1. WORKSHOP 7 TAPERED PLATE WS7-1 NAS120, Workshop 7, November 2003

2. WS7-2 NAS120, Workshop 7, November 2003

3. WS7-3 NAS120, Workshop 7, November 2003 Problem Description Model a tapered annular plate with a variable pressure loading. Due to symmetry, only a 45° slice of the plate will be modeled. The plate is constructed from two different materials as shown below: Inner Region Steel Outer Region Aluminum

4. WS7-4 NAS120, Workshop 7, November 2003 Problem Description (cont.) The thickness variation in the plate is shown below:

5. WS7-5 NAS120, Workshop 7, November 2003 Analysis Code:MSC.Nastran Element Type:Quad4 Element Global Edge Length:0.5 Problem Description (Cont.) Table 8.1 Mesh Definition Table 8.2 Material Properties: Material:SteelAluminum Modulus of Elasticity:30E+0610E+06 Poisson Ratio:0.300.33 Density:7.324E-042.588E-04

6. WS7-6 NAS120, Workshop 7, November 2003 Workshop Objectives: 1.Learn to use fields to define element thickness 2.Learn to use fields to create variable pressure loading

7. WS7-7 NAS120, Workshop 7, November 2003 Suggested Exercise Steps: 1.Create geometry representing a 45° slice of the annular plate. 2.Create the finite element mesh using the information listed in Table 12.1. 3.Create a cylindrical coordinate system. 4.Using the cylindrical coordinate system, define a spatially varying field which represents the plate thickness. Verify the field by creating an XY-plot. 5.Define material properties using the material constants shown in Table 12.2.

8. WS7-8 NAS120, Workshop 7, November 2003 Suggested Exercise Steps: 6.Define element properties by assigning the material type and element thickness to the correct region of the model. 7.Verify that the spatial variation of the element thickness has been assigned correctly to the model by creating a scalar plot. 8.Define a spatially varying field that represents the pressure load. 9.Apply the pressure load. 10.Verify that the pressure has been assigned correctly by modifying plot markers.

9. WS7-9 NAS120, Workshop 7, November 2003 Create a New Database Create a new database called annular_plate.db a.File / New. b.Enter tapered_plate as the file name. c.Click OK. d.Choose Default Tolerance. e.Select MSC.Nastran as the Analysis Code. f.Select Structural as the Analysis Type. g.Click OK.

10. WS7-10 NAS120, Workshop 7, November 2003 Create a curve a.Geometry: Create / Curve / 2D ArcAngles. b.Enter 1.0 for the Radius. c.Enter 0.0 for Start Angle and 45 for End Angle. d.Enter [0 0 0] for the Center Point List. e.Click Apply. f.Click on the Show Labels Icon. Step 1. Geometry: Create/Curve/2D ArcAngles a b c d e f

11. WS7-11 NAS120, Workshop 7, November 2003 Create two more curves. a.Enter 3.0 for the Radius. b.Click Apply. c.Enter 4.0 for the Radius. d.Click Apply. Step 1. (Cont.) Geometry: Create/Curve/2D ArcAngles a c d b

12. WS7-12 NAS120, Workshop 7, November 2003 Create two surfaces. a.Create / Surface / Curve. b.Select 2 Curve for the Option. c. Screen pick Curve 1, then Curve 2. A surface is automatically generated. d.Screen pick Curve 2, then Curve 3. A second surface is generated. Step 1. (Cont.) Create/Surface/Curve a b c d

13. WS7-13 NAS120, Workshop 7, November 2003 Mesh the two surfaces. a.Finite Element: Create / Mesh / Surface. b.Select IsoMesh as the Mesher. c.Select Quad4 Element Topology. d.Select both surfaces for the Surface List. e.Enter 0.5 as the Global Edge Length. f.Click Apply. g.Click on Hide Labels icon. Step 2. Finite Elements: Create/Mesh/Surface a b c d e f g

14. WS7-14 NAS120, Workshop 7, November 2003 Step 2. (Cont.) Finite Element: Equivalence /All/Tolerance Cube Merge all coincident nodes. a.Equivalence / All / Tolerance Cube. b.Click Apply. a b

15. WS7-15 NAS120, Workshop 7, November 2003 Create a cylindrical coordinate system. a.Geometry: Create / Coord / 3 Point b.Select Cylindrical as the type of coordinate system. c.Enter [0 0 0] for origin, [0 0 1] for Point on Axis 3, and [1 0 0] for Point on Plane 1-3. d.Click Apply. Step 3. Create/Coord/3Point a b c d

16. WS7-16 NAS120, Workshop 7, November 2003 Step 4. Fields: Create /Spatial/ Tabular Input Create a field which defines the variation in plate thickness. a.Fields: Create / Spatial / Tabular Input. b.Type in thickness_spatial for the Field Name. c.Select Coord 1 for Coordinate System. d.Select R as the Active Independent Variable. e.Click on the Input Data button to bring up the 1D Scalar Table Data window. f.Enter the values into the table using the Enter key on the keyboard. Use the values shown on this page. g.Click OK to return to the main field menu. h.Click Apply. a b c d e f g h

17. WS7-17 NAS120, Workshop 7, November 2003 Step 4. (Cont.) Field: Show Verify the field using an XY plot. a.Show. b.Select thickness_spatial in the Select Field to Show window. c.Click on the Specify Range button. d.Check the Use Existing Points option. e.Click OK to return to the main field menu. f.Click Apply. a b c d e f

18. WS7-18 NAS120, Workshop 7, November 2003 Step 5. Materials: Create / Isotropic / Manual Input Create a material property set for steel. a.Materials: Create / Isotropic / Manual Input. b.Enter steel as the Material Name. c.Click on the Input Properties button. d.Enter 30e6 for the Elastic Modulus. e.Enter 0.3 for the Poisson Ratio. f.Enter 0.0007324 for the Density. g.Click OK. h.Click Apply. a b c d e g h f

19. WS7-19 NAS120, Workshop 7, November 2003 Step 5. (Cont.) Materials: Create / Isotropic / Manual Input Create a material property set for aluminum. a.Materials: Create / Isotropic / Manual Input. b.Enter alum as the Material Name. c.Click on the Input Properties button. d.Enter 10e6 for the Elastic Modulus. e.Enter 0.33 for the Poisson Ration. f.Enter 0.0002588 for the Density. g.Click OK. h.Click Apply. a b c d e g h f

20. WS7-20 NAS120, Workshop 7, November 2003 Step 6. Element Properties: Create / 2D / Shell Define Element Properties for the inner portion of the plate. a.Properties: Create / 2D / Shell. b.Enter prop_1 as the Property Set Name. c.Click on the Input Properties button. d.Click on the Select Material Icon. e.Click on the steel in the Select Material window. f.Change the thickness option from Real Scalar to Element Nodal. g.Click on the Select Field Icon. h.For the Thickness, select thickness_spatial from the Field Definitions section. i.Click OK. j.Select the inner surface for the Application Region. k.Click Add. l.Click Apply. a b c d g i f j e h k l

21. WS7-21 NAS120, Workshop 7, November 2003 Step 6. (Cont.) Element Properties: Create / 2D / Shell a b c d g i f j e h k l Define Element Properties for the outer portion of the plate. a.Properties: Create / 2D / Shell. b.Enter prop_2 as the Property Set Name. c.Click on the Input Properties button. d.Click on the Select Material Icon. e.Click on the alum in the Select Material window. f.Change the thickness option from Real Scalar to Element Nodal. g.Click on the Select Field Icon. h.For the Thickness, select thickness_spatial from the Field Definitions section. i.Click OK. j.Select the outer surface for the Application Region. k.Click Add. l.Click Apply.

22. WS7-22 NAS120, Workshop 7, November 2003 Step 7. Element Properties: Show Verify element properties using a scalar plot of the thickness. a.Properties: Show. b.Select Thickness from the Existing Properties window. c.Select Scalar Plot as the Display Method. d.Select Default Group. e.Click Apply. a b c d e

23. WS7-23 NAS120, Workshop 7, November 2003 Step 8. Fields: Create /Spatial/ Tabular Input Create a field which defines the variation in pressure. a.Fields: Create / Spatial / PCL Function. b.Type in pressure_variation for the Field Name. c.Select Coord 1 for Coordinate System. d.Enter the function: 100*’R. e.Click Apply. a b c d e

24. WS7-24 NAS120, Workshop 7, November 2003 Step 9. Loads/BCs: Create /Pressure/ Element Uniform Create a pressure load. a.Loads/BCs: Create / Pressure / Element Variable. b.Type in press for the New Set Name. c.Set the Target Element Type to 2D. d.Click Input Data. e.Click on the Bottom Surf Pressure list box and select the field pressure_variation. f.Click OK. a b d e f c

25. WS7-25 NAS120, Workshop 7, November 2003 Step 9. Loads/BCs: Create /Pressure/ Element Uniform a Select an application region. a.Click on the Iso 3 View Icon. b.Click Select Application Region. c.For the Geometry Filter select Geometry. d.Select the Surface or Face filter. e.Click in the application region list box and select both surfaces. f.Click Add. g.Click OK. h.Click Apply. b e c f g h d

26. WS7-26 NAS120, Workshop 7, November 2003 Step 10. Modify Plot Markers Modify the pressure plot markers. a.Display: Load/BC/Elem.Props. b.Select Show on FEM only. c.Click on Vectors/Filters. d.Change the length to Scaled- Screen Relative. e.Click Apply. f.Click Cancel. g.Click on Label Style. h.Set the Label Format to Integer. i.Click OK. j.Click Apply. a c d e f g h i j b

27. WS7-27 NAS120, Workshop 7, November 2003 Step 10. Modify Plot Markers Re-plot the pressure plot markers. a.Loads/BCs: Plot Markers. b.Select the pressure load set. c.Click Apply. a b c

28. WS7-28 NAS120, Workshop 7, November 2003