[kalyan]

Hi all,

i am trying to simulate a multiphase euler-lagrangian case with assumption of incompressible flow. so i created a solver by merging pimpleFoam and icoUncoupledKinematicFoam. The solver is running fine. But my case it is running fine till certain time and is suddenly blowing up.


There is sudden increase in LineaMomentum of Particles.. Any help is greatly appreciated

Courant Number mean: 0.04043413 max: 0.4999354
deltaT = 4.509583e-06
Time = 0.148758

smoothSolver:  Solving for Ux, Initial residual = 1.557579e-05, Final residual = 7.167363e-07, No Iterations 1
smoothSolver:  Solving for Uy, Initial residual = 0.0001077576, Final residual = 4.33946e-06, No Iterations 1
smoothSolver:  Solving for Uz, Initial residual = 1.515668e-05, Final residual = 7.043948e-07, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.01890968, Final residual = 0.0007671708, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0007673827, Final residual = 6.345403e-05, No Iterations 3
time step continuity errors : sum local = 2.1412e-09, global = -4.2204e-10, cumulative = -1.454082e-07
GAMG:  Solving for p, Initial residual = 0.001474408, Final residual = 0.0001064657, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.0001064498, Final residual = 8.128193e-07, No Iterations 8
time step continuity errors : sum local = 2.742942e-11, global = -8.07545e-12, cumulative = -1.454163e-07
smoothSolver:  Solving for omega, Initial residual = 8.999363e-06, Final residual = 8.999363e-06, No Iterations 0
smoothSolver:  Solving for k, Initial residual = 1.068478e-05, Final residual = 6.815941e-07, No Iterations 1
bounding k, min: 1e-20 max: 19.51322 average: 7.276739
Evolving kinematicCloud

Solving 3-D cloud kinematicCloud
Cloud: kinematicCloud
    Current number of parcels       = 8184
    Current mass in system          = 3.82134e-05
    Linear momentum                 = (4.013661e-05 -0.0002115916 -3.440463e-05)
   |Linear momentum|                = 0.0002180955
    Linear kinetic energy           = 0.2790673
    model1:
        number of parcels added     = 12085
        mass introduced             = 5.646226e-05
    Parcels absorbed into film      = 0
    New film detached parcels       = 0
    Parcel fate (number, mass)      : patch fixedWalls
      - escape                      = 0, 0
      - stick                       = 3191, 1.489793e-05
    Parcel fate (number, mass)      : patch upperWall
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch sideWalls
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch outlet
      - escape                      = 3901, 1.824887e-05
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch baffleFaces_master
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch baffleFaces_slave
      - escape                      = 0, 0
      - stick                       = 0, 0
    Rotational kinetic energy       = 0

ExecutionTime = 94879.29 s  ClockTime = 97483 s

Courant Number mean: 0.04043416 max: 0.4999354
deltaT = 4.509583e-06
Time = 0.148762

smoothSolver:  Solving for Ux, Initial residual = 0.008377172, Final residual = 5.821064e-06, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.006608096, Final residual = 5.01418e-06, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 0.006809619, Final residual = 4.746882e-06, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.9900283, Final residual = 0.06366995, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.03142656, Final residual = 0.002906337, No Iterations 6
time step continuity errors : sum local = 1.959254e-05, global = -5.515908e-06, cumulative = -5.661324e-06
GAMG:  Solving for p, Initial residual = 0.0770012, Final residual = 0.006030893, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.006325515, Final residual = 7.318672e-07, No Iterations 22
time step continuity errors : sum local = 4.418537e-09, global = -4.954527e-10, cumulative = -5.66182e-06
smoothSolver:  Solving for omega, Initial residual = 0.01988505, Final residual = 6.423435e-06, No Iterations 10
smoothSolver:  Solving for k, Initial residual = 0.006081979, Final residual = 7.021702e-06, No Iterations 3
bounding k, min: 1e-20 max: 38.73186 average: 7.280719
Evolving kinematicCloud

Solving 3-D cloud kinematicCloud
Cloud: kinematicCloud
    Current number of parcels       = 8184
    Current mass in system          = 3.82134e-05
    Linear momentum                 = (-1.563558e+136 -3.405907e+135 1.572105e+136)
   |Linear momentum|                = 2.243263e+136
    Linear kinetic energy           = 4.816419e+280
    model1:
        number of parcels added     = 12085
        mass introduced             = 5.646226e-05
    Parcels absorbed into film      = 0
    New film detached parcels       = 0
    Parcel fate (number, mass)      : patch fixedWalls
      - escape                      = 0, 0
      - stick                       = 3191, 1.489793e-05
    Parcel fate (number, mass)      : patch upperWall
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch sideWalls
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch outlet
      - escape                      = 3901, 1.824887e-05
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch baffleFaces_master
      - escape                      = 0, 0
      - stick                       = 0, 0
    Parcel fate (number, mass)      : patch baffleFaces_slave
      - escape                      = 0, 0
      - stick                       = 0, 0
    Rotational kinetic energy       = 0

ExecutionTime = 94884.24 s  ClockTime = 97489 s

Courant Number mean: 0.0425952 max: 12617.33
deltaT = 1.78706e-10
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1055
    Increased the timePrecision from 6 to 7 to distinguish between timeNames at time 0.1487621
Time = 0.1487621

smoothSolver:  Solving for Ux, Initial residual = 1, Final residual = 2.382181e-08, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 2.382181e-08, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 1, Final residual = 2.382181e-08, No Iterations 2
[0] [1] #0  Foam::error::printStack(Foam::Ostream&)#[3] #0  Foam::error::printStack(Foam::Ostream&)0  Foam::error::printStack(Foam::Ostream&) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1  Foam::sigFpe::sigHandler(int) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1  Foam::sigFpe::sigHandler(int) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1  Foam::sigFpe::sigHandler(int) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2   in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #2   in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #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 "/lib/x86_64-linux-gnu/libc.so.6"
[1] #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 "/lib/x86_64-linux-gnu/libc.so.6"
[0] #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 "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #4  Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64Gc in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #6  cDPOpt/lib/libOpenFOAM.so"
[0] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&)Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[0] #7   in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[1] #7   in "/root/OpenFOAM/OpenFOAM-2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
[3] #7  


[3]  in "/root/OpenFOAM/root-2.3.x/platforms/linux64GccDPOpt/bin/pimpleKinematicFoam"
[3] #8  __libc_start_main[0]  in "/root/OpenFOAM/root-2.3.x/platforms/linux64GccDPOpt/bin/pimpleKinematicFoam"
[0] #8  __libc_start_main[1]  in "/root/OpenFOAM/root-2.3.x/platforms/linux64GccDPOpt/bin/pimpleKinematicFoam"
[1] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #9   in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #9  
 in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #9  
[3]  in "/root/OpenFOAM/root-2.3.x/platforms/linux64GccDPOpt/bin/pimpleKinematicFoam"

caseFIles.tar.gz

[kalyan]

I have also attached the importatn case files.. please refer to it. caseFIles.tar.gz

[wyldckat]

Greetings kalyan,

I'm answering you here because you sent me a PM asking to look into this.
Sorry, but I don't have the time to test the case, specially if the case takes 95000 seconds to run before it crashes. You will have to diagnose this on your side.

My guess is that perhaps you're using "cyclicAMI" for the baffles, which has issues in OpenFOAM, up to and including 2.4.
The other possibility seems related to a problem in preserving the stability of the flow... did you try to run the case without particles? Because the error is related to this:

Courant Number mean: 0.04043416 max: 0.4999354
deltaT = 4.509583e-06
Time = 0.148762

smoothSolver:  Solving for Ux, Initial residual = 0.008377172, Final residual = 5.821064e-06, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.006608096, Final residual = 5.01418e-06, No Iterations 2
smoothSolver:  Solving for Uz, Initial residual = 0.006809619, Final residual = 4.746882e-06, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.9900283, Final residual = 0.06366995, No Iterations 3

The initial residual for "p" increased drastically. You will have to look at the results in the case in detail for diagnosing where the problem is located. On this blog post of mine you can find several examples on how to diagnose cases: http://www.cfd-online.com/Forums/blo...onditions.html

Best regards,
Bruno

[kalyan]

Greetings Bruno,

Thank you for the reply. The simulation is running fine when the case is simulated without particles. The simulation crashes only when particles are added. I dont know what the error is.


Regards,
kalyan

[vonboett]

could you try with coupled false; in your kinematciCloudProperties? Did you merge the two solvers using kinematicCloud or kinematicCollidingCloud? I am asking because I guess that your particle-particle or particle-wall contact force goes to infinity. Maybe you could increase the diameter or vary e to make the contact softer.

[kalyan]

Hello albrecht,

Thank you for the reply. I merged both the solvers using basicKinematicCollidingCloud. Does the coupled true; in the kinematicCloudProperties mean coupling between particles and continuous phase(2-way coupling)? or particle-particle interaction (4-way coupling)?
I would try simulating with couple false; and will update the result. Thank you.

Regards,
Kalyan

[vonboett]

Hi Kalyan,
As the name says icoUncoupledKinematicFoam is not coupling between the phase flow and the particle, it is for simulating tracers that yust follow the flow. The velocity field of your pimple calculation is yust mapped onto the particles. However, particle-wall and particle-particle interaction is possible. If you want to do the 4-way coupling it gets more complex: Especially if you have more particles, you need to account for the volume fraction of your fluid in the navier-stokes equation. But as long as your particle concentration is less that some 80% you may get a stable solver (although not really correct) with neglecting the volume fraction. But still you need to implement the drag that particles put on your fluid in the UEqn.H with something like

tmp<fvVectorMatrix> UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
+ turbulence->divDevReff(U)
==
fvOptions(U)
+invrhoInf*kinematicCloud.SU(U)
);

see:http://www.tfd.chalmers.se/~hani/kur...ing_report.pdf

or



solve
(
UEqn
==
fvc::reconstruct
(
(
fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1) //surface tension
- ghf*fvc::snGrad(rho)
- fvc::snGrad(p_rgh)
) * mesh.magSf()

)
+ particles.momentumSource()
);

see http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf

or even more sophisticated but for two phase flow: HPDCInterFoam

[kalyan]

Hi Albrecht,

The simulation ran well with out error when i changed coupled false; in the kinematicCloudProperties. I Have used the below code for UEqn to merge pimple and icoUnCoupledKinematicParcelFoam

tmp<fvVectorMatrix> UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
+ turbulence->divDevReff(U)
==
fvOptions(U)
+invrhoInf*kinematicCloud.SU(U)
);

will recompile the solver using kinematicCloud instead of kinematicCollingCloud, and will check the simulation with coupled ture, in kinematicCloud.


Regards,
kalyan

[szamani]

Hi,
I am new to using openfoam lagrangian models. I was wondering how could I switch injection model from 2D to 3D?


Thank you