Hi Guillermo, As Stan mentioned, this error means the CG solver is not converging (in this case because the simulation diverged, as you can see in the last CFL output). Here are a few things I noticed in your setup, which might help you: - You set both the inflow and outflow boundaries as outflow. The correct setting for the inflow would be, for example <D VAR="u" VALUE="1"/> <D VAR="v" VALUE="0"/> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> - There are two MAPPING entries. I think the first is the correct one? - Your Mapping and MappingVel are not consistent. For example, you could have in your Mapping <E VAR="x" VALUE="x- 1.0*t" /> and in MappingVel <E VAR="vx" VALUE="-1.0" /> (note that "vx" is just the time derivative of "x"), although I am not sure what benefit you would get from this type of transformation. - Finally, in your run the CFL is relatively large (around 0.9), and therefore a transient spike in the CFL could cause the simulation to diverge. You could consider reducing the time-step a little bit. Cheers, Douglas 2017-11-22 12:08 GMT-02:00 Guillermo <guillermo180395@gmail.com>:
Hi Stan, Thanks for your quick response.
I am getting this error after several steps (22290). I am attaching the session, the mesh, output and error messages files.
Thanks, Guillermo
On 22/11/17 08:55, Stanisław Gepner wrote:
Hi Guillermo,
For some reason the CG solver failed to converge. Are you getting any iterations to execute at all, or does this happen at the very start of the simulation?
Not knowing your session and mesh I would start by having a look at the TimeStep, Kinvis and the initial condition you are using. Also, not sure here, but I think the mesh file should precede the session file, i.e.:
mpirun -np 8 IncNavierStokesSolver *mesh.msh.xml * *session.xml * Best, Stan
On 22.11.2017 12:43, Guillermo wrote:
Dear all,
I am using the Mapping function (VCSMapping) and it gave me some errors which I do not really understand the meaning. The simulation was executed in parallel: mpirun -np 8 IncNavierStokesSolver session.xml mesh.msh.xml
Output message: ... CFL (zero plane): 1.15785e+20 (in elmt 520) CG iterations made = 5001 using tolerance of 1e-09 (error = nan, rhs_mag = inf) ------------------------------------------------------- Primary job terminated normally, but 1 process returned a non-zero exit code.. Per user-direction, the job has been aborted. ------------------------------------------------------- --------------------------------------------------------------------------
mpirun detected that one or more processes exited with non-zero status, thus causing the job to be terminated. The first process to do so was:
Process name: [[36638,1],4] Exit code: 1 --------------------------------------------------------------------------
and the error messages are:
Fatal : Level 0 assertion violation Exceeded maximum number of iterations
I also have obtained a batch of error messages, however I think they are result of the simulation errors. Nevertheless, if you want them or any other file, please let me know.
So please, could you explain to me why I have obtained these error?
Thank you very much for your help.
Regards, Guillermo
_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
_______________________________________________ Nektar-users mailing listNektar-users@imperial.ac.ukhttps://mailman.ic.ac.uk/mailman/listinfo/nektar-users
_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users