CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Solver fatal error

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2017, 13:04
Default Solver fatal error
  #1
New Member
 
Jesús Miguel
Join Date: Dec 2016
Posts: 8
Rep Power: 2
jesumi is on a distinguished road
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:rintStack(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.
jesumi is offline   Reply With Quote

Old   May 5, 2017, 20:40
Default
  #2
Senior Member
 
khedar
Join Date: Oct 2016
Posts: 103
Rep Power: 2
khedar is on a distinguished road
There is something wrong with your boundary condition..check them again and also the patch types in constant/polyMesh/boundary..
khedar is offline   Reply With Quote

Old   May 6, 2017, 04:38
Default
  #3
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,652
Rep Power: 27
alexeym will become famous soon enoughalexeym will become famous soon enough
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.
alexeym is offline   Reply With Quote

Old   May 11, 2017, 09:54
Default
  #4
New Member
 
Anders Utnes
Join Date: May 2017
Location: Norway
Posts: 6
Rep Power: 2
Alasir is on a distinguished road
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.
Alasir is offline   Reply With Quote

Old   May 11, 2017, 10:13
Default thanks everyone.
  #5
New Member
 
Jesús Miguel
Join Date: Dec 2016
Posts: 8
Rep Power: 2
jesumi is on a distinguished road
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
jesumi is offline   Reply With Quote

Old   May 11, 2017, 10:19
Default
  #6
New Member
 
Anders Utnes
Join Date: May 2017
Location: Norway
Posts: 6
Rep Power: 2
Alasir is on a distinguished road
Are you talking about making the mesh move? Its usually easier to have the airfoil stand still and move the air instead.
Alasir is offline   Reply With Quote

Old   May 11, 2017, 10:43
Default dynamic mesh
  #7
New Member
 
Jesús Miguel
Join Date: Dec 2016
Posts: 8
Rep Power: 2
jesumi is on a distinguished road
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
jesumi is offline   Reply With Quote

Reply

Tags
error, openfoam, spalartallmaras

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 19:44
groovyBC sega OpenFOAM Running, Solving & CFD 12 February 17, 2010 10:30
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
Compiling problems with hello worldC fw407 OpenFOAM Installation 21 January 6, 2008 18:38
DecomposePar links against liblamso0 with OpenMPI jens_klostermann OpenFOAM Bugs 11 June 28, 2007 17:51


All times are GMT -4. The time now is 00:14.