[ashishmagar600]

Hello everyone.

I am trying to simulate flow over a body of revolution using simplefoam and turbulence model komegasstlm (newly included in openfoam5). however I am ended up in foll errors:

Time = 5.7834e-06

smoothSolver:  Solving for Ux, Initial residual = 0.679871, Final residual = 0.0448022, No Iterations 3
smoothSolver:  Solving for Uy, Initial residual = 0.721651, Final residual = 0.0362827, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 0.660802, Final residual = 0.0331744, No Iterations 3
GAMG:  Solving for p, Initial residual = 0.416956, Final residual = 0.00025435, No Iterations 8
time step continuity errors : sum local = 5.58119e+23, global = -1.00912e+23, cumulative = -3.88815e+22
smoothSolver:  Solving for ReThetat, Initial residual = 1.48391e-06, Final residual = 1.41698e-07, No Iterations 1
smoothSolver:  Solving for gammaInt, Initial residual = 0.64792, Final residual = 0.00392748, No Iterations 1
bounding gammaInt, min: -0.319182 max: 1.2152 average: 0.479616
smoothSolver:  Solving for omega, Initial residual = 0.784666, Final residual = 0.0452345, No Iterations 2
bounding omega, min: -6.48197e+36 max: 1.0888e+39 average: 1.57096e+34
smoothSolver:  Solving for k, Initial residual = 0.769725, Final residual = 0.020874, No Iterations 1
bounding k, min: -2.22583e+21 max: 4.39716e+23 average: 1.10284e+20
ExecutionTime = 966.84 s  ClockTime = 978 s

Time = 5.8548e-06

smoothSolver:  Solving for Ux, Initial residual = 0.74717, Final residual = 5.6515e+17, No Iterations 10
smoothSolver:  Solving for Uy, Initial residual = 0.784921, Final residual = 3.46486e+17, No Iterations 10
smoothSolver:  Solving for Uz, Initial residual = 0.71581, Final residual = 7.78483e+17, No Iterations 10
[0] #0  Foam::error::printStack(Foam::Ostream&) at ??:?
[0] #1  Foam::sigFpe::sigHandler(int) at ??:?
[0] #2  ? 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 at ??:?
[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 at ??:?
[0] #5  Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
[0] #6  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
[0] #7  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
[0] #8  Foam::fvMatrix<double>::solve() at ??:?
[0] #9  ? at ??:?
[0] #10  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #11  ? at ??:?
[GRACE:05924] *** Process received signal ***
[GRACE:05924] Signal: Floating point exception (8)
[GRACE:05924] Signal code:  (-6)
[GRACE:05924] Failing at address: 0x3e800001724
[GRACE:05924] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x354b0)[0x7f5d1ec934b0]
[GRACE:05924] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x38)[0x7f5d1ec93428]
[GRACE:05924] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x354b0)[0x7f5d1ec934b0]
[GRACE:05924] [ 3] /opt/openfoam5/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam10GAMGSolver5scaleERNS_5FieldIdEES3_RKNS_9lduMatrixERKNS_10FieldFieldIS1_dEERKNS_8UPtrListIKNS_17lduInterfaceFieldEEERKS2_h+0x2a7)[0x7f5d1ff76bf7]
[GRACE:05924] [ 4] /opt/openfoam5/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam10GAMGSolver6VcycleERKNS_7PtrListINS_9lduMatrix8smootherEEERNS_5FieldIdEERKS8_S9_S9_S9_S9_S9_RNS1_IS8_EESD_h+0x7b2)[0x7f5d1ff7ac82]
[GRACE:05924] [ 5] /opt/openfoam5/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZNK4Foam10GAMGSolver5solveERNS_5FieldIdEERKS2_h+0x807)[0x7f5d1ff7d577]
[GRACE:05924] [ 6] /opt/openfoam5/platforms/linux64GccDPInt32Opt/lib/libfiniteVolume.so(_ZN4Foam8fvMatrixIdE15solveSegregatedERKNS_10dictionaryE+0x15b)[0x7f5d22194bab]
[GRACE:05924] [ 7] simpleFoam(_ZN4Foam8fvMatrixIdE5solveERKNS_10dictionaryE+0x191)[0x46ccd1]
[GRACE:05924] [ 8] simpleFoam(_ZN4Foam8fvMatrixIdE5solveEv+0xd4)[0x46cf24]
[GRACE:05924] [ 9] simpleFoam[0x42425d]
[GRACE:05924] [10] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf0)[0x7f5d1ec7e830]
[GRACE:05924] [11] simpleFoam[0x426fe9]
[GRACE:05924] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 0 with PID 5924 on node GRACE exited

The same case i ran previously for komegasst (running it on both of the model is part of my project) and got a converged solution.

we see number of errrs up there as time-step continuity and floating point exception. From other posts i saw as dividing something by zero gives floating point exception.

I followed this thread having similar issue:
simpleFoam k-omegaSST convergence problem

and used the suggestions as per vkrastev

Well, apart from the grid-quality issue, I think that there are some changes to try on the fvSolution/Schemes dictionaries...

1) lower the relaxationFactors for k and omega to 0.5
2) change div(phi,U) to linearUpwindV cellMDLimited Gauss linear 1
3) change div(phi,k/omega) to Gauss upwind (I know it is only first order, but usually the convective terms inherent to the turbulent quantities are quite unstable and sensitive to higher order discretization schemes, while you can improve a lot the accuracy of the solution using a higher order scheme only on div(phi,U) )
4) change the laplacian schemes to Gauss linear limited 0.5 (usually there's no need to force the limiter value below 0.5, as it will simply slower the convergence without any benefits on stability) and coherently the snGradSchemes to default limited 0.5.
5) lower the tolerance value of the solvers for k,omega,U to at least 1e-10 (this is important especially for omega, as sometimes the residuals for the omega equation fall very quickly to pretty low values and the risk of stop in solving the equation too soon should be avoided)

Hope this helps

I also reffered post GAMG hexa vs. tetrahedron meshes refered from another post to get an idea for using a good scheme to converge pressure.


But still no help for me. I am stuck in here for days now. At my wit's end.

Any suggestion will be appreciated.

Thanks

[ashishmagar600]

Any help, please......

[Zigec]

Hey there,

When we bump into an error, we first of all try to determine where the error comes from. Try step by step to simplify your simulation until it works out:
- lower the Re number and change the turbulent model to laminar
- try pisoFoam or pimpleFoam, sometimes there can appear problems when running steady state.

If your sure in the physics than there is probably a 90% responsibility for the crash in the mesh. Try using a better mesh. For OpenFOAM simulations I prefer using meshes which are made with the OpenFOAM tools - especially snappyHexMesh. The easiest way to make the mesh is to go on simscale.com (cloud based openfoam computing with interface). There you can with only a few click do a pretty good snappyHexMesh and than export it and save it into you working directory. Under documentations you can find good tutorials for meshing.

Hope it helps.
Ziga

[ashishmagar600]

Thanks a lot Zigec for sharing your opinions.

If your sure in the physics than there is probably a 90% responsibility for the crash in the mesh. Try using a better mesh.

I quickly reviewed my flow physics and the bcs were correct. After refining the mesh, atleast the errors are gone now.

try pisoFoam or pimpleFoam, sometimes there can appear problems when running steady state.

Yes, I sampled the case for some intermediate time step, and I saw some UNSTEADY WAKES in the boundary layer. I will try running with piso / pimple.

So how do we resolve unsteadiness in the flow...? The solution is not converging because of the wakes... Do I have to further refine the mesh.?

For OpenFOAM simulations I prefer using meshes which are made with the OpenFOAM tools - especially snappyHexMesh

Me too. The mesh was generated using sHM.

The easiest way to make the mesh is to go on simscale.com (cloud based openfoam computing with interface). There you can with only a few click do a pretty good snappyHexMesh and than export it and save it into you working directory. Under documentations you can find good tutorials for meshing.

I will surely try this.



Thanks, thanks a lot for your help.

[Zigec]

If you know that there is unsteadiness in the flow you can't run as steady state. I think that is the source of your bed convergence. I had the same problem when I did a simulation of a stirred tank, steady state just did not work out, in the end I went transient and waited for periodical behavior of some output variables, but jeah it is really time consuming.

For the mesh refinement. Wall layer should be enough, but you can also make some region refinement where high velocities appear. Calculate the Courant number so that you do not overdo it. But this is not so important, first get your simulation to work out properly and than you can do this stuff if you need it.

Simscale: https://www.simscale.com/docs/conten...l-spoiler.html It really is easy to use. Just a few clicks and you get a good mesh, you do not need to bother with a pen on paper and with all the tipping in the notepads. It safes a lot of time.

Cheers.

[ashishmagar600]

Thank you Zigec, for all your help.

Simscale: https://www.simscale.com/docs/conten...l-spoiler.html It really is easy to use. Just a few clicks and you get a good mesh, you do not need to bother with a pen on paper and with all the tipping in the notepads. It safes a lot of time.

I will definitely try this.

Thanks a lot.


The issue is solved... Thanks for all your support.