ACU-T: 4003 Freely Falling Water Droplet


This tutorial introduces you to the workflow for setting up a transient droplet simulation using HyperWorks CFD. Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperWorks CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperWorks CFD and AcuSolve.

Before you begin, copy the file(s) used in this tutorial to your working directory.
Note: This tutorial does not cover the steps related to geometry cleanup and mesh settings.

Problem Description

The problem to be addressed in this tutorial is shown schematically in the figure below. In this problem, a water droplet with 1 mm diameter falls freely under gravity. Given the small drop radius, surface tension and contact angle as the imposed wall treatment play a significant role to recover the drop shape after the impact. You will use AcuSolve to simulate the different developing drop shapes after impacting the wall.

Figure 1.
Note: The schematic is not of exact scale.

Start HyperWorks CFD and Open the HyperMesh Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > Altair <version> > HyperWorks CFD.
  2. From the Home tools, Files tool group, click the Open Model tool.

    Figure 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file and click Open.
  4. Click File > Save As.
  5. Create a new directory named ContactAngle and navigate into this directory.
    This will be the working directory and all the files related to the simulation will be stored in this location.
  6. Enter FallingDroplet as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Validate the Geometry

The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.

Figure 3.

Set Up Flow

Create Materials

  1. From the Flow ribbon, click the Material Library tool.

    Figure 4.
    The Material Library dialog opens.
  2. Under Settings, click Immiscible Multiphase then click the My Materials tab.
  3. Click to create a new material.
  4. In the new dialog, rename the material to air_water_st by clicking the name in the top-left corner, then enter the properties shown below.

    Figure 5.

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, click the Physics tool.

    Figure 6.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Activate the Multiphase flow radio button.
    2. Set the Multifluid type to Immiscible and the Immiscible material to air_water_st
    3. Set the Time step size to 0.0005 and the Final time to 0.15
    4. Select Laminar as the Turbulence model.
    5. Set the gravity to -9.81 m/sec2 in the y direction.

    Figure 7.
  3. Click Solver controls and verify the following:
    • Minimum stagger iterations: 0
    • Maximum stagger iterations: 6
    • The Flow and Multifluid checkboxes are activated.

    Figure 8.
  4. Close the dialog and save the model.

Assign Material Properties

  1. From the Flow ribbon, click the Material tool.

    Figure 9.
  2. Verify that air_water_st has been assigned to the volume.
  3. Click on the guide bar.

Define Flow Boundary Conditions

  1. From the Flow ribbon, click the Symmetry tool.

    Figure 10.
  2. Click on the View Controls toolbar and set the model orientation to Isometric.
  3. Select the Z-Positive face, as highlighted below.

    Figure 11.
  4. In the Boundaries legend, double-click on Symmetry and rename it to Z_pos
  5. On the guide bar, click to execute the command and remain in the tool.
  6. Rotate the model and select the opposite face.
  7. In the Boundaries legend, double-click on Symmetry and rename it to Z_neg
  8. On the guide bar, click to execute the command and exit the tool.
  9. Click the Outlet tool.

    Figure 12.
  10. In the Boundaries legend, right-click on Default Wall and select Isolate.
  11. Click on the View Controls toolbar and set the model orientation to Isometric.
  12. Select the top and side faces, as highlighted below.

    Figure 13.
  13. In the microdialog, set the following properties then click on the guide bar.

    Figure 14.
  14. Click the No Slip tool.

    Figure 15.
  15. In the Boundaries legend, Isolate the Default Wall then Show the Outlet faces.
  16. Select the face highlighted below.

    Figure 16.
  17. In the microdialog, activate the Specify contact angle checkbox, set the Contact angle value to 75, then click on the guide bar.

    Figure 17.

Generate the Mesh

The meshing parameters for this tutorial are already set in the input file.
  1. From the Mesh ribbon, click the Volume tool.

    Figure 18.
    The Meshing Operations dialog opens.
  2. Check that the Average element size is 0.006.
  3. Accept all other default parameters.

    Figure 19.
  4. Click Mesh.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: Right-click on the mesh job and select View log file to view a summary of the meshing process.

Define Nodal Outputs and Nodal Initial Conditions

In this step, you will define the nodal output frequency and then specify the nodal initial conditions for the water droplet.

Define Nodal Output Frequency

  1. From the Solution ribbon, click the Field tool.

    Figure 20.
    The Field Output dialog opens.
  2. Click the Solution variables setting.
  3. Activate the Write initial conditions checkbox.
  4. Verify that the Write results at time step interval checkbox is active.

    Figure 21.

Define Nodal Initial Conditions

  1. From the Solution ribbon, Zones tool group, click the Cylinder tool.

    Figure 22.
  2. Select the Top face on the View Cube to orient the model.
  3. Double-click on the geometry to create the cylinder-shaped zone then press Esc.

    Figure 23.
  4. To provide the dimensions of the cylinder, right click on Nodal initial condition cylinder in the legend and select Edit.
  5. In the microdialog, click the icon on the right to expand the menu, then set the radius to 0.001 and the height to 0.00339589

    Figure 24.
  6. Click on the View Controls toolbar and select Isometric.

    Figure 25.
  7. Zoom in on the zone and select the base point of the cylinder, as shown in the figure below. Set the coordinates to (0.06, 0.02, -0.001).

    Figure 26.
  8. Select the Rear face on the View Cube and verify that cylinder zone is passing over the domain completely as shown in below figure.

    Figure 27.
  9. In the initial condition dialog, click , select Fluid, then left-click in empty space.
  10. Change the fluid to Water.

    Figure 28.

Run AcuSolve

  1. From the Solution ribbon, click the Run tool.

    Figure 29.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Leave the remaining options as default and click Run to launch AcuSolve.

    Figure 30.
    The Run Status dialog opens. Once the run is complete, the status is updated and you can close the dialog.
    Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the solution process.

Post-Process the Results with HW-CFD Post

  1. Once the solution is completed, navigate to the Post ribbon.
  2. From the menu bar, click File > Open > Results.
  3. Select the AcuSolve log file in your problem directory to load the results for post-processing.
    The solid and all the surfaces are loaded in the Post Browser.

    Figure 31.
  4. To check the contours of volume fraction of water on the solid, right-click on Z_pos in the Post Browser and select Isolate.
  5. Right-click on Z_pos again and select Edit.
    A microdialog for surface coloring opens.
  6. Set the display to volume fraction water and toggle on the Legend radio button.
  7. Click in the same dialog and to verify the legend properties shown below.
    You will be able to see the contours of volume fraction of water at time step=1.

    Figure 32.

    Figure 33.
  8. Make sure the time scale at the bottom of modelling window is at time step =1. Click on the bar to see the falling of droplet and interaction of it with surface at time step = 65, 75, 85 and final time step (where 1 time step = 2 secs).

    Figure 34.

    Figure 35.


In this tutorial, you successfully learned how to set up and solve a simulation involving contact angle and surface tension using HyperWorks CFD. You imported the geometry and then defined the simulation parameters and flow boundary conditions. Once the solution was computed, you used HyperWorks CFD Post to create the contours of volume fraction of water