LANDING GEAR STRUT ANALYSIS WORKSHOP 1 LANDING GEAR STRUT ANALYSIS NAS120, Workshop 1, November 2003 WS1-1

Problem Description A landing gear strut has been designed for a new fighter jet. Determine if the landing gear strut has been designed properly to withstand the landing load. E = 30 x 106 psi n =0.3 Landing Load = 7,080 lb

Workshop Objectives Learn the typical workflow of a finite element analysis using MSC.Patran and MSC.Nastran.

Suggested Exercise Steps Create a new database and name it strut.db. Import the strut geometry. Mesh the strut to create solid elements. Apply Loads and Boundary Conditions. Create material properties. Create physical properties. Run analysis with MSC.Nastran. Read the results into MSC.Patran. Plot the Von Mises stress and displacement.

Step 1. Create New Database Create a new database called strut.db File / New. Enter strut as the file name. Click OK. Choose Tolerance Based on Model. Select MSC.Nastran as the Analysis Code. Select Structural as the Analysis Type. d e f b c g

Step 2. Import Geometry a b c Import the parasolid file File : Import. Select the file strut.xmt. Click Apply. c

Step 3. Mesh the Object f a b c d e Create a solid mesh Elements: Create / Mesh / Solid. Select the entire solid. Deselect Automatic Calculation under Global Edge Length. Enter 0.5 for the Global Edge Length. Click Apply. Click on the Iso2 View Icon. a b c d e

Step 4. Apply Loads and Boundary Conditions Create a boundary condition Loads/BCs: Create / Displacement / Nodal. Enter hub cylinder as the New Set Name. Click Input Data. Enter <0 0 0> for Translations. Click OK. a d b c e

Step 4. Apply Loads and Boundary Conditions Apply the boundary condition Click Select Application Region. For the Geometry Filter select Geometry. Set the Selection Filter to Surface or Face and select the cylinder at the bottom of the strut, as shown. Click Add. Click OK. Click Apply. b c d a e f

Step 4. Apply Loads and Boundary Conditions Create a load Loads/BCs: Create / Total Load / Element Uniform. Enter landing load as the New Set Name. Click Input Data. Enter <0 –7080 0> for Load. Click OK. a d b c e

Step 4. Apply Loads and Boundary Conditions Apply the load Click Select Application Region. For the Geometry Filter select Geometry. Select the upper circular surface at the top of the strut, as shown. Click Add. Click OK. Click Apply. b c d a e f

Step 5. Create Material Properties Create an isotropic material Materials: Create / Isotropic / Manual Input. Enter steel for the Material Name. Click Input Properties. Enter 30e6 for the Elastic Modulus. Enter 0.3 for the Poisson Ratio. Click OK. Click Apply. a d e b c f g

Step 6. Create Physical Properties Properties: Create / 3D / Solid. Enter strut as the Property Set Name. Click Input Properties. Select steel as the material. Click OK. a d b c e

Step 6. Create Physical Properties Apply the physical properties Click in the Select Members box. Screen pick the entire solid as shown. Click Add. Click Apply. b a c d

Step 7. Run Linear Static Analysis Analyze the model Analysis: Analyze / Entire Model / Full Run. Click Solution Type. Choose Linear Static as the Solution Type. Click OK. Click Apply. a c b d e

Step 8. Read Results into MSC.Patran Attach the results file Analysis: Access Results / Attach XDB / Result Entities. Click Select Results File. Choose the results file strut.xdb. Click OK. Click Apply. a c d b e

Step 9. Plot Stress and Displacement Create a quick plot Results: Create / Quick Plot. Select Stress Tensor as the Fringe Result. Select Displacements, Translational as the Deformation Result. Click Apply. Click on the Iso1 View Icon. a b c d