# OS-T: 8030 Flutter Analysis of a General Transport Aircraft Model

This tutorial demonstrates the flutter analysis of an a General Transport Aircraft (GTA) model, using the KE method.

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

Preprocessing is done using Altair HyperWorks in the OptiStruct User profile. A model with existing structural and aeroelastic data is used as a base model and this tutorial demonstrates the creation of entities specific to flutter analysis.

Flutter is a dynamic instability in which the aerodynamic loads on a flexible body couple with its natural modes of vibration to produce oscillatory motions with increasing amplitude.

Using flutter analysis, the critical velocity to avoid flutter is identified for a given altitude. Once determined, designers aim to avoid their system nearing this critical velocity.

The following exercises are included:
• Define flutter analysis using the KE method
• Define complex eigenvalue related entries
• Submit the job
• Post-process the results

## Launch HyperWorks and Import the Model

Refer to Access the Model Files for more details about obtaining the tutorial model file. The model file required for this tutorial is aeroelasticity_flutter.fem

1. Copy the model file to your directory.
2. Launch HyperWorks.
3. From the menu bar, click File > Import > Solver Deck.
4. Select the model file and click Open.
5. In the Solver Import Options dialog, for Reader select OptiStruct.
The OptiStruct user profile loads. The functionality of HyperWorks is paired down to the appropriate template, macro menu, and import reader to create models in OptiStruct.
6. Click Import.
The base model is loaded into HyperWorks.

## Open the Aeroelasticity Browser

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

1. In the menu bar, click View > Ribbons > Aeroelasticity.
The Aeroelasticity ribbon appears on the menu bar.
2. On the Aeroelasticity ribbon, hover over any tool group and click the satellite icon that appears.
The Aeroelasticity Browser opens.

## Set Up the Model

### Create AERO Entry

In this step, the AERO entry is created to define the reference parameters.

1. In the Aeroelasticity Browser, expand AeroModule.
2. Right-click on the Controls folder and select Create > AERO.
A collector for AERO is created under Controls.
3. Enter the values for AERO as shown in Figure 4.

### Create MKAERO1 Entries

In this step, the MKAERO1 entry is used to define the Mach number and reduced frequency table. Two MKAERO1 entries are created, since each MKAERO1 entry only allows a maximum of 8 fields.

These values, along with the reference density from the AERO entry are used to calculate the aerodynamic matrix.

1. In the Aeroelasticity Browser, right-click on Controls folder and select Create > MKAERO1.
A collector for MKAERO1 is created under Controls.
2. Enter a name of your choice for the collector.
In this tutorial, the collector is called MKAERO1_1.
3. For Num Mach numbers, enter 1.
4. Enter a single Mach Number of 0.3.
5. For Num Frequency, enter 8.
6. Select .
7. Enter the reduced frequencies as shown in Figure 5.
8. Repeat the process above to create a second MKAERO1 entry.
1. Enter a name of your choice.
In this tutorial, the collector is called MKAERO1_2.
2. Use the values in Figure 6 for the reduced frequencies.

### Create FLFACT Entries

In this step, three FLFACT entries are created to define three sets of aerodynamic factors - Mach number ${M}_{i}$, reduced frequency ${K}_{j}$, and density ratio ${\rho }_{k}$.
1. In the Aeroelasticity Browser, right-click on Controls folder and select Create > FLFACT.
A collector for FLFACT is created under Controls.
2. For FORMAT, select Factors from the drop-down menu.
With this option, you can specify a list of aerodynamic factor values directly.
3. Enter a name of your choice for the collector.
In this tutorial, the collector is called FLFACT_DENS. This entry is used to specify the density ratios.
4. For Num Factors, enter 1.
5. For F (Aerodynamic factor value), enter 1.0.
This defines an FLFACT entry with a single density ratio of 1.0.
6. Repeat the process above to create a second FLFACT entry.
1. Enter a name of your choice for the collector.
In this tutorial, the collector is called FLFACT_MACH. This entry is used to specify the Mach numbers.
2. For Num Factors, enter 1.
3. For F, enter 0.3.
7. Create a third FLFACT entry.
1. For FORMAT, select THRU_FORMAT from the drop-down menu.
This defines the aerodynamic factor values to be defined using initial, final and intermediate values. See the Reference Guide for more details.
2. Enter a name of your choice for the collector.
In this tutorial, the collector is called FLFACT_RFREQ. This entry is used to specify the reduced frequencies.
3. Enter values in the browser as shown in Figure 8.

### Create FLUTTER Entry

In this step, the FLUTTER entry is used to define the flutter analysis setup. The FLFACT entries defined in the previous step are also referenced in this FLUTTER entry.

1. In the Aeroelasticity Browser, right-click on the Aero Loads folder and select Create > Aero Loads > FLUTTER.
2. Enter a name of your choice for the collector.
In this tutorial, the collector is called FLUTTER.
3. For METHOD, select KE from the drop-down menu.
This enables the KE method for flutter analysis.
4. Reference the previously created FLFACT entries.
1. For DENS, click and select .
2. In the Advanced Selection dialog, choose the FLFACT entry you created for the density ratios and click OK.
3. For MACH, select the FLFACT entry you created for the Mach numbers.
4. For RFREQ, select the FLFACT entry you created for the reduced frequencies.
5. For IMETH, select L from the drop-down menu.
This sets the interpolation method to linear.

### Create EIGRL Entry

In flutter analysis, OptiStruct uses the modal approach where the structural-vibration modes in a selected frequency range are used as the degrees of freedom. Hence, the EIGRL Bulk Data Entry is defined.

1. In the Aeroelasticity Browser, expand StructureModule.
2. Right-click on Eigenvalues and select Create > EIGRL.
A collector for EIGRL is created under Eigenvalues.
3. Enter a name of your choice for the collector.
In this tutorial, the collector is called EIGRL.
4. Enter the values as shown in Figure 10 to define the entry.

### Create PARM, VREF Entry

The output of flutter analysis can be postprocessed in the form of Velocity-Damping (V-g) and Velocity-Frequency (V-f) curves. PARAM, VREF can be used to convert the output velocities from flutter analysis to different unit systems.

This model is built in the units of mm, N, sec. The output velocity (in mm/sec) is converted to knots using this parameter.

1. In the Aeroelasticity Browser, expand AeroModule.
2. Right-click on Controls and select Create > PARAM.
A collector for PARAM is created under Controls.
3. In the collector, scroll down and select the VREF check box.
4. For VALUE, enter 514.444.
This divides the output velocity from flutter analysis by a value of 514.444 (mm/sec = $\frac{1}{514.444}$ knots.

### Create Flutter Analysis Subcase

In this step, the previously created Bulk Data Entries are referenced in the Flutter Analysis subcase.

1. In the Aeroelasticity Browser, expand SolutionJobSetup.
2. Right-click on Case Controls and select Create > Subcases.
3. Enter a name of your choice for the collector.
In this tutorial, the collector is called FLUTTER.
4. For Analysis type, select Aerodynamic Flutter from the drop-down menu.
5. Reference the previously created Bulk Data Entries as shown in Figure 11.

## 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.

## Submit the Job

1. In the Windows Start menu, select Start > Altair 2022.2 > 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.

If the job is successful, the new results files should be in the working directory. If any errors are present, look in the aeroelasticity_flutter.out file for error messages that could help debug the input deck.

## Post-Process the Results

### Review Flutter Analysis Summary

The summary from flutter analysis is available by default in the .flt file. This ASCII file can be viewed in any text editor.

In case of the KE method, each POINT corresponds to a mode number. Refer to the .flt file in the Reference Guide and the Flutter Analysis in the User Guide for more details.

By definition, instability (flutter or divergence) occurs when the damping values are zero.

At this point, if the frequency is zero, the instability is due to divergence.

Otherwise, the instability is due to flutter. In the scope of this tutorial (non-zero frequencies), determination of instability due to flutter is explained.

1. Review the damping values in the .flt file.
The instability in each mode occurs whenever damping values change sign from negative to positive (and do not return to negative) with increasing velocity.
2. From this example, look at the 7th mode.
The flutter point occurs between (KFREQ, velocity) = (0.5, 3.430E+02) and (KFREQ, velocity) = (0.6111, 3.087E+02).
3. Determine the modes which show similar changes in damping values to find the flutter point at other modes.
In this tutorial model, flutter points occur at modes 7, 10, 11, and 13.

### Determine Flutter Point from V-g and V-f Plots

The V-g and V-f plots are a more visual and robust way of post-processing. Among all the flutter points determined in the previous step, the flutter point corresponding to the lowest velocity is determined.

1. In the Aeroelasticity Browser, select the Flutter Curves tool.
2. In the Flutter Curves dialog, import the .flt file.
3. Select the curves corresponding to modes 7, 10, 11, and 13.
4. For X Axis, select VELOCITY.
5. For Y Axis, select DAMPING.
6. Select Plot to plot the V-g curve.
7. Determine the flutter points (where damping = 0).
1. Find the flutter point corresponding to the lowest velocity.
In this example, it is identified as the 7th mode (Flutter point A). This is the most critical flutter point that must be avoided.
2. Zoom in further on the plot to determine the velocity at this flutter point is 327.668.
8. In the Flutter Curves dialog, select only the 7th mode.
9. For X Axis, select VELOCITY.
10. For Y Axis, select FREQUENCY.
11. Select Plot to plot the V-f curve.
12. Zoom in on the graph to determine the frequency value for the 7th mode at a velocity of 327.688.
In this tutorial, the frequency value is 13.334.

In this way, the V-g and V-f plots are used to determine the lowest velocity at which flutter occurs. The frequency of the system is then determined. From the density ratio of the flutter mode, you can learn the altitude at which flutter instability occurs. You can then aim to keep the system from nearing this velocity and altitude.