Carnegie Mellon

Mechanical Engineering

Self-paced learning on the Web


V2 Airplane Wing
Home Course Info Problems Test Problems Students Reference

Vibration #3: Vibration in an Airplane Wing


Introduction: In this example you will execute modal analysis of an airplane wing and find its natural frequencies.

Physical Problem: The wing is uniform along its length with cross sectional area as defined below. It is firmly attached to the body of the airplane at one end.

Problem Description:

The chord of the airfoil has dimensions and orientation as shown in the figure.

·         The wing is made of low density polyethylene with a Young's modulus of 38e3 psi, Poisson's ration of 0.3, and a density of 8.3E-5 lbf-sec2/in4.

Assume the side of the wing connected to the plane is completely fixed in all degrees of freedom. The wing is solid and material properties are constant and isotropic.

·         The flow velocity of air is 2m/s.

·         Objective:

            To determine the natural frequencies of vibration

            To generate animations of these vibrations.




IMPORTANT: Convert all dimensions and forces into SI units.


Starting ANSYS:


·         Click on ANSYS 6.1 in the programs menu.

·         Select Interactive.

·         The following menu comes up. Enter the working directory. All your files will be stored in this directory. Also under Use Default Memory Model make sure the values 64 for Total Workspace, and 32 for Database are entered.  To change these values unclick Use Default Memory Model.



·         Click RUN




·         Go to the ANSYS Utility Menu

·        Click Workplane>WP Settings

·        The following window will appear:



·         Check the Cartesian and Grid Only buttons

Enter the values shown in the figure above.

·         Go to the ANSYS Main Menu.

·        Choose Utility Menu>PlotCtrls>Pan Zoom Rotate… and click on the enlarge button (the big black circle) five times. This will zoom in on the center of the area, and it will be easier to select the appropriate points below.

·         Go to Main Menu>Preprocessor>Modeling>Create>Keypoints>On Working Plane.

Create the keypoints as shown in the figure below:



Note that I have only plotted lines before to make it easier to see the keypoints.

·         Go to Main Menu>Preprocessor>Modeling>Create>Lines>Splines thru Keypoints

Create two splines through the top three and the bottom three splines. The figure should look like the one below:





·         Now create an area enclosed by the two splines. Go to Modeling>Create>Areas>Arbitrary>By Lines.

·         Pick the two splines and click OK. The model should look like the one below.



The modeling of the problem is done for now.




Setting preferences that are relevant to this problem:

Main Menu>Preferences

Turn on Structural filtering.



Hit OK.


·         Choose Preprocessor>Material Props>Material Models



Double click Structural>Linear>Elastic>Isotropic



·         Enter 38000 for Young’s Modulus. Enter 0.3 for Poisson’s Ratio

·         Also, double click Density and input 8.3e-5



Exit Define Behavior




·         As opposed to the standard method we have generated, of choosing element types in the previous stage, we will do so in this meshing section, because it is more intuitive. In this tutorial, we are going to first mesh the cross sectional area, using a 2D mesh.. with 2D element constraints. Then we will extrude this element into a 3D object, and generate a 3D mesh as well, obviously with 3D element constraints. So, we need to define two types of elements:


·         Click Preprocessor>Element Type>Add/Edit/Delete... In the 'Element Types' window that opens click on Add... The following window opens:



·         Click on Structural Mass>Solid and select Quad 4node 42. Click APPLY. Next, choose Brick 8node 45 and hit OK. Close the 'Element types' window.

·         So now we have created the appropriate material model and the element types. Meshing will produce an appropriate model.




Go to Preprocessor>Meshing>Meshtool


Click Set on the line with Global under Size Controls



·         The following window appears. Enter 0.25 for element edge length. Hit OK.



·         Click Mesh, and in the Picking Dialog, choose Pick All. Note that you will likely see a warning. Don’t worry about it. The problem is designed taking into consideration a limit on the number of nodes that the educational version of ANSYS we have. If we make the mesh more fine, then when we extrude the shape, the limit will likely be exceeded. Continue.

·         So far, the mesh should appear as follows:



·         Now, choose Main Menu>Preprocessor>Modeling>Operate>Extrude>Elem Ext Opts

·         Choose 2 (Solid45) for the Element type number and enter 10 for the number of element divisions. Hit OK.



·         Now choose Main Menu>Preprocessor>Modeling>Operate>Extrude>Areas>By XYZ Offset

·         Select Pick All in the selection dialog.



·         Don’t mind the warning. If we were using a full version of ANSYS, we would be able to choose SOLID95 instead.

·         Choose Utility Menu>PlotCtrls>Pan Zoom Rotate. Click on ISO and also on Fit. Hit close.





The firs thing to do is to unselect the Plane42 elements used in the 2D area mesh since they wont be needed/used for the analysis. Choose Utility Menu>Select>Entities.


Choose Elements, By Attributes, Elem Type num, Enter 1 for the number, choose Unselect and hit Apply



·         Next, constraints will be applied to all nodes located where the wing is fixed to the body. Select all nodes at z = 0, then apply displacement constraints:

·         Choose Nodes, By Location, Z Coordinates, enter 0 for the value, choose From Full and hit Apply.




Go to  Preprocessor>Loads>Define Loads>Apply>Structural>Displacement>On Nodes. Pick All in the picking dialog. This will pick all “Selected” Nodes (we just decided that already)


Choose All DOF and hit ok (by leaving the displacement value blank, we assign zero displacement)



·         The model should appear as follows, with new constraints on the end.



·         Finally, we reselect all the nodes. Return to the Select dialog that is still open somewhere.

·         Choose By Num/Pick, click Sele All (Select All) and then click Cancel to close the box.





Go to ANSYS Main Menu>Solution>Analysis Type>New Analysis Choose Modal

·         Choose Main Menu>Solution>Analysis Type>Analysis Options

·         Choose Block Lanczos and then enter 5 for the modes to extract and 5 for the modes to expand. Hit OK.




·         Click OK again.


Go to Solution>Solve>Current LS.


Click OK for the warnings. We already addressed the fact that these warnings are accepted. It is also ok that we did not use the Plane42 element in the analysis, since it was only developed to create the 2D mesh we eventually build off of.


Wait for ANSYS to solve the problem.


Click on OK and close the 'Information' window.





Go to General Postproc>Results Summary




It is ok if your results are slightly different due to mesh uniqueness.


·         Also, we want to animate the separate modal shapes.

·         First, select the first mode. Main Menu>General PostProc>Read Results>First Set

·         Utility Menu>Plot Ctrls>Animate>Mode Shape You can pick Linear or Sinusoidal Below.



·         Choose 30 frames and .25 seconds per frame. Then select Def+undef edge. Hit OK. Watch the first shape:

·         Play with settings if you want. For instance, in that animate dialog that opens, decrease the delay to 5 or so for the animation to be more smooth.

·         To see other modes of vibration, return to General PostProc and this time choose Read Results>Next Set

·         Animate again with Utility Menu>Plot Ctrls>Animate>Mode Shape

·         OK


Here are files for all 5 modes: (click on the image to see/download the file)

Note, I tried to use a view that showed the deformations best. Try ISO for all the animations first if you want.

Also, I plotted all the deformed shapes individually using General PostProc>Plot Results>Deformed Shape
















Home Course Info Problems Test Problems Students Reference
Send mail to the Teaching Staff with questions or comments about this web site.