WS1-1

WORKSHOP 1

LANDING GEAR STRUT ANALYSIS

NAS120, Workshop 1, January 2005Copyright 2005 MSC.Software Corporation

Problem DescriptionA 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 ν =0.3Landing Load = 7,080 lb

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

Suggested Exercise Steps1. Create a new database and name it strut.db. 2. Import the strut geometry.3. Mesh the strut to create solid elements. 4. Apply Loads and Boundary Conditions.5. Create material properties. 6. Create physical properties.7. Run analysis with MSC.Nastran.8. Read the results into MSC.Patran.9. Plot the Von Mises stress and displacement.

a

b c

d

f

g

Step 1. Create New Database

Create a new database called strut.dba. File / New.b. Enter strut as the file name.c. Click OK.d. Choose Tolerance Based on

Model.e. Select MSC.Nastran as the

Analysis Code.f. Select Structural as the Analysis

Type.g. Click OK.

a

e

Step 2. Import Geometry

Import the parasolid filea. File : Import.b. Select the file

strut.xmt.c. Click Apply.

b

c

a

Step 3. Mesh the Object

Create a solid mesha. Elements: Create / Mesh /

Solid.b. Select the entire solid.c. Deselect Automatic

Calculation under Global Edge Length.

d. Enter 0.5 for the Global Edge Length.

e. Click Apply.f. Click on the Iso2 View

Icon.

a

b

cd

e

f

Step 4. Apply Loads and Boundary Conditions

Create a boundary conditiona. Loads/BCs: Create /

Displacement / Nodal.b. Enter hub cylinder as the

New Set Name.c. Click Input Data.d. Enter <0 0 0> for Translations. e. Click OK.

b

c

d

e

a

Apply the boundary conditiona. Click Select

Application Region.b. For the Geometry Filter

select Geometry.c. Set the Selection Filter

to Surface or Face and select the cylinder at the bottom of the strut, as shown.

d. Click Add.e. Click OK. f. Click Apply.

ae

f

d

b

Step 4. Apply Loads and Boundary Conditions

c

Step 4. Apply Loads and Boundary Conditions

Create a loada. Loads/BCs: Create / Total

Load / Element Uniform.b. Enter landing load as the

New Set Name.c. Click Input Data.d. Enter <0 –7080 0> for Load. e. Click OK.

b

c

d

e

a

Apply the loada. Click Select

Application Region.b. For the Geometry Filter

select Geometry.c. Select the upper circular

surface at the top of the strut, as shown.

d. Click Add.e. Click OK. f. Click Apply.

ae

f

d

b

Step 4. Apply Loads and Boundary Conditions

c

Step 5. Create Material Properties

a

c

b

Create an isotropic materiala. Materials: Create / Isotropic /

Manual Input.b. Enter steel for the Material

Name.c. Click Input Properties.d. Enter 30e6 for the Elastic

Modulus.e. Enter 0.3 for the Poisson

Ratio.f. Click OK. g. Click Apply.

d

gf

e

Step 6. Create Physical Properties

Create physical propertiesa. Properties: Create / 3D / Solid.b. Enter strut as the Property

Set Name.c. Click Input Properties.d. Select steel as the material.e. Click OK.

a

b

c

e

d

Apply the physical propertiesa. Click in the Select

Members box.b. Screen pick the entire

solid as shown.c. Click Add.d. Click Apply.

ac

d

Step 6. Create Physical Properties

b

Step 7. Run Linear Static Analysis

Analyze the modela. Analysis: Analyze / Entire

Model / Full Run.b. Click Solution Type.c. Choose Linear Static as

the Solution Type.d. Click OK.e. Click Apply.

a

b

c

d

e

Step 8. Read Results into MSC.Patran

Attach the results filea. Analysis: Access Results /

Attach XDB / Result Entities.b. Click Select Results File.c. Choose the results file

strut.xdb.d. Click OK. e. Click Apply.

a

b

c

e

d

Step 9. Plot Stress and Displacement

Create a quick plota. Results: Create / Quick Plot.b. Select Stress Tensor as the

Fringe Result.c. Select Displacements,

Translational as the Deformation Result.

d. Click Apply.e. Click on the Iso1 View Icon.

a

d

c

b

e