This chapter was written and developed by Federica Scolari Federica Scolari


In the case in which the simulations were run in parallel, before post-processing the data, the first step consists in reconstructing (i.e., reassembling) all solution steps of the analyzed case. This can either be done for all time steps or only for a specific one. The commands that need to be typed in the terminal window are shown below:

  • To reconstruct all solution steps:

user@user123:~/OpenFOAM-9/channel/Simulation$ reconstructPar
  • To reconstruct a specific time step (substitute “x” with the time step):

user@user123:~/OpenFOAM-9/channel/Simulation$ reconstructPar -time x

Once the case has been reconstructed, as for the meshing process, the following command should be used to visualize the case in the software ParaView:

user@user123:~/OpenFOAM-9/channel/Simulation$ paraFoam

The channel.OpenFOAM should now be present in the Pipeline Browser and to visualize it in the layout, press the Apply button. Additionally, in the Fields section, the various fields that can be visualized are shown and can be selected/deselected according to the focus of the analysis.


Fig. 241 Visualization of the case results in ParaView.#

In order to visualize the air and water phases, alpha.water should then be selected in the drop-down menu as shown in the image below.


Fig. 242 Enabling the setting for viewing the air and water phases in ParaView.#

To change the shown time step, the arrows that can be seen in the area highlighted in red can be used.

openfoam timestep time step

Fig. 243 Options for changing the time step to be visualized.#

Next, to visualize only the water phase, the Clip filter is used. This can either be found in the Filters section in the menu, or alternatively, the shortcut can be used. The Clip Type should be set to Scalar, selecting alpha.water as scalar and setting the value to 0.5, which represents the interface between air and water. To view the air phase, the Invert option should be selected whereas for the water phase it should be deselected.

openfoam clip water interFoam

Fig. 244 Clip filter used for viewing the water phase in ParaView.#

Finally, to also add the walls and patches to the view, the Extract Block filter can be implemented (click on the channel.OpenFOAM file before applying it).


Fig. 245 List of filters available in ParaView, highlighting ExtractBlock.#

The patches of interest can then be either selected or deselected, and the Coloring can be set to Solid Color.


Fig. 246 Available options for selecting the patches and changing the color.#

The resulting view of the water phase and block extraction is shown below:


Fig. 247 Simulation results highlighting the water phase.#

Different parameters can also be viewed, such as the flow velocity, and this can be done in the Coloring section by selecting U. The preset can be modified to better view the results by selecting the corresponding icon (highlighted in green).


Fig. 248 Simulation results highlighting the flow velocity.#