Flutter Analysis Walkthrough

FEMAP Flutter Analysis Example

This example will demonstrate how to create the "Aerodynamic model" and specify some analysis parameters used to perform a flutter analysis using NX Nastran. Topics discussed will be:

1. Create an "Aero Panel" (CAERO1 and PAERO1) to represent the "Aeroelastic Model" for the flutter analysis, then connect the "Aero Panel" to nodes of the "Structural Model" using an Aero Spline (SPLINE1).
   
2. Set up a "Mach Number vs. Frequency" function in FEMAP to represent the MKAERO2 cards in NX Nastran. Also, create 3 "vs. Aerodynamic Factor" functions in FEMAP to specify the Mach Numbers, Densities, and Velocities (FLFACT cards) used by the PK-Method for Flutter Analysis.
   
3. Create an Analysis Set in FEMAP for the Flutter Analysis. This includes specifying the number of modes to recover, as well as Flutter specific values which will appear on the AERO and FLUTTER cards.
   
4. Interrogate the NX Nastran printed output file (.f06 file) to determine the mode and velocity at which Flutter is occurring. Once determined, make a small change to the list of velocities and run the analysis again to recover complex mode results.
   
5. Expand the results of a particular complex mode within FEMAP to visualize the flutter mode shape.
   

Part 1: Import of an existing structural model

Use the "File, Import, FEMAP Neutral" command, select "Flutter Base.neu", then click Open. In the "Neutral File Read Options" dialog box, be sure to click OK. A model of a simple wing should now be visible. Save the model using "File, Save As". Remember the "save" directory, you will need it later.

Notice, the wing is "flying" in the -X direction. Also, the nodes at the "root" of the wing are fully constrained.

Part 2: Creating the Aero Panel, Aero Property, and Aero Spline

1. Right-click anywhere in the Graphics Window and select "Snap to Node" from the menu.
   
2. Select the "Model, Aeroelasticity, Panel/Body" command. Alternatively, open the "Aero Model" branch in the Model Info tree, right-click on "Panels/Body" heading and select "New" from the context-sensitive menu which appears. The following dialog box will appear: 
   
   
   
1. Click the "Aero Property" icon button next to the Property drop-down list. In the "Create Aero Property" dialog box, simply enter "Wing" into the Title field and click OK.
2. In the Surface section, place the cursor in the X field of Point 1, then select the node on the leading edge at the "root" of the wing (Node 18). Next, place the cursor in the X field of Point 4, then select the node on the leading edge at the "tip" of the wing (Node 263).
   
3. For "Edge Chord 1-2", enter a value of 72.0 and for "Edge Chord 4-3", enter a value of 36.0. If you do not know the lengths when creating the panel, you can use the "Measure Distance" icon button next to the "Edge Chord..." fields to pick 2 locations and get a distance.
4. In the "Mesh Control" Section, for "Number Chord", enter a value of 10 and for "Number Span", enter a value of 16.
   
5. Enter a Title (for example, "Flutter Wing Panel"). Click OK, then click Cancel.
3. Select the "Model, Aeroelasticity, Spline" command. Alternatively, open the "Aero Model" branch in the Model Info tree, right-click on "Splines" heading and select "New" from the context-sensitive menu which appears. The following dialog box will appear:
   
   
   
1. In the "Spline" section, click the "Select Aero Panel/Body" icon button (2nd icon button to the right next to CAERO ID field). In the "Select Aero Panel for Aero Spline" dialog box, select the Aero Panel created in the previous step, then click OK.
   
2. In the "Aerodynamic Points" section, click the "All Boxes" button. This will choose all the "Aero Boxes" of the selected "Aero Panel/Body". If you only wanted certain "Aero Boxes" to be connected using the spline, you would want to enter the aero box numbers manually or place the cursor into the "Box1" or "Box2" field and graphically select aero boxes from the model.
   
3. In the "Structural Grid Group" section, select the group "5..Spline Nodes" from the "ID" drop-down. If you want to see which nodes are included in the group, click the "Show When Selected" icon button (icon button next to "ID" drop-down). Click the icon button again to turn off the highlighting.
   
4. In the "Usage" section, change the option to "Both".
5. Give the Spline a Title (for example, "Spline for Panel 1"). Click OK, then Cancel.
   

Part 3: Using FEMAP functions to specify input values for Flutter Analysis.

1. Select the "Model, Function" command. This function will represent the Mach Number - Frequency Table used by NX Nastran (creates multiple MKAERO2 entries). In the "Function Definition" dialog box:
   
1. Enter a Title of "MKAERO"
   
2. Select "34..Mach Number vs. Freq" from the "Type" drop-down.
   
3. In the "Data Entry" section, select "Single Value" and enter "X" = 0.001, "Y" = 0.8 and click "Add" button.
   
4. In "Data Entry" section, change option to "Linear Ramp". Enter "X" = 0.1, "To X" = 1.0, "Y" = 0.8, "To Y" = 0.8, and "Delta X" = 0.1, then click "Add" button. Click OK.
   
2. The next function will represent the Mach Number(s) (creates a FLFACT entry) used as Aerodynamic Physical Data for Flutter Analysis. In the "Function Definition" dialog box:
   
1. Enter a Title of "Mach Number"
   
2. Select "35..vs. Aerodynamic Factor" from the "Type" drop-down.
   
3. In the "Data Entry" section, select "Single Value". Enter "X" = 0.8, then click "Add" button. Click OK.
   
3. The next function will represent the Density Ratio(s) (creates a FLFACT entry) used as Aerodynamic Physical Data for Flutter Analysis. In the "Function Definition" dialog box:
   
1. Enter a Title of "Density"
   
2. Select "35..vs. Aerodynamic Factor" from the "Type" drop-down.
   
3. In the "Data Entry" section, select "Single Value". Enter "X" = 0.3106, then click "Add" button. Click OK.
   
4. This density Ratio corresponds to a standard atmosphere altitude of 35,000 ft.
   
4. The final function will represent the Velocities (creates a FLFACT entry) used as Aerodynamic Physical Data for Flutter Analysis. In the "Function Definition" dialog box:
   
1. Enter a Title of "Velocities"
   
2. Select "35..vs. Aerodynamic Factor" from the "Type" drop-down.
   
3. In the "Data Entry" section, select "Linear Ramp". Enter "X" = 120, "To X" = 12,000, and "Delta X" = 120 then click "Add" button. Click OK, then Cancel.
   
4. These Velocities represent speeds of 120 in/sec to 12,000 in/sec.
   

Part 4: Setting up the Analysis Set for Flutter Analysis

1. Select the "Model, Analysis" command. Click the "New" button. In the "Analysis Set" dialog box:
   
1. Enter a Title of "Flutter"
2. Using the "Analysis Type" drop-down, select "26..Aerodynamic Flutter"
   
3. Click OK
   
2. Expand the "Options" branch. Highlight "Modal/Buckling", then click "Edit". In the "NASTRAN Modal Analysis" dialog box:
   
1. In the "Eigenvalues and Eigenvectors" section, change the value of "Number Desired" to 8.
   
2. Click "Next" button.
   
3. In the "NASTRAN Aerodynamic Data (AEROx, MKAEROx)" dialog box:
   
1. For "Ref Length", enter a value of 114.0 and for "Ref Density", enter a value of 1.1462E-7
   
2. Using the "Mach Number Func" drop-down, select "1..MKAERO".

   
3. Click OK.
   
4. Expand the "Master Requests and Conditions" branch. Highlight "Master Requests and Conditions ", then click "Edit". In the "Master Requests and Conditions" dialog box:
   
1. Click the "End Text (Off)" button.
   
2. Enter the following line into the "Analysis Text" dialog box: LINE=50000
   
3. Click OK, then click "Next" button.
   
5. In the "NASTRAN Flutter Parameters" dialog box:
   
1. Check the "Enable Flutter" check box.
   
2. Select "1..PK-Method" from the "Flutter" drop-down.
   
3. Select "3..Density" from the "Density Ratios" drop-down.
   
4. Select "2..Mach Number" from the "Mach Numbers" drop-down.
   
5. Select "4..Velocities" from the "Velocity/Reduced Freq" drop-down.

   
6. Click "Next" button 2 times
   
6. In the "Nastran Output Requests" dialog box:
   
1. Un-check the "Constraint Forces" and "Stress" check boxes (i.e., only "Displacement" should be selected).
   
2. Click OK
   
7. In the "Analysis Set Manager", click the "Analyze" button to run the Flutter Analysis.
   

Part 5: Reviewing the "Flutter Summary" in the Printed Output file (.f06 file)

1. Open the .f06 file created from the Nastran Analysis using a text editor. Depending on your setting for "Direct Output To" on the "Interfaces" tab of the "Preferences" dialog box ("File, Preferences" command), the .f06 file you are looking for will either be in "Current Directory", the "Model File Directory" (default), or "Specified Directory" (a specific directory chosen by the user).
   
2. Scroll down or "Search" until you get to the "FLUTTER SUMMARY" section (if searching, there are 2 spaces between the words FLUTTER and SUMMARY). Each "POINT" represents a mode. The values of interest in these tables are the DAMPING and VELOCITY values. If the DAMPING value is negative, no flutter is occurring at that VELOCITY for the given mode. When/if the DAMPING value goes positive, flutter is occurring. In this example, the only "positive" DAMPING values are in "POINT = 2" (Mode 2) and begin at a VELOCITY of 11,520 in/s. Make a note of the first positive DAMPING value for each POINT, then close the .f06 file.
   

Part 6: Modifying the Velocity Input and Running the Model Again

1. In FEMAP, select the "Modify, Edit, Function" command. Select "4..Velocities" from the list and click OK.
   
1. Locate the "first positive DAMPING value" (11520) in the list of function values, then click the value in the list.
   
2. Change the "X" value to -11520, then click the "Update" button; the negative value in the list of velocities is used to request Complex Modal Results at the specified velocity for each requested mode.
   
3. Click OK
   
2. Select "Modal, Analysis" and click the "Analyze" button in the "Analysis Set Manager" to run the analysis again. If using "Femap with NX Nastran", the results will either be directly imported into FEMAP automatically or you will need to click the "Load Results" button in the "NX Nastran Analysis Monitor" pane. If running stand-alone NX Nastran, you will want to use the "File, Import, Analysis Results" command and select the .op2 file from the second set of Nastran files in the directory.

Part 7: Expanding the Complex Modal Results to visualize the Flutter Mode Shape

1. Select "Model, Output, Expand Complex" command. Since the first "positive" DAMPING value occurred in "POINT = 2", expand "Mode 2". In the "Expand Complex Output Data" dialog box:
   
1. Select "2..Mode 2..." from the "Output Set" drop-down in the "From" section.
   
2. Enter a value of 15 for "Increment" in the "Expand For" section.

   
3. Click OK. This command will create 24 additional Output Sets in the model.
   
2. Select the "View, Select" command (or use F5 key) to open the "View Select" dialog box.
   
1. Choose the "Animate-MultiSet" option in the "Deformed Style" section.
   
2. Click "Deformed and Contour Data" button. Using the drop-down in the "Output Set" section, select "9..Freq 4.315, Phase 0" (if you have imported additional results somehow, look for the output set which has "Freq 4.315, Phase 0" in the title).
   
3. Using the drop-down in the "Final Output Set" drop-down, select "32..Freq 4.315, Phase 345" (if you have imported additional results somehow, look for the output set which has "Freq 4.315, Phase 345" in the title).
   
4. Click OK, then click OK again.
   

The model should now be animating. You will probably want to rotate the model to better visualize the animation of the model. If you would like to "clean-up" the display, use the "View, Visibility" command (or press Ctrl+Q). On the "Entity/Label" tab, click the "All Off" button, then "check" the box next to "Element" in the "Mesh..." section. Click "Done".

This concludes the exercise.

​

• Related Articles

• 5 Things You Should Know About Flutter

  Ben Names Sr. Stress Engineer If you like this article, be sure to check out my webinars: Introduction to Aeroelasticity in Nastran - This recording includes a demonstration of Aerodynamic Flutter, a static aeroelastic analysis, and the benefits of ...

• Dynamic Design Analysis Method (DDAM)

  What is in this webinar? Siemens CAE Solutions Consultant Jay Medeiros will be presenting this webinar on Dynamic Design Analysis Method (DDAM). In this webinar, Jay will cover the following topics: DDAM model setup requirements Simcenter NASTRAN ...

• Model Preparation and Analysis in Femap w/ NX Nastran

  What is in this webinar? This webinar shows a live demonstration of applying loads and constraints to a meshed finite element model (FEM) in Femap, and running a Normal Modes and Static Analyses in the NX Nastran solver. NASTRAN Details and Licensing ...

• Buckling Analysis using Femap w/ Nastran Advanced Nonlinear

  What is in this webinar? In this webinar, Alex Skavdahl will explore post-buckled behavior by running a model far in excess of when it buckles. The advanced non-linear solver can track the post-buckled behavior well into the plastic range. It’s ...

• Advanced Aeroelastics for Full Aircraft

  What is in this webinar? Static Aeroelastic Trim Analysis The first topic to be covered will be how to set up an aeroelastic trim analysis on an entire aircraft, and how to interpret the results. This will include how to setup a control surface, ...