Paraview is an open-source software application which is utilised to portray TransAT simulation results
in a visual 2D or 3D manner. This process allows data to be easily intrepreted, as opposed to analysing
large quantities of text which would be deeply impractical. This tutorial will introduce Paraview by first
aclimatising the user with the GUI layout and then proceeding to describe how to import and visualise
TransAT simulation data.
1.2 Paraview GUI
The Paraview GUI 1.1 is made up of 4 main sections: Main Control Toolbar, Pipeline Browser, 3D
Viewer and Properties Tab.
Figure 1.1: GUI
Main Control Toolbar: The main control toolbar 1.2 contains numerous functions related
to the operation of the software, some of which will be referred to later in the tutorial.
Figure 1.2: Main Options Toolbar
Pipeline Browser: The pipeline browser is 1.3 used to display which files are currently
being visualised in the software and also to show the seperate isosurfaces incorporated into
each visualisation. Multiple visualisations can be open at any one time and this file tree
allows the user to select and switch between visualisations using the eye tabs next to the
file.
Figure 1.3: Pipeline Browser
3D Viewer: The 3D viewer window 1.4 portrays the current graphical visualisation and
animation of the datasets file in question. It allows the user to alter the view of the
visualisation using the mouse and also display variable colour scales integrated with the
visualisation, such as the temperature in 1.4
Figure 1.4: 3D View
Properties Tab: The properties tab 1.5, located below the pipeline browser is used to define
contours, alter isosurface value ranges and change the colour settings of a visualisation.
Figure 1.5: Properties
1.3 Test Case Example (Heated Bundle)
1.3.1 Process Overview
To allow the user to gain experience in the working process of visualising TransAT simulation data in
Paraview, a test case example has been explained in explicit detail for the user to work through and
become familiar with the steps and operations involved. This example will focus on the
heated bundles test case which can be found in the tutorial folder at the following location
TransAT simulation results are always saved in the folder RESULT, which is located inside the
directory the simulation was initially run in. Start Paraview by typing the following command into
the terminal:
$paraview&
Listing 1.1: Paraview command
Once the software is open, the user should begin by first importing the simulation results into
Paraview. A Paraview visualisation can be saved at any time by selecting File–Save State and opened
similarly by File– Load State.
1.3.2 Data Import
To import the data, select File–Open in the main toolbar. In the file selection window, navigate to the
RESULT folder which is located inside the directory TransAT was opened with and run in e.g.
/”projectname”. Inside the RESULT folder are the simulation datasets which will be used
to visualise the results. Select the file <projectname>...vtm. This file contains numerous
<projectname>.XXXXXX.vtm files which act as individual frames in the final animation Paraview will
create. Be sure to select the father file ...vtm as it allows all the enumerated .vtm files for
each time sequence to be imported and compiled into an animation instead of just a single
frame.
1.3.3 Defining Contours
After selecting the file and opening it, the project file will appear in the Pipeline browser. Select the
Apply button in the Properties tab. This will introduce the domain to the 3D view. Now it is time to
define what Paraview should display in the visualisation. To apply the contour filter on the
heated_bundle data that was imported, select heated_bundle.000* in the pipeline browser with a
simple click. Then, select Filters–Common–Contours in the main toolbar or select the Contour button
in the main options toolbar 1.6. A contour entry will appear in the Pipeline browser.
Figure 1.6: Contour button
The properties of this contour can now be defined using the Properties tab. The contour function
selects a scalar array which is then used to create isolines and/or isosurfaces to be seen
in the visualisation. Multiple scalar arrays are available in the drop down menu however
the only two used in this simulation are EmbI and PHI. In the Contour option tab select
Contour by: EmbI in the drop down menu. EmbI is the distance to the solid-fluid interface and is used
to visualise the interface between a solid part and the fluid flow in question. Below in the
Isosurfaces panel, add a New Value of 0 and Delete the previous value. Select Apply. The 3Dview tab should now show the solid-fluid interface, which in this case is the cylindrical
tubes.
The fluid Isosurface should now be defined. To apply the contour filter on the heated_bundle
data, select heated_bundle.000* in the pipeline browser with a simple click. Then, select
Filters–Common–Contours. A second contour file will appear in the Pipeline browser. Similarly to the
first contour, its properties must be defined in the Properties tab. Select Contour by: PHI in the drop
down menu, where PHI is the level set distance of the liquid-gas interface. As before, a value of 0 should
be added in the Isosurface value range and the other value that was there by default should be removed.
Select Apply. The fluid Isosurface will now appear alongside the cylinders in the 3D viewer as shown
in 1.7
Figure 1.7: Defined Contours
After both the Isosurfaces have been defined, the animation can be played using the
vcr controls in the main toolbar. Make sure both contours are visible by checking the eye
on the left hand side of their branch in the Pipeline browser1.8. Press play in the vcr
controls 1.9 to see the animation of the two Isosurfaces and how they react with each other
physically.
Figure 1.8: Eye Tabs
Figure 1.9: Vcr Controls
1.3.4 Variable Visualisation
In TransAT, multiple basic equations can be activated as part of the simulation including temperature,
pressure, and velocity. The variables that are solved for can be visualised in the animation. To do this,
first select the EmbI contour file (cylinders) in the Pipeline browser. In the Properties tab,
scroll to the bottom and find the Colour panel. In the drop down list there are multiple
options including pressure P, temperature T and unit vectors U, V and W. Select T, the
temperature of the surface and press the button Show to bring up the colour scale as seen in 1.10
Figure 1.10: Coloured Simulation
In the Colour panel you can also customise the colour scale used by clicking Edit. Select two
appropriate colours for either end of the scale i.e. green and red, and in the Colour Space drop down
menu select Wrapped HSV. Select Apply and then Close. Rescale will alter the axis values so they are
within an appropriate range for the simulation. Press play in the vcr controls to view the animation
again. The Isosurfaces will now display temperature change by varying colour scales. This process
should be repeated for the PHI (fluid) contour.
1.3.5 Vectors and Streamlines
In addition to the Isosurfaces seen in the visualisation, vectors and streamlines from the fluid flow can
also be visualised. To do this, highlight the project father file (i.e. heated_bundle.000*) in the
Pipeline browser, and select the Calculator button directly above it 1.12. The calculator
function will appear in the Properies tab 1.11. In the input box, type or select the buttons
in the calculator so that the field below the Result Array Name field is the following:
U*iHat+V*jHat+W*kHat
This equation combines the unit vectors iHat,jHat and kHat with the scalar velocities U,V and W
provided by TransAT. Select Apply. Press the Glyph button which is located in the MainOptions Toolbar and then Apply again, at which point flow vectors will appear in the 3Dview. These vector arrows can be cutomised using the Arrow panel in the Properties
tab.
Figure 1.11: Calculator
Figure 1.12: Calculator, Glyph and Stream tracer respectively
For streamlines, highlight the Calculator entry in the Pipeline browser and select the StreamTracer button in the Main Options Bar. A stream tracer file will appear in the Pipelinebrowser and and its properties become available in the Properties tab. Select Apply and the
streamlines will appear in the 3D viewer. In the Properties tab of the StreamTracer file there are
some options for customising the streamline visualisation. Seed Type allows the user to
select whether the stream lines originate along the entire Z axis plane Point Source1.13
or more precisely originating from either the X or Y axis domian lines along the Z plane
High Resolution Line Source1.14. The origination axis can be selected using the X Axis, Y Axis
and Z Axis buttons. The Colour panel can also be used to characterise the streamlines
further so that they display specific functions such as unit vectors U, V, W or temperature
T. The number of streamlines can be increased or decreased by changing the value in the
Number of Points. This function is very useful for creating a more accurate visualisation of flow
vorticies.
Figure 1.13: Visualisation with Vectors and Streamlines.
