Solver fatal error
 

Hello everyone,

I attempted to run a simulation on OpenFOAM with simpleFoam using spalart-allmaras model. I am trying to simulate the starting and stopping vortices of an airfoil. I found that I can set time-dependent boundary conditions using uniformFixed Value, so I can accelarate and decelerate the flow to make the two vortices appear. However, when running the simulation, this error message appears:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.1
Exec : simpleFoam
Date : May 05 2017
Time : 18:50:09
Host : "jesumi-SATELLITE-P70-B"
PID : 4396
Case : /home/jesumi/OpenFOAM/jesumi-4.1/run/vortex2
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: convergence criteria
field p tolerance 1e-05
field U tolerance 1e-05
field nuTilda tolerance 1e-05

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model SpalartAllmaras
Selecting patchDistMethod meshWave
SpalartAllmarasCoeffs
{
sigmaNut 0.66666;
kappa 0.41;
Cb1 0.1355;
Cb2 0.622;
Cw2 0.3;
Cw3 2;
Cv1 7.1;
Cs 0.3;
}

No MRF models present

No finite volume options present


Starting time loop

Time = 0.001

smoothSolver: Solving for Ux, Initial residual = 1, Final residual = 43.2673, No Iterations 1000
smoothSolver: Solving for Uy, Initial residual = 1, Final residual = 1.30142, No Iterations 1000


--> FOAM FATAL ERROR:
Attempt to cast type uniformFixedValue to type freestream

From function To& Foam::refCast(From&) [with To = const Foam::freestreamFvPatchField<Foam::Vector<double> >; From = const Foam::fvPatchField<Foam::Vector<double> >]
in file /home/ubuntu/OpenFOAM/OpenFOAM-4.1/src/OpenFOAM/lnInclude/typeInfo.H at line 114.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::freestreamPressureFvPatchScalarField::update Coeffs() at ??:?
#3 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::Boundary::updateCoeffs() at ??:?
#4 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricFi eld<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:?
#5 Foam::fv::gaussLaplacianScheme<double, Foam::SymmTensor<double> >::fvmLaplacianUncorrected(Foam::GeometricField<do uble, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6 Foam::fv::gaussLaplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#7 Foam::fv::laplacianScheme<double, double>::fvmLaplacian(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#8 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::word const&) at ??:?
#9 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::laplacian<double, double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#10 ? at ??:?
#11 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#12 ? at ??:?
Aborted (core dumped)

ANY ADVICE??

THANK YOU.

There is something wrong with your boundary condition..check them again and also the patch types in constant/polyMesh/boundary..

Hi,

@jesumi

Since you utilise freestreamPressure BC for pressure, you have to utilise freestream for velocity. Set (for example) zeroGradient BC for pressure at the boundary, where you would like to use uniformFixedValue.

If you are trying to develop the vortexes themselves, you might be using the wrong solver.

SimpleFoam S-A is meant to give you a steadystate solution. If I understand you correctly, you may be better served with a PisoFoam LES solver instead.

thanks everyone.
 

Thank you for your answers.

I figured that out. Finally, I decided to use pimpleDyFoam, since I am trying to get the starting and stopping vortices. I already figured out how to make the airfoil to move linearly, but does anyone know how to make it stop?

Thanks in advance again

Are you talking about making the mesh move? Its usually easier to have the airfoil stand still and move the air instead.

dynamic mesh
 

Yes, I know. But if I do it that way, the results won't be the same because it's not the same if you move the airfoil and then stop it as if you move the air and then stop it. Inertial forces take place in the second scenario that I want to avoid