WS15-1 WORKSHOP 15 THERMAL STRESS ANALYSIS WITH DIRECTIONAL HEAT LOADS NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation

WS15-2 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation

WS15-3 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation n Problem Description This example demonstrates how to apply the thermal(temperature) results of a previous workshop to performing a stress analysis. The temperature loading for the stress/displacement analysis is enabled by using a continuous spatial FEM field. Another approach is to use a punch file with the include option to access the thermal results. The diameter of the cylinder is 1.5 inch with a length of 6 inches. The material is aluminum.

WS15-4 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation n Suggested Exercise Steps 1. Open an existing database 2. Create a continuous spatial FEM Field 3. Change the analysis type from thermal to structural 4. Specify material for structural analysis 5. Define element properties 6. Create a new load case for structural analysis 7. Apply a clamped boundary condition 8. Define a temperature load 9. Display all structural boundary conditions 10. Perform the structural stress analysis 11. Run MSC.Nastran 12. Attach the results file 13. Display the stress analysis results 14. Quit MSC.Patran

WS15-5 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 1: Open an Existing Database Open the database for the workshop on directional heat loads. a.File: Open b.Select direct_heat.db for File name. c.Click OK. c a b

WS15-6 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 2: Create a Continuous Spatial FEM Field Create a continuous Spatial FEM field based on the temperature profile. The temperature contour plot must be displayed to create the field. a.Fields: Create/Spatial/FEM b.Enter tempload for Field Name. c.Select Continuous for FEM Field Definition. d.Select Scalar for Field Type. e.Select Current Viewport for Mesh Results Group Filter. f.Select default_group for Select Group. g.Click Apply. c a b g f d e

WS15-7 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Change the Analysis Type From Thermal to Structural Change the analysis type to structural. a.Preferences/Analysis… b.Select MSC.Nastran for Analysis Code. c.Select Structural for Analysis Type. d.Click OK. c a b d

WS15-8 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 4: Specify Material for Structural Analysis Specify the structural material. a.Materials: Create/Isotropic/Manual Input. b.Enter alum_st for Material Name. c.Click Input properties… d.Enter 1.0e7 for Elastic Modulus. e.Enter 0.34 for Poisson Ratio. f.Enter 1.3e-5 for Thermal Expan. Coeff. g.Enter 0.0 for Reference Temperature. h.Click OK. c a b g h f d e

WS15-9 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 5: Define Element Properties Define 2D shell element properties. a.Properties: Create/2D/Shell b.Enter alum_st for property Set Name. c.Click Input Properties… d.Click Material Name box and select alum_st e.Enter for Thickness f.Click OK g.Enter Surface 1 for Select Members. h.Click Add i.Click Apply j.Click Yes c a b j i g h f d e

WS15-10 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 6: Create a New Load Case for Structural Analysis Create a new load case. a.Load Case: Create. b.Enter struct_load for Load Case Name. c.Select Make Current toggle. d.Select Static for Load Case Type. e.Enter 1.0 for Load Case Scale Factor. f.Click Apply. c a b e f d

WS15-11 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 7: Apply a Clamped Boundary Condition Clamp one end and seam of cylinder. a.Loads/BCs: Create/Displacement/Nodal. b.Enter clamp_bc for New Set Name. c.Click Input Data… d.Enter for Translations. e.Enter for Rotations. f.Click OK. g.Click Select Application Region… h.Click Geometry for Geometry Filter. i.Enter Curve 1 Surface 1.3 for Select Geometry Entities. j.Click Add. k.Click OK. l.Click Apply. c a b l j k i g h f d e

WS15-12 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 7: Apply a Clamped Boundary Condition (Cont.)

WS15-13 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 8: Define a Temperature Load Define temperature load using the Spatial FEM field. a.Loads/BCs: Create/Temperature/Nodal. b.Enter temp_load for New Set Name. c.Click Input Data… d.Click in Temperature box and select tempload under Spatial Fields. e.Click OK. f.Click Select Application Region… g.Enter Surface 1 for Select Geometry Entities. h.Click Add. i.Click OK. j.Click Apply. c a b j i g h f d e

WS15-14 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 9: All Structural Boundary Conditions

WS15-15 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 10: Perform the Structural Stress Analysis Perform the stress analysis. a.Analysis: Analyze/Entire Model/Analysis Deck. b.Enter str_stress for Job Name. c.Click Subcase Select… d.Select struct_load for Subcases For Solution Sequence: 101 e.Click OK f.Click Apply c a b f d e

WS15-16 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 11: Run MSC.Nastran Run MSC.Nastran a.Run MSC.Nastran b.Select str_stress.bdf for File name. c.Click Open d.Click Run c a b d

WS15-17 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 12: Attach the Results File Attach the MSC.Nastran results file. a.Analysis: Attach XDB/Result Entities/Local b.Click Select Results File… c.Select str_stress.xdb for File name. d.Click OK. e.Click Apply. c a b d e

WS15-18 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 13: Display the Stress Analysis Results Display the deformation and stress results. a.Results:Create/Quick Plot. b.Select SC1:STRUCT_LOAD.. for Select Result Cases. c.Select Stress Tensor for Select Fringe Result d.Select Displacements, Translational for Select Deformation Result. e.Click Apply. c a b d e

WS15-19 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 13: Display the Stress Analysis Results (Cont.)

WS15-20 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 13: Display the Stress Analysis Results (Cont.) Set the scale for the displacement plot to True Scale and Scale Factor of 1.0 a.Results:Create/Deformation. b.Select Display Attributes icon. c.Select True Scale under Scale Interpretation. d.Specify Scale Factor as 1.0 e.Click Apply.

WS15-21 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation Step 14: Quit MSC.Patran Quit MSC.Patran a.Select File on the Menu Bar and select Quit from the drop down menu a

WS15-22 NAS104, Workshop 15, March 2004 Copyright 2004 MSC.Software Corporation