OS-T: 8000 Trim Analysis using the Stick Model of an Aircraft Wing

Tutorial Level: Advanced This tutorial demonstrates trim analysis using the stick model of a simple aircraft wing.

Before you begin, copy the file(s) used in this tutorial to your working directory.

Stick models are generally used to simplify the representation of an aircraft for aeroelastic analysis.

Preprocessing is done using Altair HyperWorks in the OptiStruct user profile. A structural stick model with existing data is used as a base model and this tutorial demonstrates the creation of entities in the Aeroelasticity domain.

The following exercises are included:
  • Create Panels (CAERO1)
  • Create interpolation splines (SPLINE2)
  • Create rigid body motions for aeroelastic TRIM variables (AESTAT)
  • Define TRIM variables
  • Submit the job
  • View the results

Launch HyperMesh

  1. Launch HyperMesh.
  2. In the New Session window, select HyperMesh from the list of tools.
  3. For Profile, select OptiStruct.
  4. Click Create Session.
    Figure 1. Create New Session


    This loads the user profile, including the appropriate template, menus, and functionalities of HyperMesh relevant for generating models for OptiStruct.

Import the Model

  1. On the menu bar, select File > Import > Solver Deck.
  2. In the Import File window, navigate to and select aeroelasticity_trim_wing_stick.bdf you saved to your working directory.
  3. Click Open.
  4. In the Solver Import Options dialog, ensure the Reader is set to OptiStruct.
    Figure 2. Import Base Model in HyperMesh


  5. Accept the default settings and click Import.
    The base structural stick model is loaded in HyperMesh. The model is comprised of CBAR elements.
    Figure 3. Base Structural Model of Aircraft Wing Stick Model


Open the Aeroelasticity Browser

The Aeroelasticity Browser is useful for upcoming tasks in this tutorial. If the Aeroelasticity is not already on your menu bar, click View > Ribbons > Aeroelasticity to add it.

  1. On the menu bar, click Aeroelasticity.
  2. On the Aeroelasticity ribbon, hover over any tool group and click the satellite icon that appears.
    The Aeroelasticity Browser opens.
    Figure 4. Access the Aeroelasticity Browser


Set Up the Model

Create AEROS Entry

In this step, basic/reference parameters for the simulation are defined through AEROS.

  1. Right-click on the Aeroelasticity Browser and select Create > Controls > AEROS.
    A default collector for AEROS is created.
  2. In the Aeroelasticity Browser, expand AeroModule.
  3. Click on the AEROS collector.
  4. For REFC (Reference chord length), enter 0.1.
  5. For REFB (Reference span), enter 0.55.
  6. For REFS (Reference wing area), enter 0.055.
    Figure 5. Definition of AEROS


Create Grid Points around the Stick Model

Since the base structural model is a stick representation, grid points are created around the stick model as corner points of the panel mesh.

  1. On the menu bar, click Topology.
  2. On the ribbon, click the Create Points and Nodes tool.
    Figure 6. Create Points


  3. Left click anywhere in the modeling window.
    The grid coordinate window opens.
  4. Specify the grid coordinate values, then left-click outside the grid coordinate micro-dialog.
  5. Use this method to create four grid points using the following coordinates:
    Table 1. Coordinates of Grid Points
    Grid Point X Y Z
    1 0.0 0.0 0.0
    2 0.1 0.0 0.0
    3 0.1 0.55 0.0
    4 0.0 0.55 0.0
    Figure 7. Create Grid Points


  6. Right click and exit the tool.
    Figure 8. Grid Points around Stick Model


Create Aeroelasticity Panels

The CAERO1 entry is used to create aeroelasticity panel mesh in the base structural model.

  1. On the Aeroelasticity ribbon, Aero Meshing tool group, click the Panel Mesh tool.
    Figure 9.


  2. Select the Transparent check box.
    The points surrounding the structural model are displayed.
    Figure 10. Open Panel Mesh Tool


  3. Select the end points of the CAERO1 panel mesh so that node 1 and node 4 are along the span direction and node 1 and 2 are along the chord direction. For more information, refer to CAERO1.
    Figure 11 shows the correct selection order.
    Figure 11. Grid Point Selection for CAERO1 Definition


  4. In the microdialog that appears, for Span enter 10. Hit Enter to confirm.
  5. For Chord, enter 5. Hit Enter to confirm.
  6. Click .
    Figure 12. Specify Span and Chord Values in CAERO1 Definition


    The panel mesh is created.
  7. Click to exit the tool.
    Figure 13. Aeroelastic Panel Mesh for the Problem


Create Interpolation SPLINES

In this step, a SPLINE2 entry is created for interpolating motion and/or forces between the aeroelastic and structural domain. The SPLINE2 entry refers to the panels (aeroelastic domain), a node-set (structural domain) and the corresponding CAERO1 entry. The node-set for the structural domain is already available in the base model.

  1. On the Aeroelasticity ribbon, click the Spline tool.
    Figure 14.


    The SPLINE2 creation tool opens.
  2. Click the icon.
  3. For Spline type, select Linear_Spline_2 from the drop-down menu.
    Figure 15. Selection of Linear Spline (SPLINE2)


  4. Reference the aero panels.
    1. In the Aero drop-down menu, select Elements.
      Figure 16. Element Based Selection in Aero Domain


    2. On the model, select the aero panels.
      Figure 17. Selection of Aero Panels on Model


  5. Reference the node-set.
    1. In the Structure drop-down menu, select Sets.
      Figure 18. Set Based Selection in Structural Domain


    2. Click .
    3. In the Advanced selection dialog, select SET1 (structural domain set).
      Figure 19. Selection of Structural Node Set


    4. Click OK.
  6. Reference the CAERO1.
    1. Next to Component, click .
    2. In the dialog, select the CAERO1 previously created.
      Figure 20. Selection of CAERO1 Entry


    3. Click OK then to exit the tool.
  7. Under the Splines section of the Aeroelasticity Browser, right-click and select Rename.
  8. Enter the name SPLINE2.
  9. Reference the existing coordinate system.
    1. For CID, click and select .
    2. In the dialog, select the existing coordinate system.
  10. Specify other parameters as shown in Figure 21.
    Figure 21. SPLINE2 Definition


Create AESTAT Entry

The AESTAT entry specifies rigid body motions which are used as trim variables in the aeroelastic analysis. This is later referenced in the TRIM Bulk Data Entry.

  1. In the Aeroelasticity Browser, right-click on Controls and select Create > AESTAT.
    The AESTAT collector is created.
  2. For Name, enter ANGLEA_AESTAT.
  3. For Label, select ANGLEA from the drop-down list.
    A Degree of Freedom (DoF) for Angle of Attack is created.
    Figure 22. Definition of AESTAT


Define TRIM Entry

In this step, the Mach number, Dynamic pressure, and constraint values for the aerodynamic trim variables are defined.

  1. In the Aeroelasticity Browser, right-click and select Create > Loads > TRIM.
  2. For Name, enter TRIM ANGLEA 0.1 RAD1.
  3. For Q (Dynamic pressure), enter 1500.0.
  4. For NUM_LABEL, enter 1.
  5. Reference AESTAT.
    1. Under TRIM1, for LABEL, click and select .
    2. In the Advanced Selection dialog, choose ANGLEA_AESTAT.
      Figure 23. Reference AESTAT in TRIM Entry


    3. Click Click OK.
    4. For UX, enter 0.1.
      The angle of attack is constrained to 0.1 radians.
      Figure 24. Definition of TRIM Entry


Reference the TRIM Entry in the Subcase

In this step, the TRIM entry is referenced in the subcase.

  1. In the Aeroelasticity Browser, select the TRIM_ANALYSIS subcase.
  2. Under Subcase Definition, for Analysis type select Static Aeroelastic Response from the drop-down menu.
  3. For TRIM, click and select .
  4. In the Advanced Selection dialog, choose TRIM ANGLEA 0.1 RAD1.
  5. Click OK.
    Figure 25.


  6. Under SUBCASE OPTIONS, for Analysis TYPE, select SAERO from the drop-down menu.

Export the Input File

In this step, the input file is exported to the working directory. This file is later solved using OptiStruct as the solver.

  1. From the menu bar, click File > Export > Solver Deck.
  2. Enter a name for the file.
  3. Click Save.
    The Solver Export Options dialog opens.
  4. In the dialog, accept the default options.
  5. Click Export.
    The file is now available in your working directory.
    Figure 26.


Submit the Job

The Altair Compute Console (ACC) is used to submit the job.

  1. In the Windows Start menu, select Start > Altair 2025 > Compute Console.
  2. For Input file, use to browse your working directory for the desired file.
  3. Click Open.
  4. For Options, click .
    1. In the Select Solver Options dialog, click the -nt check box.
    2. Enter 4 for the argument.
    3. Click OK.
    4. Click the -out check box.
  5. Click Apply Selected.
  6. Click Close.
  7. Click Run.
    If the job is successful, the new results files should be in the working directory. If any errors are present, look in the aeroelasticity_trim_wing_stick.out file for error messages that could help debug the input deck.

View the Contour Plot

The following steps describe how to review the results in HyperView.

HyperView is a complete post-processing and visualization environment for finite element analysis (FEA), multi-body system simulation, video, and engineering data.

  1. After you receive the analysis completion message, click Results.
  2. In HyperView, click the Contour panel button .
  3. For Result type, select Displacement (v) from the first drop-down menu.
  4. Select Mag from the second drop-down menu.
  5. Click Apply.
    The resulting contour represents the displacement field for the aeroelastic trim analysis.
    Figure 27. Displacement Contour Plot of Wing Stick Model