[Nagesh Atreyas]

Hello Dear Foamers,
I am a newbie to OpenFoam and would like to seek your help to solve an internal flow problem inside a valve.
Its a Steady state turbulent flow and I get the error after 6-8 iterations as quoted below while trying to solve with SimpleFoam.

Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#7 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#8 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#9 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#10
at simpleFoam.C:0
#11
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#12 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"

I hereby attach my fv solution, fv schemes and log files. Any help/guidance is much appreciated.

Thanks
Nagesh

[alexeym]

Hi,

could you post:

1. checkMesh output (using CODE tag or as an attachment)
2. your boundary conditions (maybe at archive of your 0 folder)

[Nagesh Atreyas]

Hi Alexey Matveichev...
Thanks for the reply.Here are my boundary conditions file. Will upload my checkMesh file in the following post.
I now realise that nut file wasn't needed for a K-epsilon model. But just want to clarify if it does any harm afterall?

Regards
Nagesh

[Nagesh Atreyas]

And here is the checkMesh file.

Thanks and regards
Nagesh

[Nagesh Atreyas]

My apologies.Due to a wrong epsilon value, I had got the error posted above.
Although I corrected it according to my problem, the error still persists and is as below.

Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#8
at simpleFoam.C:0
#9
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"

[alexeym]

Well, already at this point

Time = 19

smoothSolver:  Solving for Ux, Initial residual = 0.147683, Final residual = 0.00583124, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.320759, Final residual = 0.0176555, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 0.241805, Final residual = 0.00195216, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.370724, Final residual = 0.0175371, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.743256, Final residual = 0.0194592, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.133363, Final residual = 0.00447017, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.017872, Final residual = 0.00064358, No Iterations 3
time step continuity errors : sum local = 0.634471, global = 0.0016497, cumulative = 0.00164894
smoothSolver:  Solving for epsilon, Initial residual = 0.995526, Final residual = 0.047355, No Iterations 2
bounding epsilon, min: -2685.71 max: 645262 average: 31.6256
smoothSolver:  Solving for k, Initial residual = 0.999051, Final residual = 0.00853984, No Iterations 4
bounding k, min: -5137.77 max: 899607 average: 34.0357
ExecutionTime = 43.41 s  ClockTime = 44 s

it's more-or-less obvious, you've got problem with turbulence model. It can be due to mesh, ICs, or BCs.

How did you calculate IC and BC values for k and epsilon? You're using fixedValue BC for both, though maybe it's better to use turbulentIntensityKineticEnergyInlet and turbulentMixingLengthDissipationRateInlet with intensity and mixing length estimated from Re and hydraulic radius.

[Nagesh Atreyas]

Hello Alexy,
Thanks for your insight to my problem. I calculated the values for k and epsilon using the expressions which is herewith attached file.
I shall try out your suggestion and get back if the problem still persists.

Sorry if the attached file is of any inconvenience.

Thanks and regards
Nagesh

[Nagesh Atreyas]

Hello again,
As per your suggestions I made the changes accordingly.And I get quite a different error but at the same point of time. (27th iteration).
Vaguely I understand that it might be a problem with Mesh.
However I would like to know if mesh is the only problem or might there be problem with BC s and IC s again.

Here is the error. Kindly provide with your inputs.


#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 void Foam::multiply<Foam::Tensor<double> >(Foam::Field<Foam::Tensor<double> >&, Foam::UList<double> const&, Foam::UList<Foam::Tensor<double> > const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleTurbulenceModel.so"
#4 void Foam::multiply<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<Foam::Tensor<d ouble>, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleTurbulenceModel.so"
#5 Foam::tmp<Foam::GeometricField<Foam::Tensor<double >, Foam::fvPatchField, Foam::volMesh> > Foam:perator*<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::tmp<Foam::GeometricField<Foam::Tensor<double >, Foam::fvPatchField, Foam::volMesh> > const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleTurbulenceModel.so"
#6 Foam::incompressible::RASModels::kEpsilon::divDevR eff(Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>&) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libincompressibleRASModels.so"
#7
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#8 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"

[alexeym]

Hi,

for the future: it'll be more convenient, if you provide part of the log before the error.

As for the post, suggestions will be rather generic:

1. You've got non-hex cells in your mesh, use "leastSquares" instead of "Gauss linear" for gradSchemes

2. Set divSchemes to first-order upwind

3. Reduce relaxation factors for k and epsilon (let's say 0.3). Though if the problem is elsewhere this will just move FPE to later time.

4. Finally, if the problem persists, try moving from "corrected" schemes to "limited corrected 0.5".

[Nagesh Atreyas]

Hi,
Firstly thank you for your valuable inputs. Although they helped me to keep my solver running, I get worst results.
I hereby would like to know if its because of mesh/ICs BCs or could there still be problem with my fv schemes.
I have attached the log file herewith,the solver is still running,however results are very bad.
I have an inlet velocity of 5 m/s and at the end of 5th iteration,it shoots upto 36 m/s and the same with pressure as well.(above 500 at the end of 5th time step).
I am having a tough time with my little knowledge to dodge this problem.
Any inputs is highly appreciated.

[alexeym]

Well, dynamics of residuals looks quite promising, i.e. they are reducing during iterations.

Though if you plan to compare results of the simulation with experimental values (or just would like to get something meaningful), you should set convergence criterion for SIMPLE algorithm. Currently you've got none:

SIMPLE: no convergence criteria found. Calculations will run for 300 steps.

add residualControl dictionary to your SIMPLE dictionary in fvSolution, so it looks like:

SIMPLE
{
    nNonOrthogonalCorrectors 3;

    residualControl
    {
        "(p|k|epsilon)" 1e-6;
        Ux 1e-6;
        Uz 1e-6;
    }
}

maybe you don't need 1e-6, maybe 1e-4 will be enough.

[Nagesh Atreyas]

Aha yes.I thought the same about residuals as well. I have set up the convergence criterian now.
But I feel I might have gone wrong with the mixing length.Could you please tell me how to calculate mixing length?

[alexeym]

1. http://www.cfd-online.com/Wiki/Turbu...ary_conditions
2. http://www.cfd-online.com/Wiki/Turbulent_length_scale

Usually I use 7% of hydraulic radius.

[Nagesh Atreyas]

Thank you so much for all your suggestions.But for the fact that results seem to be too unrealistic,the solver works fine. Will work on it to get a satisfying result.

[Nagesh Atreyas]

Hello,
I had previously solved for one half of a Valve and now I am trying to analyse flow inside a Complete Valve.Unfortunately, I get the error which I had got earlier during Half-valve model.
Obviously I have changed BCs and ICs as per flow and model requirements and the other settings remaining the same as before.
It would be of great help for me if anyone could throw some light on where the problem lies.
Herewith I am attaching all the related files,which might be helpful.

Thanks
Nagesh

Solverlog.c

epsilon.c

k.c

U.c

p.c

[Nagesh Atreyas]

fvSchemes.cfvSolution.c

Oops, and this is the error msg that I get

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6 Foam::fvMatrix<double>::solveSegregated(Foam::dict ionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#8
at simpleFoam.C:0
#9
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"
#10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#11
in "/opt/openfoam222/platforms/linux64GccDPOpt/bin/simpleFoam"

[Tobi]

• Can you post some pictures of your mesh?

• Use uncorrected schemes for epsilon and k

• Further more, as suggested by alex, could you please use code tags

• Also post logfiles with error message: solver > log 2>&1

[Nagesh Atreyas]

Hi Tobi,
First of all thanks for the reply. And I am afraid I cant post the pictures due to confidentiality issues.However,I can look for it myself if you let me know what aspect to monitor.Was it because of snap layers( Morphing) warning?

You suggested me not to use smooth solver.May I know what I can use instead?

And sorry for the inconvenience with the error msges. I shall correct myself in the future posts.

Thanks and regards
Nagesh

[onetwothree]

Hello, Dear Nagesh Atreyas:
It seems that I came cross a problem similar to this one.
Could you share your way to solve this problem for me?
I am looking forward to your help. Thank you very much.

[Tobi]

We need more input to solve your question. Can you please share your logfile (stdout and stderr please).