[flotus1]

For various reasons I have been using Paraview only in serial mode until now.
Today I thought I should give it another try. The goal: create an animation for a rather large transient simulation (~60 mio cells, 450 time steps).
So I activated auto mpi, set the max number of cores to 22 (machine has 24 cores) and restarted paraview.

AutoMPI: SUCCESS: command is:
 "/opt/paraview/ParaView-5.3.0-Qt5-OpenGL2-MPI-Linux-64bit/lib/paraview-5.3/mpiexec" "-np" "22" "/opt/paraview/ParaView-5.3.0-Qt5-OpenGL2-MPI-Linux-64bit/lib/paraview-5.3/pvserver" "--server-port=51753"
AutoMPI: starting process server
-------------- server output --------------
Waiting for client...
AutoMPI: server successfully started.

Loading the state file turned out to be very promising. A "cell data to point data" filter and calculation of the Q-criterion were done in no time for the initial time step.
Unfortunately, that is about all I got. I can not switch to any other time step. Writing an animation creates the first image for the initial time step and nothing else. The 22 instances of "pvserver" are all running at 100% CPU load even after loading the initial time step is finished. Processing a single time step in serial mode takes around 11 minutes. I waited longer than that.
Paraview version is the latest release 5.3.0, operating system is Opensuse Leap 42.1. Edit: same negative result with Paraview version 5.2.0.
Any suggestions are welcome.

[flotus1]

A small bump with some new information.
Tweaking the ensight gold case file to include file set and time set for the geometry, I at least managed to get an error message out of paraview. It loads the first time step, but when I try to switch to a different time step I get this:
pv_error.png

What I am very suspicious about is the "0" added after the geometry path. Does ParaView expect some kind of parallel file format?

Edit: just to clarify, doing the same steps in serial mode works like a charm with no error messages. So my data structure can not be entirely wrong.

[flotus1]

Problem solved.
My case files looked something like this:

FORMAT
type: ensight gold

GEOMETRY
model: ../ModelEnsight/LB_results.geo

VARIABLE
scalar per element:         1         1 Pressure LB_results_primary_Scalar.scl
vector per element:         1         1 Velocity LB_results_primary_Vector.vec

TIME
time set:            1
number of steps:        3
time values:
         0
         1
         2
FILE
file set:            1
number of steps:        3

Adding a 0 at the right place resolved the issue:

FORMAT
type: ensight gold

GEOMETRY
model: 0 ../ModelEnsight/LB_results.geo

VARIABLE
scalar per element:         1         1 Pressure LB_results_primary_Scalar.scl
vector per element:         1         1 Velocity LB_results_primary_Vector.vec

TIME
time set:            1
number of steps:        3
time values:
         0
         1
         2
FILE
file set:            1
number of steps:        3