WS16-1 WORKSHOP 16 THERMAL STRESS ANALYSIS OF A BI-METALIC PLATE Thermal Stress From Thermal NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software. - презентация

1 WS16-1 WORKSHOP 16 THERMAL STRESS ANALYSIS OF A BI-METALIC PLATE Thermal Stress From Thermal NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation

2 WS16-2 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation

3 WS16-3 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation n Problem Description For this example perform a thermal stress analysis of a bi-metallic strip made of Ge and solder. The dimensions(length x width) of the bi-metallic strip are one inch by one inch. The thickness for the solder material is 0.05 inch, and the thickness of the Ge material is inch. Thus the assembly thickness is inch. The outside(away from the solder/Ge interface) surface temperature of the solder is 70 C. The outside surface temperature of the Ge is –30 C. The thermal model is to consist of two hex8 meshes connected together, together with thermal properties and constant temperature boundary conditions. The temperature distribution is to be obtained by running a steady-state thermal analysis. Use the thermal results as loading for a stress analysis. Pior to the development of the MSC.Patran/MSC.Nastran heat transfer interface to use the thermal results for a stress analysis it was necessary to specify TEMP(PUNCH)=all in the MSC.Nastran Case Control section for the thermal run. This caused the thermal analysis temperature results to be saved in the punch file. In the subsequent stress analysis the punch file was accessed by specifying TEMP(LOAD)=1 in the Case Control section. However, now MSC.Patran supports MSC.Nastran heat transfer analysis. Because of this it is possible to create a field based on the thermal results. The field can be used for the creation of a temperature load for a stress analysis. In order to have non-zero stresses for the stress analysis it will be necessary to have enough displacement constraints to eliminate rigid body motion. Once the thermal base field is created, a stress/structural model is to be created using the hex8 meshes that were used for the thermal analysis. Also, it will be necessary to create structural materials.

4 WS16-4 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation

5 WS16-5 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation n Suggested Exercise Steps 1. Create a new database. 2. Set the solver to MSC.Nastran Thermal 3. Create a solid for each of the two materials 4. Create mesh seeds for IsoMesh-ing 5. IsoMesh the two solids 6. Connect the Hex8 elements at the geometric interface 7. Define the two materials 8. Define the element properties for the two materials 9. Apply temperature Load/BCs 10. Perform the thermal analysis 11. Run MSC.Nastran 12. Attach the results file 13. Display the temperature results 14. Create a continuous spatial FEM field 15. Change the analysis type to structural 16. Define material for structural analysis 17. Specify 3D element properties

6 WS16-6 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation n Suggested Exercise Steps (continued) 18. Create a load case for structural analysis 19. Define a temperature load 20. Apply displacement constraints 21. Perform the structural analysis 22. Run MSC.Nastran 23. Read the results file 24. Display the stress analysis results 25. Quit MSC.Patran

7 WS16-7 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 1: Create a New Database Create a new database. a.File: New b.Enter bimetalic for File name. c.Click OK. c a b

8 WS16-8 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 2: Set the solver to MSC.Nastran Thermal Specify the thermal solver. a.Select Based on Model b.Enter 10 for Model Dimension. c.Select MSC.Nastran for Analysis Code. d.Enter Thermal for Analysis Type. e.Click OK c a b d e

9 WS16-9 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Create a Solid for Each of the two Materials Create the two geometric solids. a.Geometry: Create/Surface/XYZ b.Enter for Vector Coordinates List. c.Enter [0 0 0] for Origin Coordinates List. d.Click Apply e.Create/Solid/Extrude f.Click IsoMeshable icon g.Enter for Translation Vector h.Enter Surface 1 for Surface List i.Click Apply c a b i g h f d e

10 WS16-10 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 3: Create a Solid for Each of the two Materials (Cont.) Create the two geometric solids (continued). a.Geometry: Create/Solid/Extrude. b.Click IsoMeshable icon for Solid Type c.Enter for Translation Vector d.Enter Solid 1.6 for Surface List. e.Click Apply. c a b d e

11 WS16-11 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 4: Create Mesh Seeds for IsoMesh-ing Create mesh seeds to control the IsoMesh-er. a.Elements: Create/Mesh Seed/Uniform b.Enter 4 for Number c.Enter Solid for Curve List. d.Click Apply. e.Elements: Create/Mesh Seed/Uniform f.Enter 2 for Number g.Enter Solid for Curve List h.Click Apply. c a b g h f d e

12 WS16-12 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 5: IsoMesh the two Solids IsoMesh the solids. a.Elements: Create/Mesh/Solid b.Select Hex for Elem Shape. c.Select IsoMesh for Mesher. d.Select Hex8 for Topology. e.Enter Solid 1 2 for Solid List. f.Enter 0.1 for Value of Global Edge Length. g.Click Apply c a b g f d e

13 WS16-13 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 6: Connect the Hex8 Elements at the Geometric Interface Connect the Hex8 elements. a.Elements: Equivalence/All/Tolerance Cube b.Enter for Equivalencing Tolerance. c.Click Apply c a b

14 WS16-14 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 7: Define the two Materials Specify thermal material property for Ge. a.Materials: Create/Isotropic/Manual Input. b.Enter Ge for Material Name. c.Click Input Properties… d.Enter for Thermal Conductivity. e.Click OK. f.Click Apply. c a b f d e

15 WS16-15 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 7: Define the two Materials (Cont.) Specify thermal material property for solder. a.Materials: Create/Isotropic/Manual Input. b.Enter Solder for Material Name. c.Click Input Properties… d.Enter 1.27 for Thermal Conductivity. e.Click OK. f.Click Apply c a b f d e

16 WS16-16 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 8: Define the Element Properties for the two Materials Create element property set for Ge material. a.Properties: Create/3D/Solid. b.Enter Ge for Property Set Name. c.Click Input Properties… d.Click in the Material Name box and select Ge from Material Property Sets. e.Click OK f.Enter Solid 2 for Select Members. g.Click Add h.Click Apply. c a b g h f d e

17 WS16-17 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 8: Define the Element Properties for the two Materials (Cont.) Create element property set for Solder material. a.Properties: Create/3D/Solid b.Enter Solder for Property Set Name. c.Click Input Properties… d.Click in Material Name and select Solder from Material Property Sets. e.Click OK. f.Enter Solid 1 for Select Members. g.Click Add. h.Click Apply. c a b g h f d e

18 WS16-18 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 9: Apply Temperature Load/BCs Apply temperature boundary conditions. a.Loads/BCs: Create/Temp/Nodal b.Enter temp_bottom for New Set Name. c.Click Input Data… d.Enter 70 for Boundary Temperature. 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

19 WS16-19 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 9: Apply Temperature Load/BCs (Cont.) Apply temperature boundary conditions a.Loads/BCs: Create/Temp/Nodal b.Enter temp_top for New Set Name. c.Click Input Data… d.Enter –30 for Boundary Temperature. e.Click OK. f.Click Select Application Region… g.Enter Solid 2.6 for Select Geometry Entities. h.Click Add. i.Click OK. j.Click Apply. c a b j i g h f d e

20 WS16-20 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 9: Apply Temperature Load/BCs (Cont.)

21 WS16-21 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 10: Perform the Thermal Analysis Perform the thermal analysis. a.Analysis: Analyze/Entire Model/Analysis Deck. b.Enter bimetalic for Job Name. c.Click Apply. c a b

22 WS16-22 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 11: Run MSC.Nastran Run the thermal solver. a.Run MSC.Nastran b.Select bimetalic.bdf for File name. c.Click Open. d.Click Run. c a b d

23 WS16-23 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 12: Attach the Results File Attach the xdb.file. a.Analysis: Attach XDB/Result Entities/Local. b.Click Select Results File… c.Select bimetalic.xdb for File name. d.Click OK. e.Click Apply. b a e c d

24 WS16-24 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 13: Display the Temperature Results Create a temperature contour. a.Results:Create/Quick Plot. b.Select SC1DEFAULT,A1.. for Select Result Cases. c.Select Temperatures for Select Fringe Result. d.Click Apply. c a b d

25 WS16-25 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 14: Create a Continuous Spatial FEM Field Define a spatial FEM field based on the temperature profile. a.Fields: Create/Spatial/FEM b.Enter t_load for Field Name. c.Select Continuous for FEM Field Definition. d.Select Scalar for Field Type. e.Select default_group for Select Group. f.Click Apply. c a b d f e

26 WS16-26 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 15: Change the Analysis Type 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

27 WS16-27 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 16: Define Material for Structural Analysis Specify structural material properties. a.Materials: Create/Isotropic/Manual Input. b.Enter Solder_st for Material Name. c.Click Input Properties… d.Enter 1.3e7 for Elastic Modulus e.Enter 0.4 for Poisson Ratio f.Enter 2.47e-5 for Thermal Expan. Coeff. g.Enter –30 for Reference Temperature. h.Click OK. i.Click Apply. c a b i g h f d e

28 WS16-28 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 16: Define Material for Structural Analysis (Cont.) Specify structural material properties. a.Materials: Create/Isotropic/Manual Input. b.Enter Ge_st for Material Name. c.Click Input Properties… d.Enter 1.885e7 for Elastic Modulus. e.Enter 0.933e7 for Shear Modulus. f.Enter 5.8e-6 for Thermal Expan. Coeff. g.Enter –30 for Reference Temperature. h.Click OK. i.Click Apply. c a b i g h f d e

29 WS16-29 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 17: Specify 3D Element Properties Create element properties. a.Properties: Create/3D/Solid b.Enter Ge_st for Property Set Name. c.Click Input Properties… d.Click in Material Name box and select Ge_st for Material property Sets. e.Click OK. f.Enter Solid 2 for Select Members. g.Click Add. h.Click Apply. i.Click Yes c a b i g h f d e

30 WS16-30 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 17: Specify 3D Element Properties (Cont.) Create element properties. a.Properties: Create/3D/Solid b.Enter Solder_st for Property Set Name. c.Click Input Properties… d.Click in the Material Name and select Solder_st for Material Property Sets. e.Click OK. f.Enter Solid 1 for Select members. g.Click Add. h.Click Apply i.Click Yes. c a b i g h f d e

31 WS16-31 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 18: Create a Load Case for Structural Analysis Create a load case for structural analysis. a.Load Case: Create. b.Enter struct_load for Load Case Name. c.Select Make Current. 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

32 WS16-32 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 19: Define a Temperature Load Define a temperature load. a.Loads/BC: Create/Temperature/Nodal b.Enter temp_load for New Set Name. c.Click Input Data… d.Click in Temperature box and select t_load under Spatial Fields. e.Click OK. f.Click Select Application Region… g.Select Solid 1 2 for Select Geometry Entities. h.Click Add. i.Click OK. j.Click Apply. c a b j i g h f d e

33 WS16-33 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 20: Apply Displacement Constraints Apply constraints on the four corners of the top solid face. a.Loads/BCs: Create/Displacement/Nodal b.Enter fix_x for New Set Name. c.Click Input Data… d.Enter for Translations e.Click OK. f.Click Select Application Region… g.Enter Point 9 10 for Select Geometry Entities h.Click Add. i.Click OK. j.Click Apply c a b i g h f d e j

34 WS16-34 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 20: Apply Displacement Constraints (Cont.) Apply constraints on the four corners of the top solid face. a.Loads/BCs: Create/Displacement/Nodal b.Enter fix_y for New Set Name. c.Click Input Data… d.Enter for Translations e.Click OK. f.Click Select Application Region… g.Enter Point 11 for Select Geometry Entities. h.Click Add. i.Click OK. j.Click Apply. c a b j i g h f d e

35 WS16-35 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 20: Apply Displacement Constraints (Cont.) Apply constraints on the four corners of the top solid face. a.Loads/BCs: Create/Displacement/Nodal. b.Enter fix_z for New Set Name. c.Click Input Data… d.Enter for Translations e.Click OK. f.Click Select Application Region… g.Enter Point 9:12 for Select Geometry Entities h.Click Add. i.Click OK j.Click Apply c a b j i g h f d e

36 WS16-36 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 21: Perform the Structural Analysis Perform the structural analysis. a.Analysis: Analyze/Entire Model/Analysis Deck b.Enter bimetalic_st for Job Name c.Click Translation Parameters… d.Select OP2 and Print for Data Output. e.Click OK f.Click Subcase Select… g.Select struct_load for Subcases For Solution Sequence: 101. h.Click OK. i.Click Apply. d a c h g e f i b

37 WS16-37 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 22: Run MSC.Nastran Run the structural solver. a.Run MSC.Nastran. b.Select bimetalic_st.bdf for File name. c.Click Open. d.Click Run. c a b d

38 WS16-38 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 23: Read the Results File Read the OP2 file. a.Analysis: Read Output2/Result Entities/Translate. b.Click Select Results File… c.Select bimetalic_st.op2 for File name. d.Click OK. e.Click Apply. c a b d e

39 WS16-39 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 24: Display the Stress Analysis Results Create plot of stress and displacement. a.Results: Create/Quick Plot. b.Select struct_load, Static Subcase for Select Result Cases c.Select Stress Tensor for Select Fringe Result. d.Select Von Mises for Quantity. e.Select Displacements, Translational for Select Deformation Result f.Click Apply. c a b e f d

40 WS16-40 NAS104, Workshop 16, March 2004 Copyright 2004 MSC.Software Corporation Step 25: Quit MSC.Patran Quit MSC.Patran a.Select File on the Menu Bar and select Quit from the drop down menu a