Previous: Solver setup Up: Running the simulation Next: The Flow around a

This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Results evaluation

  • 43 One can continually watch the convergence of velocity vector components during the computation using a small script for gnuplot that is given in the following listing. Let’s name the file residual.gp.
    # Gnuplot script file for plotting data from file "log"
    set title "Convergence process"
    set xlabel "Iterations"
    set ylabel "Residuals"
    set grid
    set logscale y
    plot "< cat log | grep Ux | cut -d' ' -f9 | tr -d ','" title 'u', \
         "< cat log | grep Uy | cut -d' ' -f9 | tr -d ','" title 'v', \
         "< cat log | grep Uz | cut -d' ' -f9 | tr -d ','" title 'w'
    pause 10   # or "pause mouse"
  • The script expects the output of the solver to be in the file log. If any other output file is to be used, e.g. log.simpleFoam , one has first to create a symbolic link named log.
    # ln -s log.simpleFoam log
    # gnuplot residual.gp
openfoam tutorial car case velocity residual

Figure: OpenFOAM tutorial car case. Residuals of velocity vector components.

  • One can reconstruct the case after the end of parallel computation by running command:
    # reconstructPar -latestTime

  • The switch -latestTime tells the utility reconstructPar to reconstruct just the last time level, because the case is computed as a steady state simulation.

  • The results can be analyzed using paraview. Either simply run paraFoam without any arguments as usually, or create first carNoMotor.OpenFOAM placeholder file by typing
    # paraFoam -touch
    and then run ParaView without the OpenFOAM wrapper paraFoam:
    # paraview


  • To load the case results into plain ParaView select File $ \rightarrow$ Open and open the placeholder *.OpenFOAM file.

  • ParaView uses “states”, which are prepared templates for visualization of the cases. They contain an already populated pipeline and view transformations.
  • A prepared scene can be saved as a ParaView state using the menu item File $ \rightarrow$ Save state.
  • NOTE: ParaView state file *.pvsm provides absolute path to the *.OpenFOAM placeholder.

  • To load a preset “state” into ParaView delete all objects from the pipeline and select File $ \rightarrow$ Load State and choose a prepared template, e.g. pvsm/uField.pvsm.
  • NOTE: The absolute path to the *.OpenFOAM placeholder in loaded “state” file may differ from current path to the *.OpenFOAM placeholder. If the path is different ParaView ask you for it via “Fix Paths in State File” window.
  • The template uField displays velocity field in xy plane and stream lines around a car body.

Figure: OpenFOAM tutorial car case. Velocity field in the 178 plane and stream lines


Figure: OpenFOAM tutorial car case. Pressure field in the 178 plane and pressure distribution on the car body

  • Similarly, loading the template pField.pvsm will display the pressure field in the 178 plane and the pressure distribution on a the car body.
  • The utility foamLog 179log 180 can be used to extract all interesting data from log file.
  • All the data obtained by foamLog can be visualized using gnuplot.
  • The reader can find more information about foamLog 179log 180 in the chapter “Backward-facing step” of CFD support manual part I.
  • A sample script allresiduals.gp is in the case directory.
openfoam tutorial car case all residual puvw 1

Figure: OpenFOAM tutorial car case. Residuals of velocity components, pressure and turbulent variables

  • Computed aerodynamic coefficients 181 a  are stored in directory
  • Coefficients have been written for each time step, therefore their running could be visualized.