error. I switched the B.C. between compressible::turbulentHeatFluxTemperature and turbulentHeatFluxTemperature.

I'll continue battling this error, and get be to be more clear...

Regards,

Appie

[CFDUser_]

Originally Posted by appie

Wow, thanks for the quick reply.

It's a bit different. I'm changing my case from a compressible solver to an incompressible. I'm not sure where the error originates, but I make it till here:

DILUPBiCG: Solving for Ux, Initial residual = 0.999999999998, Final residual = 2.60220350182e-08, No Iterations 4
DILUPBiCG: Solving for Uy, Initial residual = 0.999999999987, Final residual = 3.46113359058e-08, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.999999999999, Final residual = 3.1130707825e-08, No Iterations 4
DILUPBiCG: Solving for H2O, Initial residual = 0.999999891847, Final residual = 5.29106562959e-09, No Iterations 3
DILUPBiCG: Solving for CO2, Initial residual = 5.87534515923e-05, Final residual = 5.55965647659e-08, No Iterations 1


--> FOAM FATAL ERROR:

lookup of turbulenceModel from objectRegistry region0 successful
but it is not a turbulenceModel, it is a realizableKE


The enthalpy(h) is the next equation to be solved, so I would think T so be the source of error. I switched the B.C. between compressible::turbulentHeatFluxTemperature and turbulentHeatFluxTemperature.

I'll continue battling this error, and get be to be more clear...

Regards,

Appie

Check all your bc's. May be you are specifying some other field as compressible.


CFDUser_

[appie]

Thanks, you were right. Thanks for the help!

I had wallHeatTransfer instead of incompessibleWallHeatTransfer..

[jairoandres]

Dear Foamers... I am having a similar issue than CFDUSER___ I replaced the AachenBomb tutorial with a modified spray (that I already tested), and finally I added flow with the proper boundary conditions... However i am having an error I havent figured.... It comes after calculating the first step for most variables (after rho), I have read of bugs with sprayfoam and kepsilon but i've read that this worked for CFDUSER .... Can i have any guess of the issue on this??
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.99435e-09, global = -1.24757e-09, cumulative = -3.71235e-05
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 void Foam::divide<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&) at ??:?
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > Foam:perator/<Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > const&) at ??:?
#6 Foam::compressible::RASModels::kEpsilon::correct() at ??:?
#7
at ??:?
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
at ??:?
Floating point exception (core dumped)

[lramutti]

Division by zero. Somewhere in your 0 or systems folder - depending what solver you are using (i.e. conjugate heat transfer) - has a zero value boundary/ initial condition. Might be worth it to take a look.

Cheers

-Lucas

[jairoandres]

Thanks for your answer... I figured the same, however I wouldnt expect any issues since I replaced Aachenbomb and added inlet and oulet boundaries...After giving it a big though I think I know where is this heading into... sprayFoam.c says it handles energy instead of temperature as a transport equation. Since there were no inlets / outlets of energy in Aachenbomb as boundary conditions I guess they didnt use an EEqn.h (because it was not necessary). However if I add flow, the flow has enthalpy on it and it becomes a source in time=0, and maybe this is creating the error. I will check everything then add this and will tell you... Thanks again

[lramutti]

Now that you mentioned I recall that I had a similar problem. In order for you to run the SST k omega model you must define some parameters. If I remember correctly the equation considers the division of a factor which I believe it is labeled as B while calculating the F or F-max values. Might be worth it to confirm what values those parameters take and check if this solves the problem. If its set as 0 just make them infinitesimally small.

Hope that helps

Lucas

[jairoandres]

Ok it worked for me at last.... Thank you all... some advice for the new guys...

1) Sprayfoam looks to be only a compressible flow solver. one of the errors i had was because i changed the wall functions to incompressible.

2) I was used to set pressure outlet to 0 in the boundary for 0-p. But of course since solver is compressible this will get a big error..

3) Something logical, but sometimes u dont see it because i was migrating from simplefoam... use mut instead of nut. Otherwise you will have dimensional problems.

[StefanosTrat]

hello foamers, kinda similar problem here , cant understand it because in cumbustion properties i have set the model PaSR

--> FOAM FATAL ERROR:
[3]
lookup of combustionProperties from objectRegistry region0 successful
but it is not a CombustionModel<rhoReactionThermo>, it is a PaSR<psiReactionThermo>
[3]
[3] From function const Type& Foam:bjectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::combustionModels::singleStepCombustion<Foam: :rhoReactionThermo, Foam::sutherlandTransport<Foam::species::thermo<Fo am::janafThermo<Foam:erfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > >]