WS1-1 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation WORKSHOP 1 LANDING GEAR STRUT ANALYSIS. - презентация

1 WS1-1 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation WORKSHOP 1 LANDING GEAR STRUT ANALYSIS

2 WS1-2 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation

3 WS1-3 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation l Workshop Objectives: l Run a linear static analysis from beginning to end to learn the workflow of a typical finite element analysis using MSC.Nastran and MSC.Patran. l Problem Description: l 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. Strut material: Steel with E = 30 x 10 6 psi and =0.3 l Landing Load = 7,080 lb

4 WS1-4 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation l Suggested Exercise Steps 1. 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. Open and review the.f06 file. 9. Read the results into MSC.Patran. 10. Plot the Von Mises stress and displacement.

5 WS1-5 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a b c d f g Step 1. Create New Database Create a new database called strut.db a.File / New. b.Enter strut as the file name. c.Click OK. d.Set Tolerance to Based on Model. e.Select MSC.Nastran as the Analysis Code. f.Select Structural as the Analysis Type. g.Click OK. a e

6 WS1-6 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Import Geometry Import the parasolid file a.File : Import. b.Select the file strut.xmt. c.Click Apply and answer OK. b c a

7 WS1-7 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation b d e a Step 3. Mesh the geometry Create a solid mesh a.Click on the Iso2 View Icon. b.Elements: Create / Mesh / Solid. c.Screen pick the solid. d.Enter 0.5 for the Global Edge Length. e.Click Apply. c

8 WS1-8 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation b c d e a Step 4. Apply Loads and Boundary Conditions Create a boundary condition a.Loads/BCs: Create / Displacement / Nodal. b.Enter hub cylinder as the New Set Name. c.Click Input Data. d.Enter for Translations. e.Click OK.

9 WS1-9 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a f g e b c Step 4. Apply Loads and Boundary Conditions Create a boundary condition a.Click Select Application Region. b.For the Geometry Filter select Geometry. c.Set the Selection Filter to Surface or Face d.Screen pick the inner cylindrical face of the strut as shown. e.Click Add. f.Click OK. g.Click Apply. d

10 WS1-10 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation b d e a Step 4. Apply Loads and Boundary Conditions Create a load a.Loads/BCs: Create / Total Load / Element Uniform. b.Enter landing load as the New Set Name. c.Click Input Data. d.Enter for Load. e.Click OK. c

11 WS1-11 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a e f d b Step 4. Apply Loads and Boundary Conditions Create a load a.Click Select Application Region. b.For the Geometry Filter select Geometry. c.Screen pick the inside circular surface at the upper end of the strut as shown. d.Click Add. e.Click OK. f.Click Apply. c

12 WS1-12 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a c b d g f e Step 5. Create Material Properties Create an isotropic material a.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.

13 WS1-13 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a b e d Step 6. Create Physical Properties Create a solid property a.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. c

14 WS1-14 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a c d b Step 6. Create Physical Properties Apply the physical properties a.Click in the Select Members box. b.Screen pick the solid as shown. c.Click Add. d.Click Apply.

15 WS1-15 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a b c d e Step 7. Run Linear Static Analysis Analyze the model a.Analysis: Analyze / Entire Model / Full Run. b.Click Solution Type. c.Choose Linear Static as the Solution Type. d.Click OK. e.Click Apply.

16 WS1-16 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation Step 8. Open and Review the.f06 file Review the.f06 file a.Open the file strut.f06 with a text editor. b.Review the diagnostic messages and analysis results.

17 WS1-17 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation a b c e d Step 8. Read Results into MSC.Patran Attach the results file a.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.

18 WS1-18 NAS120, Workshop 1, May 2006 Copyright 2005 MSC.Software Corporation e Step 9. Plot Stress and Displacement Create a quick plot a.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