ACU-T: 7010 Shape Optimization using HyperStudy

Prerequisites

Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, and have a basic understanding of HyperMesh, AcuSolve, and HyperView. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

Prior to running through this tutorial, click here to download the tutorial models. Extract ACU-T7010_HyperStudy.hm from HyperMesh_tutorial_inputs.zip.

Since the HyperMesh database (.hm file) contains meshed geometry, this tutorial does not include steps related to geometry import and mesh generation.

Problem Description

The geometry for this problem consists of a simple pipe channel with perfectly circular cross-section as the base shape. Water enters the Inlet at the rate of 0.0003 kg/s and the outlet is a standard pressure outlet at zero relative pressure. Walls of the channel are no-slip walls.

The objective is to generate the pressure drop between the inlet and outlet with the effect of changes in pipe shape. After performing the baseline simulation, a DOE study will be executed to analyze the effect of changes in pipe shape on the pressure drop between inlet and outlet. This is just to illustrate one of the many types of studies that can be done using AcuSolve with HyperMesh and HyperStudy.


Figure 1.

Open the HyperMesh Model Database

  1. Start HyperMesh Desktop and load the AcuSolve user profile.
    Refer to the HM introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, to learn how to select AcuSolve from User Profiles.
  2. Click the Open Model icon located on the standard toolbar.
    The Open Model dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T7010_HyperStudy.hm and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named Pipe_HyperStudy 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 Pipe_HyperStudy as the file name for the database, or choose any name of your preference.
  7. Click Save to create the database.

Specify the Boundary Conditions

In this simulation, you will use the standard simulation parameters and solver settings.

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.

  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Fluid. In the Entity Editor,
    1. Change the Type to FLUID.
    2. Set the Material to Air_HM.


    Figure 2.
  3. Click Inflow. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Change the Inflow type to Mass flux.
    3. Set the Mass flux value to 0.0003 kg/sec.


    Figure 3.
  4. Click Outflow. In the Entity Editor, change the Type to OUTLFOW and leave the remaining options as default.


    Figure 4.
  5. Click Wall. In the Entity Editor, verify that the Type is set to WALL.


    Figure 5.
  6. Save the model.

Set the Optimization Parameters

Generate and Export Morph Shapes

  1. In the panel area, click HyperMorph then select morph volumes.
  2. In the create sub-panel, click the elems collector and select all.
  3. Click create.
    A new morph volume is created.


    Figure 6.
  4. Go to the split/combine sub-panel. In the panel area, toggle the option to # of splits and set it to 3.


    Figure 7.
  5. In the graphics area, select the edge shown in the figure below.


    Figure 8.
  6. In the panel area, click split.
    The morph volume is split into smaller volumes.


    Figure 9.
  7. In the panel area, go to the update edges sub-panel. Click the first arrow and select update ends. Then, click the second arrow and select by mvols. Finally, click the third arrow and select the main-secondary option.


    Figure 10.
  8. Activate the main morphvolmes collector and select the outer two morph volumes shown in the figure below. Then, activate the secondary morphvolumes collector and select the inner two morph volumes.


    Figure 11.
  9. After selecting the volumes in the order mentioned, click update.
    The edges in the volume should resemble the figure shown below.


    Figure 12.
  10. Click return to go the HyperMorph panel. Select morph in the panel area then select the move handles sub-panel. In this panel,
    1. Click the second arrow and change it from interactive to translate.
    2. Below that, click the arrow and select along vector.
    3. Under that, set the orientation selector to y-axis.
    4. In the dist= field, enter 0.01.


    Figure 13.
  11. Activate the handles collector and select the four middle handles as shown in the figure below.


    Figure 14.
  12. In the panel area, click morph.
    The grid is morphed.


    Figure 15.
  13. Go to the save shape sub-panel. In this panel,
    1. Set the name field to shape_1.
    2. In the second row, set the selector to as node perturbations.
    3. Click save.
    4. Select Yes when asked to save perturbations for nodes at global and morph volume handles.
    A new folder named Shapes is created in the Model Browser. The display of the saved shape can be shown or hidden by right-clicking on the shape_1 and selecting the appropriate option.
  14. Click undo all then click return to exit the panel.
  15. Go to the Utility Menu.
    If you do not see the utility menu, click View on the menu bar and select Browsers > HyperMesh > Utility from the drop-down.
  16. In the utility menu, click Disp then click Clear Temp Nodes to remove any temporary nodes in the model.

Define the Design Variable

  1. Click Design Study on the menu bar and select Define DV from the drop-down.
  2. In the panel area, in the desvar sub-panel, enter bend as the name in the desvar= field.
  3. Click on the shape= field and select shape_1.
  4. Click create to create a design variable named 'bend'.


    Figure 16.
  5. Click return to exit the panel.
  6. Save the model.

Launch the DOE Study Using HyperStudy

Start the Nominal Run

  1. Click on the CFD toolbar.
    The HyperStudy Job Launcher dialog.
  2. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  3. Verify that the Solver is set to AcuSolve.
  4. In the Define Responses table, select the following to identify what the pressure change will be at inflow due to shape changes.
    1. Set Responses to Pressure.
    2. Set Components to Inflow.
  5. Verify that both Launch HyperStudy without nominal run and Export options are left unchecked.
  6. Click Launch.


    Figure 17.
  7. Click Yes in the prompt that appears.
A nominal run is launched and the AcuTail and AcuProbe windows are launched automatically. Once the nominal run is completed, the HyperStudy window is launched.

In the HyperStudy window, check step by step by clicking on each setup from the Explorer menu to ensure that everything was properly defined.

Run the DOE Study

  1. In the Explorer window, right-click on Study 1 and select Add.


    Figure 18.
  2. In the Add – Altair HyperStudy dialog, select DOE then click OK.
    A new study folder named DOE 1 is created in the Explorer.
  3. In the Explorer, click Specifications under DOE 1.
  4. In the Work Area, set the Mode to Full Factorial by expanding the Show more… option.


    Figure 19.
  5. Click the Levels tab, set the number of levels to 5, then click Apply.


    Figure 20.
  6. In the Explorer, click Evaluate under DOE 1.
    The table used to run the study appears, showing all of the runs (1 - 5) to be executed.


    Figure 21.
  7. Click Evaluate Tasks at the bottom of the Work Area.
    As the runs progress, the status of each run will be updated in the table in the Work Area.
  8. Once all the runs are complete, click the Evaluation Data tab.
    The table displays the list of values used for the design variable and also the corresponding value of the response variable (inflow pressure).


    Figure 22.
  9. In order to view the above table as a plot, click the Evaluation Plot tab.
  10. Plot the values of the response variable (inflow pressure) by selecting it in the Channel selector.


    Figure 23.

    You can also plot the list of design variables by switching the label to bend.

Post-Process the Results with HyperView

Switch to the HyperView Interface and Load the AcuSolve Model and Results

  1. In the HyperMesh Desktop window, click the ClientSelector drop-down in the bottom-left corner of the graphics window.


    Figure 24.
  2. Select HyperView from the list.
  3. In the pop-up dialog that appears, click Yes.
    The interface is changed to HyperView.

    Once HyperView is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.

  4. In the Load model and results panel, click next to Load model.
  5. In the Load Model File dialog, navigate to your working directory and then navigate into the following directory …\approaches\doe_1\run_00001\m_1\. Select the Pipe_HyperStudy.1.Log file.
  6. Click Open.
  7. Click Apply in the panel area to load the model and results of the first run of the DOE study.
    The model is colored by geometry after loading.

Create a Pressure Contour on a Cut Plane

In this step, you will create a contour plot of pressure on a section cut on the z-axis.
  1. Click on the Results toolbar to open the Contour panel.
  2. In the panel area, change the Result type to Pressure (s).
  3. Click Apply to create a pressure contour plot.
  4. Click the Section cut icon on the HV-Display toolbar.
  5. In the panel area, click Add to create a new section cut named Section 1.
  6. In the Define plane section, set the axis to Z Axis then click Apply.
  7. Set the Z Base coordinate to 0 and press Enter.
  8. Click Gridline. In the Gridline Options dialog, deactivate the Show check box under Grid line then click OK.


    Figure 25.
  9. Orient the display to the xy-plane by clicking on the Standard Views toolbar.


    Figure 26. Run 1
  10. Repeat the above steps to create a contour plot of pressure for each individual run using the respective log files.


    Figure 27. Run 2


    Figure 28. Run 3


    Figure 29. Run 4


    Figure 30. Run 5

Summary

This tutorial introduced you to running a DOE study using Altair products, namely HyperMesh, AcuSolve, HyperStudy and HyperView. You started by importing a HyperMesh database and then set up the simulation parameters for AcuSolve and created a morph shape using HyperMorph. Next, you set up the design variable and linked the morph shape to it. Then, you proceeded to set up the DOE study. Once the results were obtained, you processed the results using HyperView.