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 tutorial, ACU-T: 1000 Basic Flow Set Up, 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-T4300_HoneyTeaSpecies.hm from HyperWorksCFD_tutorial_inputs.zip.

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 ACU-T4300_HoneyTeaSpecies.hm and click Open.
  4. Click File > Save As.
    The Save File As dialog opens.
  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

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

Set the General Simulation Parameters

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


    Figure 4.
    The Setup dialog opens.
  2. Click the Time setting, change the option to Transient, and set the Time step size is 0.125.


    Figure 5.
  3. Click the Flow setting, then:
    1. Activate the Laminar option.
    2. Check the Include Gravitational Acceleration option.
    3. Set the Gravity value to 9.81 m/s2 in the z direction.


    Figure 6.
  4. Click the Species transport setting then activate the Species checkbox.


    Figure 7.
  5. Click the Solver controls setting then set the Transient maximum steps to 80.


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

Assign Material Properties

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


    Figure 9.
    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 10.
  5. Similarly, define the viscosity values for water and honey according to the figure below.


    Figure 11.
  6. Close the material editing dialog, then rename the Fluid material to Honey.


    Figure 12.
  7. From the Flow ribbon, click the Material tool.


    Figure 13.
  8. Select both model volumes.
  9. Select Honey from the Material drop-down menu.


    Figure 14.
  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 15.
  2. Select the top two surfaces highlighted in the figure below then click on the guide bar.


    Figure 16.

Define Nodal Initial Conditions

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


    Figure 17.
  2. Select the volume highlighted below.


    Figure 18.
  3. In the microdialog, click and select Species 1 from the list.
  4. Set the Type to Constant and the Value to 1.


    Figure 19.
  5. Save the model.

Run AcuSolve

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


    Figure 20.
    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 21.

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 22.

Post-Process the Results with HW-CFD Post

  1. Once the solution is completed, navigate to the Post ribbon.
    Important: In order to access the Post ribbon in HyperWorks CFD, you have to set the following environment variable: HWCFD_Post=1.
  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 23.
  4. From the Post ribbon, click the Slice Planes tool.


    Figure 24.
  5. Select the plane shown in the figure below.


    Figure 25.
  6. In the Post Browser, hide the Slip and Auto surfaces.
  7. Click Slice on the guide bar.
  8. In the 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 26.
  10. Click on the guide bar.
  11. Make sure that the time scale at bottom of the modeling window is at 0 sec.


    Figure 27.
  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 28.
  13. In the Post Browser, hide the slice plane and show the Auto and Slip surfaces.
  14. Click the Boundary Groups tool.


    Figure 29.
  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 30.
  17. Click on the guide bar.
  18. Click the Iso-Surfaces tool.


    Figure 31.
  19. In the Iso-function microdialog, change the Iso Variable to species 1 and set the Iso Value to 0.5


    Figure 32.
  20. Click Calculate then click .


    Figure 33. Distribution of species at 3 sec

Summary

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.