ACU-T: 4300 Species Transport Modeling

This tutorial provides instructions for modeling species transport 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 from <Altair_installation_directory>\hwcfdsolvers\acusolve\win64\model_files\tutorials\AcuSolve to a local directory. Extract from

Note: This tutorial does not cover the steps related to geometry cleanup and meshing.

Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. It consists of two sections, Cup_Honey and Cup_Main. Honey enters from Cup_Honey to Cup_Main and mixes with water.

Figure 1.

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 HoneyTeaPlug 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 HoneyTeaPlug as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Validate the Geometry

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

    Figure 3.
    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 4.
  2. Press Esc or right-click in the modeling window and swipe the cursor over the green check mark from right to left.
  3. Save the database.

Set Up Flow

Set the General Simulation Parameters

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

    Figure 5.
    The Setup dialog opens.
  2. Under the Physics models setting:
    1. Set Time marching to Transient.
    2. Set the Time step size to 0.125.
    3. Select Laminar as the Turbulence model.
    4. Check the Include Gravitational Acceleration option and set the gravity to 9.81 m/s2 in the z direction.
    5. Set the Number of passive species to 1.

    Figure 6.
  3. Click the Solver controls setting then set the Transient maximum steps to 80.

    Figure 7.
  4. Close the dialog and save the model.

Assign Material Properties

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

    Figure 8.
    The Material Library dialog opens.
  2. Under Settings, click Fluid, then click the My Materials tab.
  3. Click to create a new material.
  4. For density:
    1. Change the type to Piecewise Linear.
    2. Define the Curve fit variable as Species 1.
    3. Click twice under Function then enter 1000 kg/m3 and 1500 kg/m3 in the Y column for the density of water and honey, respectively.

    Figure 9.
  5. Similarly, define the viscosity values for water and honey according to the figure below.

    Figure 10.
  6. Close the material editing dialog, then rename the Fluid material to Honey.

    Figure 11.
  7. From the Flow ribbon, click the Material tool.

    Figure 12.
  8. Select both model volumes.
  9. Select Honey from the Material drop-down menu.

    Figure 13.
  10. On the guide bar, click to execute the command and exit the tool.

Define Flow Boundary Conditions

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

    Figure 14.
  2. Select the top two surfaces highlighted in the figure below then click on the guide bar.

    Figure 15.

Define Nodal Initial Conditions

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

    Figure 16.
  2. Select the volume highlighted below.

    Figure 17.
  3. In the microdialog, click and select Species 1 from the list.
  4. Set the Type to Constant and the Value to 1.

    Figure 18.
  5. Save the model.

Run AcuSolve

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

    Figure 19.
    The Launch AcuSolve dialog opens.
  2. Enter the following text in the additional arguments field: -tlog -lprobe.
    This will instruct AcuSolve to launch the AcuTail and AcuProbe windows, which can be used to monitor the solution as the simulation progresses.
  3. Set the Parallel processing option to Intel MPI.
  4. Optional: Set the number of processors to 4 or 8 based on availability.
  5. Leave the remaining options as default and click Run to launch AcuSolve.

    Figure 20.

Post-Process with AcuProbe

As the solution progresses, the AcuTail and AcuProbe windows are launched automatically. The surface output and residual ratios can be monitored using AcuProbe.

In the AcuProbe window, under the Data Tree, expand Residual Ratio, right-click on Final, and select Plot All.
Note: You might need to click on the toolbar in order to properly display the plot.

Figure 21.

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 22.
  4. From the Post ribbon, click the Slice Planes tool.

    Figure 23.
  5. Select the plane shown in the figure below.

    Figure 24.
  6. In the Post Browser, hide the Slip and Auto surfaces.
  7. In the slice plane microdialog, click to create the slice plane.
  8. In the display properties microdialog, change the Display option to species 1.
  9. Activate the Legend radio button then click and set the Colormap name to Rainbow Uniform.

    Figure 25.
  10. Click on the guide bar.
  11. Make sure that the time scale at bottom of the modeling window is at 1 sec.

    Figure 26.
  12. Adjust the time scale to show 2 sec, 4, sec, 6 sec, 8 sec, and 10 sec.
    The distribution of species 1 (honey) at those times is shown below.

    Figure 27.
  13. In the Post Browser, hide the slice plane and show the Auto and Slip surfaces.
  14. Click the Boundary Groups tool.

    Figure 28.
  15. Select all the surfaces on the model to create a new boundary group.
  16. In the microdialog, move the Transparency slider to the middle to add a transparency effect.

    Figure 29.
  17. Click on the guide bar.
  18. Click the Iso-Surfaces tool.

    Figure 30.
  19. In the Iso-function microdialog, change the Iso Variable to species 1 and set the Iso Value to 0.5

    Figure 31.
  20. Click Calculate then click .

    Figure 32. Distribution of species at 3 sec


In this tutorial, you successfully learned how to set up and solve a simulation involving species transport using HyperWorks CFD. You started by opening the HyperMesh input file with the geometry and then defined the simulation parameters, fluid material, and boundary conditions. Once the solution was computed, you visualized the results of species transport with help of planes and an iso-surface.