OS-T: 8010 Trim Analysis of a Full Aircraft Model

This tutorial demonstrates trim analysis of a full aircraft model.

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

Preprocessing is done using Altair HyperMesh in the Nastran MSC User profile. A structural 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 Panel Mesh divisions (AEFACT)
  • Create Panels (CAERO1)
  • Ceate aeroelasticity box list (AELIST)
  • Create interpolation splines (SPLINE1)
  • Create rigid body motions for aeroelastic TRIM variables (AESTAT)
  • Create aerodynamic control surfaces (AESURF)
  • Define TRIM variables and link control surfaces (AELINK)
  • Submit the job
  • View the results
Note: HyperMesh is used as the preprocessor in this tutorial. As some aeroelastic entities are not fully supported in HyperMesh, they are manually added to the input file later in the tutorial process.

Launch HyperMesh and Set the Nastran MSC User Profile

  1. Launch HyperMesh.
  2. In the User Profiles dialog, for Application, select Engineering Solutions from the drop-down menu.
  3. Click the Aerospace radio button.
  4. In the drop-down list next to Aerospace, select NastranMSC.


    Figure 1. Aerospace (Nastran MSC) User Profile in HyperMesh
  5. Click OK.
    The Aerospace (NastranMSC) user profile loads. The functionality of HyperMesh is paired down to the correct template, macro menu, and import reader to create aeroelasticity models in Nastran MSC.

Open the Model and Aeroelasticity Browser

The Aeroelasticity Browser is useful for upcoming tasks in this tutorial.

  1. From the menu bar, click File > Import > Solver Deck.
  2. Select the aeroelasticity_trim.bdf file you copied to your working directory.
  3. Click Open.
  4. Click Import.
    The model database is loaded into the HyperMesh session.


    Figure 2. Base Structural Model of an Aircraft
  5. On the menu bar, select Aerospace > Aeroelasticity > Aeroelasticity Browser.
    The Aeroelasticity Browser opens.

Set Up the Model

This section is the main portion of this tutorial; the aeroelastic domain is defined. There are 18 entities total, as shown in Figure 3. The structural domain is shown in light grey.



Figure 3. Entities of Aeroelastic Domain

Create AEROS Entry

In this step, basic/references parameters for the simulation are defined.

  1. In the Aeroelasticity Browser, expand AeroModule.
  2. Right-click on the Controls folder and select Create > AEROS.
    A collector for AEROS is created under Controls.
  3. Click on the AEROS collector.
  4. Define the reference coordinate system identification for rigid body motion.
    1. Click RCSID.
    2. Select the System button.
    3. On the panel, click system.
    4. For id, enter 100. Hit Enter to confirm.
    5. Click proceed.
  5. For REFC (Reference chord length), enter 36.0.
  6. For REFB (Reference span), enter 360.0.
  7. For REFS (Reference wing area), enter 12960.0.


    Figure 4. Definition of AEROS Entry

Create AEFACT Entries

The AEFACT entry is used to create tabular data of division points for the Aero panels; these panels are later referenced in the CAERO1 entry.

  1. Right-click on the Controls folder and select Create > AEFACT.
    A collector for AEFACT is created in the Controls folder.
  2. Click on the AEFACT collector.
  3. For ID, enter 101.
  4. For Name, enter AEFACT_elev_l.
  5. For Num Factors, enter 6.
    A Data D row and table icon appear in the browser.


    Figure 5. Definition of AEFACT Entry
  6. Click .
  7. In the table, enter the information in the following table.
    Table 1. Divisions for Left Horizontal Elevator Aero Panel
    D1 D2 D3 D4 D5 D6
    0 0.08716 0.28208 0.71791 0.91283 1.0
  8. Click Close.
  9. Repeat the process to create AEFACT entries for each Aero panel in the model, using the divisions in the tables below.
    Table 2. Horizontal Elevator
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    102 Right Elevator 0.08716 0.28208 0.71791 0.91283 1.0 0.08716
    Table 3. Horizontal Elevator Tip
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    103 Left (Span) 0 0.03824 0.63813 0.80915 0.92351 0.99999
    104 Left (Chord) 0 0.08716 0.28208 0.71791 0.91283 1.0
    105 Right (Span) 0 0.03824 0.63813 0.80915 0.92351 0.99999
    106 Right (Chord) 0 0.08720 0.2821 0.71790 0.9128 1.0
    Table 4. Horizontal Stabilizer Tip
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    107 Left (Span) 0 0.03824 0.63813 0.80915 0.9235188 0.99999
    108 Left (Chord) 0 0.08720 0.28210 0.71790 0.9128 1.0
    109 Right (Span) 0 0.03824 0.63813 0.80915 0.9235188 0.99999
    110 Right (Chord) 0 0.08720 0.28210 0.7179 0.9128 1.0
    Table 5. Horizontal Stabilizer
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    111 Left Stabilizer 0 0.08716 0.28208 0.71791 0.91283 1.0
    112 Right Stabilizer 0 0.08716 0.28208 0.71791 0.91283 1.0
    Table 6. Rudder
    AEFACT ID D1 D2 D3 D4 D5 D6
    113 0 0.0871677 0.28208 0.71791 0.91283 1.0
    Table 7. Rudder Top
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    114 Span 0 0.09403 0.25484 0.52980 1.0
    115 Chord 0 0.08716 0.28208 0.71791 0.91283 1.0
    Table 8. Rudder Vertical Tip
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    116 Span 0 0.09403 0.25484 0.52980 1.0
    117 Chord 0 0.08716 0.28208 0.71791 0.91283 1.0
    Table 9. Vertical Stabilizer
    AEFACT ID D1 D2 D3 D4 D5 D6 D7 D8
    118 0 0.06147 0.16658 0.34632 0.6536 0.83341 0.93852 0.99999
    Table 10. Wing Aileron
    AEFACT ID Details D1 D2 D3 D4 D5 D6
    119 Left Aileron 0 0.08716 0.28208 0.71791 0.91283 1.0
    120 Right Aileron 0 0.08716 0.28208 0.71791 0.91283 1.0
    Table 11. Wing Outer
    AEFACT ID Details D1 D2 D3 D4 D5 D6 D7 D8 D9 D10 D11
    121 Left 0 0.03824 0.09542 0.18093 0.30879 0.5 0.6912 0.81906 0.90457 0.96175 1.0
    122 Right 0 0.03824 0.09542 0.18093 0.30879 0.5 0.6912 0.81906 0.90457 0.96175 1.0
    Table 12. Wing Inner
    AEFACT ID Details D1 D2 D3 D4 D5 D6 D7 D8 D9 D10 D11
    123 Left 0 0.03824 0.09542 0.18093 0.30879 0.5 0.6912 0.81906 0.90457 0.96175 1.0
    124 Right 0 0.03824 0.09542 0.18093 0.30879 0.5 0.6912 0.81906 0.90457 0.96175 1.0

Create Aeroelasticity Panels

The CAERO1 entry is used to create aeroelasticity panel mesh in the base structure model. The AEFACT entries are used to create divisions in the panel mesh along the chord and span directions.

  1. On the menu bar, click Aerospace > Aeroelasticity > Panel Mesh CAERO1.
  2. In the panel mesh utility, for Points 1-4, select nodes.


    Figure 6. Nodes Selection in CAERO1 Definition
  3. In the panel, verify node list is selected.
  4. 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 7 shows the correct selection order.


    Figure 7. Selection Order of Nodes for CAERO1 Definition
  5. Click proceed.
  6. Select the AEFACT entry along the chord and span.
    1. In the panel mesh utility, click the Chord Table check box.
    2. Click AEFACT Chord.
    3. In the pop-up, select the corresponding AEFACT entry.
    4. Similarly, click the Span Table check box to select an AEFACT entry for span.


    Figure 8. Definition of Chord and Span Tables in CAERO1
  7. Repeat the above process using Figure 9 as a reference for point selection.
    The structural domain is greyed out for better visibility.


    Figure 9. CAERO1 Definitions for Different Parts of the Aircraft

Create Aeroelasticity Box Lists

The AELIST entry is used to create lists of aeroelasticity boxes from the panel mesh (CAERO1).

  1. In the Aeroelasticity Browser, right-click on the Aero Sets folder and select Create > AELIST.
    A collector for AELIST is created under Aero Sets.
  2. Next to Entity IDs, click and select Elements.
  3. In the panel, click elems and choose a method of element selection.
  4. Select elements corresponding to one of the CAERO1 collectors.
  5. When selection is finished, click proceed.


    Figure 10. AELIST Definition
  6. Use this process to create AELIST entries for each of the CAERO1 collectors.


    Figure 11. Selection of Elements for Each AELIST

Create Interpolation SPLINES

In this step, SPLINE1 entries are created for interpolating motion and/or forces between the aeroelastic and structural domains. Each SPLINE1 entry is reference to an AELIST set (aeroelastic domain), a node set (structural domain) and the corresponding CAERO1 entry. 18 SPLINE1 entries are created for each of the 18 entities in the aeroelastic domain. The node set for the structural domain is already available in the base model.

  1. In the Aeroelasticity Browser, right-click on Splines and select Create > SPLINE2.
    The SPLINE2 collector is created.
  2. For Name, enter wing outer (left).
  3. Reference the AELIST.
    1. Next to Aero Surface, click and select Sets.
    2. In the dialog, select the corresponding AESTAT entry.


      Figure 12. Reference AELIST in SPLINE1
    3. Click OK.
  4. Reference the node-set.
    1. Next to Struct Surface, click and select Sets.
    2. In the dialog, select the corresponding structural set already present in the model.


      Figure 13. Reference SET1 in SPLINE1
    3. Click OK.
  5. Reference the CAERO1.
    1. Next to CAERO, click and select Component.
    2. In the dialog, select the corresponding CAERO1 entry.


      Figure 14. Reference CAERO1 in SPLINE1
    3. Click OK.
  6. Repeat this process for each of the 18 entities in the aeroelastic domain.


    Figure 15. SPLINE1 Entities for the Model

Create AESTAT Entries

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.
  4. Use this process to create AESTAT entries for each DoF. For more information, refer to AESTAT.


    Figure 16. AESTAT Entries Defined in Model

Create AESURF Entries

In this step, the aerodynamic control surface is defined.

  1. Create 5 AELIST sets corresponding to the entitites in Figure 17.


    Figure 17. Additional AELIST for AESURF
  2. In the Aeroelasticity Browser, right-click on Control Surface and select Create.
    The AESURF collector is created.
  3. For Name, enter AILR_R.
  4. Next to Control Surf 1, click and select Sets.
  5. In the pop-up window, choose the AELIST corresponding to the right wing alieron.


    Figure 18. Select the AELIST for AESURF
  6. Next to CID1, click and select System.
  7. In the pop-up window, click system and for ID enter 28.
  8. Click proceed.
  9. For EFF, enter 1.0.
  10. For PLLIM, enter -1.5708.
  11. For PULIM, enter 1.5708
  12. Repeat this process to create additional AESURF entries using the information in Table 13.
    Table 13. AESURF Details
    AESURF Name Linked AELIST CID1
    AILR_L For AESURF - wing aileron (left) 29
    ELEV_L For AESURF - horizontal elevator + tip (left) 30
    ELEV_R For AESURF - horizontal elevator + tip (right) 31
    RUDDER For AESURF - rudder + top 32
  13. Use the same EFF, PLLIM, and PULIM values for all entries.
  14. Verify the name of each AESURFentry exactly matches what is specified in this tutorial.
    This is important, as the names are referenced later in AELINK entries.

Export the Input File and Add Aeroelastic Entities

In the following steps, certain entities which are not fully supported in HyperMesh are added to the input file manually using a text editor.

Export the Input File

  1. From the menu bar, click File > Export > Solver Deck.
  2. In the Export browser, click .
  3. Enter a name for the file.
  4. Click Save.
  5. Accept the default export options.
  6. Click Export.


    Figure 19. Export Input File from HyperMesh

Define TRIM Entry

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

  1. From your file directory, open the input file in a text editor.
  2. In the Bulk Data section (after the "BEGIN BULK" keywords), paste the following snippet. 
    $--1---><---2--><---3--><---4--><--5---><--6---><---7--><--8---><---9-->
TRIM    1       .4      1.65    ROLL    0.      PITCH   0.
        YAW     0.      URDD2   0.      URDD3   -1.     URDD4   0.
        URDD5   0.      URDD6   0.
  3. Save the input file.

Define AELINK Entry

In this step, the AELINK entries are used to define relationships between the AESURF entries.

  1. In the Bulk Data section (after the "BEGIN BULK" keywords), paste the following snippet in the input file. 
    $--1---><---2--><---3--><---4--><--5---><--6---><---7--><--8---><---9-->
AELINK  1       AILR_L   AILR_R   -1.
AELINK  1       ELEV_L   ELEV_R   1.
  2. Save the file.
    Note: The ID of the AELINK must match the ID of the referenced TRIM entry.

Define Aeroelastic Subcase Information Entries

In this step,
  • The TRIM Bulk Data Entry is referenced in the subcase.
  • Aeroelastic output requests are added.
  • Symmetry flags are added.
  1. In the Bulk Data section (after the "BEGIN BULK" keywords), paste the following snippet in the input file. 
    TRIM = 1
 AESYMXZ = Asymmetric
 AESYMXY = Asymmetric
 AEROF = ALL
 APRES = ALL
  2. Save the file.

Perform Corrections to the Input File

Due to some HyperMesh export issues, the input file requires some manual correction. These issues will be addressed in future releases.

  1. In SPLINE1, check that BOX1 ID and BOX2 ID match the upper and lower bounds of the corresponding CAERO1 entries.
    1. If the bounds are incorrect, review the CAERO1 entries and correct them in SPLINE1.
  2. In SPLINE1 verify that BOX1 ID < BOX2 ID.
    1. If the values are incorrect, swap them accordingly.
  3. Change the value of EFF in AESURF from 0.0 to 0.1.

Submit the Job

  1. In the Windows Start menu, select Start > Altair 2022.1 > 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 8 for the argument.
    3. Click OK.
    4. Click the -out check box.
  5. Click Apply Selected.
  6. Click Close.
  7. Click Run.


    Figure 20. Altair Compute Console

    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.out file for error messages that could help debug the input deck.

View the Contour Plot

  1. After you receive the analysis completion message, click Results.


    Figure 21. Altair Compute Console Solver View Window
  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 22. Displacement Contour Plot of the Aircraft