Water Flow Tutorial-2.10

This page contains an in-depth visualization tutorial for a water flow simulation.

Description of Simulation Data

This tutorial uses the dbreak3d dataset -- available at: http://www.visitusers.org/index.php?title=Tutorial_Data

The dataset simulates the evolution of water and air in a water tank after an interface holding a column of water is instantaneously removed. The data was generated using the OpenFOAM open source CDF simulator, using a two-phase volume of fluid (VOF) method to resolve the interface between the water and air.

Our case is a 3D variant of the 2D Dam Break OpenFOAM tutorial, which is described in detail at: http://www.openfoam.org/docs/user/damBreak.php. Several changes to the 2D tutorial input deck were necessary to create the 3D simulation. We started with guidance from http://www.calumdouglas.ch/openfoam-example-3d-dambreak/. Our OpenFOAM input deck is available at: https://github.com/cyrush/dbreak3d_vtutorial. We ran the simulation on a single node of the insight cluster at Clemson (Special thanks to Vetria Byrd and Galen Collier of Clemson for access to this resource)

After running the simulation we converted the OpenFOAM output to Silo data files. The Silo files are compressed and contain the subset of the variables of interest for this tutorial. The final dataset has 160 silo files holding 4 seconds of the simulation at time intervals of 0.025 seconds [40 timesteps per second].

You can open the entire time series in VisIt using the dbreak3d_fluid.visit file.

Variables

The simulation is run in an Eulerian fashion: The mesh itself is static -- but the variables evolve to reflect the physics.

Each of the 160 time steps contains three variables:

• U {u,v,w} -- Velocity vector
• alpha1 -- Volume fraction of water (0.0 - 1.0)
• p_rgh -- A pressure term

Boundaries

In addition to the fluid data the dbreak3d_boundaries.silo data file contains the boundaries of the water tank. We will use this additional file to bring context to our visualizations.

Exploring the Fluid Data

Viewing the Tank Boundaries

We will start by creating a plot that shows the water tank boundaries.

• Open dbreak3d_boundaries.silo file.
• Create a Subset Plot of domains
• Click Draw

This subset plot shows the different faces that comprise the water tank. We do not want to view all of the boundaries because they will block the fluid data, so next we turn off a few of the boundary faces that are identified as subsets or domains in the data file.

• Open the Set Selection Window (click on the Ven Diagram next to domains)
• Under domains: Turn off domain5 and domain6

• Click Apply

Finally, lets color all the faces with a uniform color:

• Open the Subset plot attributes window
• Select Single and choose the light pastel green color

• Click Apply and Dismiss

Viewing the Water sub-volume

Now we will plot the water in the tank.

• Uncheck Apply operators to all plots

• Open dbreakd3d_fluid.visit
• Create a Pseudocolor Plot of alpha1
• Double click on the Pseudocolor plot to bring up its attributes.
• Change the color table to PuBu
• Click Apply and Dismiss
• Create a Mesh Plot of mesh
• Click Draw
• Rotate to view the back face of the water column.

These are the initial conditions of the simulation.

The alpha1 variable defines the fraction of each cell's volume that is water. We are interested in the portion of the simulation mesh that are at least 50% water. To extract this sub-volume we use an Isovolume Operator:

• Delete the Mesh plot
• Add an Isovolume Operator (Operators->Selection->Isovolume)
• Double click on the Isovolume operator to bring up its attributes
• Set the Lower bound to .5
• Select alpha1 as the Variable option

• Click Apply and Dismiss
• Create the Subset plot of the boundaries dataset as before.
• Click Draw
• Rotate the plot to view the column of water in front of the tank boundaries.

Save Session File with Basic Visualization Setup

We will use these two basic plots as foundation for the rest of the tutorial, so it will be helpful to have a way to easily recreate them.

• Save the session (File->Save session as)
  • Set the file name to dbreak3d_plots_basic.session

You can use this session file to easily restore these two plots in the future.

You can also use the dbreak3d_plots_basic.py python script to reproduce these plots if you have both the dbreak3d_fluid.visit and dbreak3d_boundaries.silo databases opened.

Animate the simulation

• Click the Play button on the timer slider control.

Watch the water in the simulation move according to gravity and the constraints at the tank boundaries.

Later in the tutorial we will make a movie displaying water evolution in the tank.

Exploring Time Varying Properties of the Water

Next we will analyze two time varying aspects of the water flow.

Before we begin, there are two preparation items:

Import dbreak3d Tutorial Expressions

• Open the Expressions Window (Controls->Expressions)
• Click Load
• Select the dbreak_fluid_exprs.xml file (available in the dbreak3d folder in the tutorial examples folder.)
• Click Apply and Dismiss

Set Query Over Time Options

• Open the Query over time options Window (Controls->Query over time options)
• Select Time as the X-axis variable.
• Click Apply and Dismiss

Height of Water Over Time

The first question we will explore is:

What is the highest point in the tank that some volume of water reaches?

We will use VisIt's Expression and Query building blocks to answer the question. First, we need a way to extract the height of the water. We will start with the basic water and tank plot setup described previously and create a plot of y_coord. The definition for this expression is coord(mesh)[1], which extracts the second spatial coordinate from the mesh geometry and exposes it as a scalar variable.

• Change the active plot variable to y_coord
• Double click on the Pseudocolor plot to bring up its attributes.
• Change the color table to RedYlBlu
• Click Apply and Dismiss

The color of the plot now varies according to the height of the mesh cells.

Now we use the Max query to capture how the highest value varies over the duration of the simulation.

• Open the Query Window (Controls->Query)
• Select that Max Query

In the query options:

• Select Actual Data
• Check Do Time Query
• Click Query

This will process all 160 time steps and extract the max y-coordinate of the mesh cells that are more than 50% water. (It may take a few seconds to complete)

When the query completes a new window will appear with a curve plot that displays the max value vs time.

The curve shows us that the max height decays over time as gravity pulls the water to the bottom of the tank. From this curve we also see that the max height of any volume of water in the simulation happens at 0.475 seconds [timestep =19].

• Return to the window with your y_coord plot, and change the time slider to timestep=19.

At this time step we can see a blob of water near the top of the tank reach its maximum height as gravity overcomes its upward velocity.

• Use the time slider to view time steps before and after timestep = 19.

Number of Water Droplets Over Time

The next question we will explore about the water is:

How do blobs of water break away from the main water volume as the water column splashes and settles?

Again, we will use VisIt's Expression and Query building blocks to answer the question.

VisIt's connected components algorithm allows us to identify topologically distinct sub-volumes of a mesh. In the case of our water flow simulation we will use it to identify blobs or droplets of water that separate from the main water volume.

We will use the cc_label expression to view the droplets. First we need to make sure execute the cc_label expression after the Isovolume selects the water sub-volume.

• Select time step 25
• Add a DeferExpression Operator (Operators->Analysis->DeferExpression)
• Double click on the DeferExpression operator to bring up its attributes
• Enter cc_label in the Variables field.
• Click Apply

Select a different color table too improve the contrast of the labels:

• Double click to open the Pseudocolor attributes.
• Select the rainbow color table
• Click Apply
• Click Draw

The colors identify the different connected sub-volumes of the water. Next, lets execute the time varying query to see how the number of connected blobs evolves over time:

• Open the Query Window (Controls->Query)
• Select that Max Query

In the query options:

• Select Actual Data
• Check Do Time Query
• Set the Ending timestep to 80 (this is after that water settles down back into one connected sub-volume)
• Click Query

This will process 80 timesteps and extract the max connected component id. (It may take a few seconds to complete)

When the query completes a new window will appear with a curve plot that displays the max value vs time.

We can see that the water breaks into multiple chunks after the column splashes into the right wall of the tank. The maxim number of components occurs at t=0.75 seconds [timestep = 30] We can use a threshold operator to isolate the smaller components from the bulk of the water.

• Select time step 30
• Add a Threshold' operator to the current cc_label plot (Operators->Selection->Threshold)
• Double click on the Threshold operator to bring up its attributes
• Set the Minimum to be 1

• Click Apply and Dismiss
• Click Draw

There are 24 components at this time step (Labeled 0 though 23) -- we removed the largest which happens to be labeled 0. We can see that many of the components are quite small volumes of water:

Exploring the Velocity Vector Field

We will now explore three ways to visualize the velocity vector field of the simulation.

Plotting the Velocity Field using Vector Plots

First we will directly plot the velocity vectors that exist on the mesh nodes.

• Start with the basic tank boundaries and water sub-volume plots outlined previously.
• Use the time slider to select timestep = 1 (The velocity at timestep = 0 is fully zero)

• Add a Vector plot of U
• Open the Vector plot attributes
• On the 1st tab (Vectors), set the Stride to 30
• On the 2nd tab (Data), select the RdYlBu color table
• On the 3rd tab (Glyphs)
  • Set Scale to 0.75
  • Set Arrow body to Cylinder
  • Set Geometry Quality to High

• Click Apply and Dismiss
• Click Draw
• Zoom in to explore the plot results.

The vector plot uses glyphs to draw portions of the instantaneous vector field. The arrows are colored according to the speed at each point (the magnitude of the velocity vector). Next we will look at a more advanced technique to visualize the flow of the velocity vector field.

Streamlines at the Advancing Interface

Streamlines visualize flow by advecting a set of massless particles, initially placed at user selected seed points, through an instantaneous vector field. In our simulation, as the column of water falls it quickly pushes the water at the bottom outward and it collides with a small ledge. We can use a Streamline plot to explore the water velocity field at the advancing water front.

First we want to get an idea of where the advancing portion of the water is:

• Start with the basic tank boundaries and water sub-volume plots outlined previously.

• Select the Pseudocolor plot of alpha1
• Open the Query Window (Controls->Query)
• Execute a SpatialExtents Query with Original Data selected

This gives us the full extent of the fluid simulation mesh:

(0, 0.584, 0, 0.584, 0, 0.584)

• Now execute a SpatialExtents Query with Actual Data selected.

This gives us the extents of just the water column:

 (0, 0.146, 0, 0.275799, 0, 0.3066

With this info in hand, we can create a Streamline plot with seed points near this interface.

• Use the time slider to select time step = 1 (The velocity at time step = 0 is fully zero)
• Add a Streamline plot of U
• Open the Streamline attributes
  • Under the 1st tab (Streamlines)
    • Create a Plane source at
      • Origin: 0.148 0.15 0.15
      • Normal: 1 0 0
      • Up axis: 0 1 0
      • Samples in X: 8
      • Samples in Y: 5
      • Distance in X: 0.25
      • Distance in Y: 0.25
    • For termination:
      • Set Limit maximum time elapsed for particles to .1
  • Under the 2nd tab (Appearance)
    • Select the RdYlBlu color table
    • Draw as Tubes
    • Deselect Show seeds
    • Select Show heads and Display as Cone
    • Set the heads Radius to 0.012
    • Set the heads Height:Radius Ratio to 4
  • Under the 3rd tab (Advanced)
    • • Turn off all warnings

• Click Apply and Dismiss
• Click Draw

At this point save your visualization session:

• Save the session (File->Save session as)
  • Set the file name to dbreak3d_plot_streamlines.session

You can experiment with both advancing the time slider and moving the X-origin of the plane used to define the seed points.

• Open the Streamline attributes
• Select time step = 3
• Under the 1st tab (Streamlines) set:
  • Origin: 0.18 0.025 0.15
  • Distance in Y: 0.05
• Click Apply

• Select time step = 4:
• Under the 1st tab (Streamlines) set:
  • Origin: 0.195 0.025 0.15
  • Distance in Y: 0.05
• Click Apply

• Select time step = 5:
• Open the Streamline attributes
• Under the 1st tab(Streamlines) set:
  • Origin: 0.210 0.025 0.15
  • Distance in Y: 0.05
• Click Apply

You can also exaggerate the length by increasing the termination time -- however recall there are only 0.025 seconds between each timestep. To be a better visualize of how seed points travel though the vector field as it evolves over time, we will use a pathline technique.

Using Pathlines to Understand Time Varying Flow

Pathlines extend the advection / integral curve concept of streamlines to a time varying vector field. Using pathlines we can trace the paths massless particles would take from the start to the end of the simulation, using the velocity vector field data from all output files.

To do so, we first adjust to select seed points that are well embedded in the fluid column at the beginning of the simulation.

• Start with the Streamline plot previously outlined (you can use your dbreak3d_plot_streamlines.session or the dbreak3d_plot_streamlines.py python script)
• Set the timer slider to time step = 0
• Open the Streamline attributes
  • Under the 1st tab (Streamlines)
    • Create a Plane source at
      • Origin: 0.12 0.1 0.15
      • Distance in X: 0.225
      • Distance in Y: 0.2
    • For termination:
      • Set Limit maximum time elapsed for particles to 2
  • In the 3rd tab (Advanced)
    • Select Pathline
    • Select Mesh is static over time
• Click Apply and Dismiss

This will create paths that start at timestep=0 at our seed points and travel with the flow for 2 seconds to simulation time. (This will process may take a few seconds because it will process 80 data files)

Pathlines expose the complex flow behavior of the velocity vector field.

Lets extend the termination time to the final time of the simulation.

• Open the Streamline attributes
  • Under the 1st tab(Streamlines)
    • For termination:
      • Set Limit maximum time elapsed for particles to 4

At this point save your visualization session:

• Save the session (File->Save session as)
  • Set the file name to dbreak3d_plot_pathlines.session'

Animating pathlines with a python script

The Streamline plot allows you to crop away portions of paths without recomputing the streamlines or pathlines to help support integral curve animations. You can use the dbreak_animate_pathlines.py to animate our pathline visualization from 0 to 4 seconds.

Source("path/to/examples/dbreak3d/dbreak_animate_pathlines.py")

You can easily execute this script using the Commands Window (Controls->Command)

Rendering a Movie of the Fluid Data

To finish this in-depth tutorial we will create a a simple movie from the water flow simulation data. The movie will display the movement of the water sub-volume and leverage a few more bells and whistles to create a polished visualization.

• Start with the basic tank boundary and water isovolume plot setup (you can restore your dbreak3d_plot_basic.session file or use the dbreak3d_plot_basic.py python script)
• Open the Pseudocolor plot attributes
• Under Color, for Opacity select Constant
• For Opacity select Constant
• Set the Opacity slider value to 65%
• Click Apply and Dismiss

Setting the Window Annotations

To make the visualization look more polished, we will change the window annotations and background, lighting, and add a time slider annotation:

• Open the Annotations Window (Controls->Annotation)
• On the 1st Tab:
  • Click No Annotations
  • Click Apply
• On the 3D Tab:
  • Recheck Show bounding box
• On the Color Tab:
  • Set the Foreground color to be the same color as our tank boundaries plot.
  • Select a Gradient background with the Radial style.
  • Set Gradient color 1 to be light gray
  • Set Gradient color 2 to be very dark gray

• On the Objects Tab:
  • Create a new Time slider annotation.
  • For the name dialog type ts and click Ok
    • Set the Width to 40%
    • Set the Height to 7%
    • Set the Start color to Light Blue
    • Set the End color to a darker Blue
    • Set the Text color to White
    • Uncheck Rounded and Shaded

The default light shines straight on to the scene, which is not as intuitive for humans who are primarily used to overhead lighting.

• Open the Lighting Window (Controls->Lighting)
  • Move the light vector up and to the right.
  • Click Apply

Try a few different settings until you find a setting you are satisfied with.

• Click Dismiss

Encoding the movie

Now we are ready to create an mpeg of the visualization.

• Open the Save Movie wizard (File->Save movie)
• Follow the prompts to create a MPEG movie with a 1000x1000 output resolution.

This will render all of the timesteps of the simulation data and create an mpeg in your home directory. You can also save a sequence of images in addition to encoding to a movie format.

The end!