Department of Aerospace Engineering

Faculty of Engineering

Universiti Putra Malaysia

Modal and Flutter Analysis of a Square Flat PlateWorkshop

August 2005

Workshop 1 – Modal Analysis of a Flat Plate

Objective: to find the first five natural frequencies and mode shapes of the plate which is used in flutter analysis in M-k pair set definition.

Model Description:

For this example, we use Lanczos method to find the first five natural frequencies and mode shapes of a flat square plate (0.254m x 0.254 m). Figure 1 shows the plate geometry in MSC.Patran environment.

Figure 1 - Flat Square Plate Geometry

Elastic properties of the aluminum plate are stated in Table 1:

Table 1 – Elastic Properties of Aluminum 6061

Elastic Modulus / 6.8947e10 Pa
Shear Modulus / 2.6518e10 Pa
Poisson’s Ratio / 0.3
Density / 2643.4 kg/m3
Plate Thickness / 0.000508 m

Figure 2 - Loads and Boundary Conditions

In this example at Nodes 1, 12, 23, 34, 45 we have neither translation nor rotation (T1, T2, T3, R1, R2, R3 = 0); at all other nodes of the plate the vertical component of the translation (T2) as well horizontal and lateral component of the rotation (R1 and R3) are zero.

Exercise Procedure:

1.Create a new database named prob1.db.

File/New

New Database Name prob1

OK

In the New Model Preferences form, set the following:

Tolerance Default

Analysis Code: MSC/NASTRAN

OK

2.Activate the entity labels by selecting the Show Labels icon on the toolbar.

3.Create a surface.

Geometry

Action:Create

Object:Surface

MethodXYZ

Vector Coordinates List 0.254, 0.254, 0>

Origin Coordinates List [0, 0, 0]

Apply

4.Create the finite element model and mesh the surface.

Finite Elements

Action: Create

Object: Mesh Seed

Type: Uniform

Figure 3 - The surface should resemble the output below.

Number of Elements

Number = 10

Curve List Surface 1.4

(See Figure 3)

Apply

5.Change the number of mesh seeds to 4 and select the right edge.

Finite Elements

Number = 4

Curve List Surface 1.1

(See Figure 3)

Apply

6.Mesh the Surface

Action: Create

Object: Mesh

Type: Surface

Surface ListSurface 1

Apply

Figure 4-The model should appear as below

7.Create a set of material properties for the plate.

Materials

Action: Create

Object: Isotropic

Method: Manual Input

Material Name mat_1

Input Properties...

Elastic Modulus = 6.8947e10

Poisson Ratio = 0.3

Shear Modulus = 2.6518e10

Density = 0.282

OK

Apply

8.Define the plate thickness.

Properties

Action: Create

Dimension: 2D

Type: Shell

Property Set Name plate

Input Properties...

Material Namem:mat_1

(Select from Material Property Sets box.)

Thickness 0.100

OK

Select Members Surface 1

Add

Apply

9.Apply constraints to the model.

Load/BC’s

Action:Create

Object: Displacement

Type: Nodal

New Set NameSeta

Input Data...

Translations <T1 T2 T3><0, 0, 0>

Rotations <R1 R2 R3> <0, 0, 0

Analysis Coordinate Frame Coord 0

OK

Select Application Region...

Geometry FilterFEM

Select NodesNode 1:45:11

Add

OK

Apply

Repeat this action for Setb

Action:Create

Object: Displacement

Type: Nodal

New Set NameSetb

Input Data...

Translations <T1 T2 T3>, 0,>

Rotations <R1 R2 R3> <0, , 0

Analysis Coordinate Frame Coord 0

OK

Select Application Region...

Geometry FilterFEM

Select NodesNode 2:1113:22 24:33 35:44 46:55

Add

OK

Apply

10.Run the analysis.

Due to the fact that only one full run can be done at a time so we analyze this job using analysis deck and after creation of *.bdf file students should queue to run their files and get the result.

Action: Analyze

Object: Entire Model

Method Analysis Deck

Job Nameplate

Translation Parameters...

Data Output: XDB and Print

OK

Solution Type...

Solution Type: NORMAL MODES

Subcase Create...

Available SubcasesDefault

Subcase Parameters...

Number of Desired Roots = 5

OK

Apply

An MSC.Nastran input file called plate.bdf will be generated. The process of translating your model into an input file is called Forward Translation. The Forward Translation is complete when the Heartbeat turns green.

Submitting the input file for analysis:

On these computers the *.bdf files usually will be created in C:\Windows\Temp folder. After the analysis is completed try to locate this file in that folder. Now you have to submit this file which should be named as plate.bdf to Nastran for analysis. From Start Menu find this path: All Programs/MSC.Softeware/ MSC.Nastran NONE/ MSC.Nastran 2005.Run this application. In the dialogue box which will be popped up select plate.bdf as the input file and select open. Now on another dialogue box select run and wait until the beep which demonstrates that the analysis is complete. Go to the same folder (C:\Windows\Temp) and try to find plate.f06 file. Open this file with Notepad and search for the term FATAL. If there is no FATAL in your file, most probably you have done this analysis correctly. Now go back to Patran environment and invoke the analysis button. And follow this procedure:

Action: Analyze

Object: Access Results

Method Attach XDB

Job NameResults Entities

Select Result File …

(Try to find plate.xdb in C:\Windows\Temp folder)

Apply

Now go to Result Menu, you can see the 5 natural frequencies of this plate.

Results

Action: Create

Object: Deformation

Select Results Cases Default, A1: Mode 1: Freq. = 6.7767

Select Deformation Result Eigenvectors, Translational

Apply

Figure 6 – The First Mode Shape

The first five natural frequencies should be the same as following:

1- 6.7767 Hz

2- 42.003 Hz

3- 101.14 Hz

4- 116.44 Hz

5- 185.23 Hz

Workshop 2 – Flutter Analysis of the Flat Plate

Objectives:

  • Obtaining the flutter speed and frequency using MSC.Nastran PK-method.
  • Getting the V-g graph using Microsoft Excel.
  • Getting the V-F graph using Microsoft Excel.

Here we can use either the Graphical User Interface (GUI) or Input file for flutter analysis. The GUI for aeroelastic analysis is MSC.FlighLoads and Dynamics whose environment is actually MSC.Patran with aeroelasticity analysis module added to its analysis preference. Regardless of what method you opt there are three general steps for aeroelastic analysis using MSC.Nastran.

  1. Defining the structural geometry and elements.
  2. Defining the aerodynamic geometry and boxes.
  3. Creating the appropriate splines to interpolate between structural elements and aerodynamic boxes.

The structural geometry and elements have been defined in the previous workshop so we will leave it to the user to work with the same structure or create a new one following the procedure elaborated in the aforementioned exercise. Thus we start our exercise with aerodynamic geometry definition.

Exercise Procedure:

  1. From the Preference Menu, select Analysis and change the analysis type to Aeroelasticity.
  1. Create Aerodynamic Surface

Geometry

Action:Create

Object:Surface

MethodXYZ

Vector Coordinates List 0.254, 0.254, 0>

Origin Coordinates List [0.01, 0.01, 0.01]

(The origin coordinates list should be different from structural geometry)

Apply

  1. Create the Aerodynamic Model

Flight Loads/Aero Modeling/Model Management

Action:Create

Object:SuperGroup

Type:Flat Plate

SuperGroup Name (8 chars)

Aeroelas

Apply

Cancel

Remark: If you don’t assign any name to the SuperGroup the Flight Load will automatically assign AeroSG2D for it as a default

Flight Loads/Aero Modeling/Flat Plate Aero Modeling…

Action:Create

Object:Lifting Surface

Method:Existing Surface

Surface Name

aero

Select Existing Surface

Surface 2

Mesh Control

Span Mesh:Uniform

Number =10

Chord Mesh:Uniform

Number =4

Ok

Apply

Cancel

  1. Define the Aerodynamic Parameters

Flight Loads/Aerodynamic/Global Data

Aero Model:Aeroelas

Full ModelHalf Model

(We will select full model for this exercise)

Reference Span:0.254

Reference Chord:0.254

Densities:SL kg/m3

Reference Density

1.226

OK

Flight Loads/Aerodynamic/Unsteady Aerodynamics…

Action:Create

Create:MK Pair Set

MK Pair Set Name

MK-Flutter

Mach Frequency Pairs…

Mach Set:Uniform

Mach:0.09

Frequency Set:Uniform

Dimensional

Fmin:6.7767

Vmax:50

Fmax:185.23

Vmin:10

Number:8

Add

OK

Apply

Cancel

  1. Fmax and Fmin are referred to first and fifth natural frequencies of the plate respectively.
  2. Vmax and Vmin are referred to maximum speed and minimumspeed of the plate respectively.
  1. Define Splines

Flight Loads/Aeroelasticity/Aero-Structure Coupling…

Action:Create

Object:Surface

Method:General

Spline Name

spline

Structural Points

NodesGroups

Select Groups…

Existing Groups: default_group

Close

Aero Boxes

ElementsSurface

Existing Surface…

Existing Surfaces: aero

Close

Apply

Flight Loads/Aeroelasticity/Aeroelastic Model…

Auto Select Splines

Ok

  1. Aeroelastic Analysis

Flight Loads/Aeroelasticity/Analysis…

Solution Type:Flutter

Subcase Create…

Action:Create

Subcase Name

Flutter

Mach-Frequency Paris…

Mach-Frequency Sets: MK-Flutter

Ok

Flutter Parameters…

XZ Symmetry:Symmetry

XY Symmetry:Symmetry

Method:PK

Mach:0.09
Density Ratio Sets…

Action:Create

Density Ratio Set Name

Density

Input

1

Enter

Apply

Action:Select

Density Ratio Set:

Density

Apply

Velocity Sets…

Action:Create

Velocity Set Name

Velocity

Input

1

Enter

10

Enter

15

.

.

.

50

Enter

Apply

Action:Select

Velocity Set:

Velocity

Apply

OK

Subcase Select…

Subcases for Solution Sequence 145:

Flutter

OK

Job Name

Flutter

Job Parameters…

Run Type:Analysis Deck

(like previous exercise you can choose between Analysis Deck or Full run, but due to the same reason it is strongly advised to choose Analysis Deck and apply *.bdf file which is generated afterward to MSC.Nastran for Analysis).

OK

Run

After the run is complete try to find flutter.bdf in C:\Windows\Temp folder and do the upcoming procedure as previously stated in the modal analysis exercise. Now find flutter.f06 file in the same folder, open it u with Notepad and search for the term FATAL, if you didn’t find any FATAL error messages your procedure is most probably correct. In this file you can find these data for the Mach-Frequency Pairs that you have defined:

KFREQ, 1./KFREQ, VELOCITY, DAMPING, FREQUENCY, COMPLEX EIGENVALUE.

Take a quick look at the results, your flutter will normally occur at the first points. Try to plot velocity against damping for the first 4 points using Microsoft Excel. Flutter will occur when the damping is tending to zero. So the flutter speed value is the point where the graph crosses the velocity axis. This graph is called V-g graph. A Typical V-g graph should resemble this:

In the above graph Flutter occurs at 151 m/s and the corresponding frequency is the Flutter Frequency.

For the square flat plate the V-g and V-F (Velocity – Frequency) graph would be as following; for this example the flutter speed is around 29 m/s and flutter frequency is 35.8356 Hz.

1