ACU-T: 4000 Transient Dam Break Simulation

Prerequisites

This tutorial introduces you to the workflow for setting up an AcuSolve transient dam break 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.

Prior to running through this tutorial, copy HyperWorksCFD_tutorial_inputs.zip from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract ACU-T4000_dambreak2D.x_t from HyperWorksCFD_tutorial_inputs.zip.

Problem Description

The problem to be addressed in this tutorial is shown schematically in the figure below. It consists of a square water column held in place by the reservoir walls. At time t=0, the walls are removed and the water column is now free to flow out. The simulation can be used to visualize and study the surge patterns as the column of water rushes out, as in a dam wall break.



Figure 1.

Start HyperWorks CFD and Create the HyperMesh Model Database

  1. Start HyperWorks CFD from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperWorks CFD.
    When HyperWorks CFD is loaded, the Geometry ribbon is open by default.
  2. Create a new .hm database in one of the following ways:
    • From the menu bar, click File > Save.
    • From the Home tools, Files tool group, click the Save tool.


      Figure 2.
  3. In the Save File As dialog, navigate to the directory where you would like to save the database.
  4. Enter DamBreak as the name for the database then click Save.
    This will be your problem directory and all the files related to the simulation will be stored in this location.

Import and Validate the Geometry

Import the Geometry

  1. From the menu bar, click File > Import > Geometry Model.
  2. In the Import File dialog, browse to your working directory then select ACU-T4000_dambreak2D.x_t and click Open.
  3. In the Geometry Import Options dialog, leave all the default options unchanged then click Import.


    Figure 3.


    Figure 4.

Validate the Geometry

  1. From the Geometry ribbon, Cleanup tools, click the Validate tool.


    Figure 5.
    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.

    The current model doesn’t have any of the issues mentioned above. Alternatively, if any issues are found, they are indicated by the number in the brackets adjacent to the tool name.

    Observe that a blue check mark appears on the top-left corner of the Validate icon. This indicates that the tool found no issues with the geometry model.


    Figure 6.
  2. Press Esc or right-click in the modeling window and select Exit from the context menu to exit the tool.
  3. Save the database.

Set Up the Problem

Set Up the Simulation Parameters and Solver Settings

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


    Figure 7.
    The Setup dialog opens.
  2. Click the Time setting and select Transient.
  3. Set the Time step size to 0.002498 and the Final time to 1.0
  4. Make sure the Final time termination option is active.


    Figure 8.
  5. Click the Flow setting then select Laminar.
  6. Activate the Include gravitational acceleration option and set the gravity to -9.81 m/sec2 in the y-direction.


    Figure 9.
  7. Click the Multifluid setting, set the Multifluid type to Immiscible, and the Immiscible material to Air-Water.


    Figure 10.
  8. Click the Solver Controls setting and set the Maximum stagger iterations to 5.


    Figure 11.
  9. Exit the dialog and save the database.

Assign Material Properties

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


    Figure 12.
  2. Click anywhere on the dam geometry.
  3. In the microdialog, select Air-Water from the Material drop-down.


    Figure 13.
  4. On the guide bar, click to execute the command and exit the tool.
  5. Save the database.

Define Flow Boundary Conditions

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


    Figure 14.
  2. Select the right most face on the positive z-axis, as shown in the figure below.


    Figure 15.
  3. In the Boundaries legend, double-click on Symmetry, rename it to z_pos and press Enter.
  4. On the guide bar, click to execute the command and remain in the tool.
  5. Rotate the model and select the opposite face.
  6. In the Boundaries legend, rename Symmetry to z_neg.
  7. On the guide bar, click to execute the command and exit the tool.
  8. Save the database.

Generate the Mesh

In this step, first you will create a surface mesh using the Interactive meshing tool; then, you will specify a global mesh size and growth rate for the model and generate the volume mesh using the Batch tool in the Mesh ribbon.

Create Surface Mesh

  1. From the Mesh ribbon, Surface tools, click the Interactive tool.


    Figure 16.
    By default, the Create should be selected from the secondary ribbon.
  2. Click on the guide bar to open the options menu, then make the following changes:
    1. Set the Element size to 0.00254.
    2. Set the Mesh type to Mapped.
    3. Set the Map method to Map as triangle.


    Figure 17.
  3. On the guide bar, change the entity selector to Solids then select the solid in the modeling window.
  4. Click Mesh in either the microdialog or on the guide bar to generate the surface mesh.
  5. Once the surface mesh is created, press Esc to exit out of the tool.

Generate Volume Mesh

  1. From the Mesh ribbon, Mesh tools, click the Batch tool.


    Figure 18.
    The Meshing Operations dialog opens.
  2. Verify that the Mesh size option is set to Average size.
  3. Set the Average element size to 0.006.


    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 column.

Define Nodal Output Frequency

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


    Figure 20.
    The Field Output dialog opens.
  2. Click the Solution variables setting.
  3. Activate the Write initial conditions option.
  4. Verify that the Write results at time step interval option is active.
  5. Set the Time step interval to 5.


    Figure 21.

Define the Nodal Initial Conditions

  1. From the Solution ribbon, Initialize tools, click the Box tool.


    Figure 22.
  2. Hover the cursor over the dam geometry. When the zone is aligned with the surfaces of the model, double-click on the geometry.
    An initialization zone with arbitrary dimensions should be visible on the model.


    Figure 23.
  3. In the microdialog, select Fluid then click in empty space in the dialog. Change the Value field to Water.


    Figure 24.
  4. In the zone initialization microdialog, expand the drop-down and set the dimensions of the zone as shown in the figure below.


    Figure 25.
    Note: If you do not see the microdialog for entering the dimensions, move the NIC variable microdialog.
  5. Click the center of the manipulator on the model, as shown in the figure below, then enter the following coordinates for the center: 0.028575, 0.028575, 0.003.


    Figure 26.

    This will ensure that the fluid domain is initialized with a water column at the corner of the dam.

  6. Right-click in the modeling window and select the check mark to exit the tool.

Run AcuSolve

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


    Figure 27.
    The Launch AcuSolve dialog opens.
  2. Set the Parallel processing option to Intel MPI.
  3. Optional: Set the number of processors to 4 or 8 based on availability.
  4. Verify that the Automatically define pressure reference option is active.
  5. Expand the Default initial conditions tab and deactivate the Pre-compute flow option.
  6. Set all the velocity components to 0 and set the Immiscible fluid to Air (if not already set).
  7. Leave the remaining options as default and click Run to launch AcuSolve.


    Figure 28.
    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 AcuSolve solution process.

Post-Process the Results with HyperView

In this step, you will create an animation of the water flow as it surges once the walls restricting the water column are removed.

Open HyperView and Load the Model and Results

  1. Start HyperView from the Windows Start menu by clicking Start > All Programs > Altair <version> > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is DamBreak.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create the Water Flow Animation

  1. Orient the display to the xy-plane by clicking on the Standard Views toolbar.
  2. Click on the Results toolbar to open the Contour panel.
  3. Select Volume_fraction-2-Water (s) as the Result type.
  4. Click Apply to display the volume fraction contour at the first time step.
  5. Click the Legend tab then click Edit Legend.
  6. In the Edit Legend dialog, change the Number of levels to 2 and the Numeric format to Fixed then click OK.


    Figure 29.
  7. On the Animation toolbar, click the Animation Controls icon .
  8. Drag the Max frame Rate slider to 20 fps.
  9. Click the Start/Pause Animation icon to play the animation in the graphics area.

Save the Animation

  1. In the menu area, select Preferences > Export Settings > AVI.
  2. In the Export Settings AVI dialog, set the Frame rate to 20 fps then click OK.
  3. On the ImageCapture toolbar, make sure that the Save Image to File option is On.


  4. Click the Capture Graphics Area Video icon .
    The Save Graphics Area Video As dialog opens.
  5. Navigate to the location where you want to save the file, enter a name of your choice, and click Save.

Summary

In this tutorial, you successfully learned how to set up and solve a multiphase flow problem using HyperWorks CFD and AcuSolve. You started by importing the geometry and then completed the flow set up. Once the volume meshing was done, you specified the field initial conditions for the water column using the zone initialization tool. Once the solution was computed, you post-processed the results in HyperView. Here, you generated an animation of the water flow as it surged once the dam walls were removed.