WORKSHOP 9B 2½ D CLAMP – ISO MESHER

WS9B-2 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation

WS9B-3 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation l Workshop Objectives l Practice the construction of simple (blue) solids

WS9B-4 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description l Analyze the clamp shown below: 60 mm 100 mm 150 mm 200 mm 30 mm 50 mm R = 10 mm

WS9B-5 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description (cont.) l A pressure loading of 1 N/mm 2 is applied to the top face. l Constrain the bolt hole in all three translations. l Material Properties: l E = 109 x 10 3 N/mm 2 =0.3

WS9B-6 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation l Suggested Exercise Steps 1. Create a new database. 2. Create surface geometry. 3. Extrude the surface geometry into solids. 4. Mesh the solid geometry. 5. Create a boundary condition. 6. Create a pressure load. 7. Define material properties. 8. Create Physical Properties. 9. Run the finite element analysis using MSC.Nastran. 10. Plot displacements and stresses.

WS9B-7 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation b c d f g h Step 1. Create New Database Create a new database called clamp.db a.File / New. b.Enter clamp_isomesh as the file name. c.Click OK. d.Choose Tolerance Based on Model. e.Enter 200 for the Approximate Maximum Model Dimension. f.Select MSC.Nastran as the Analysis Code. g.Select Structural as the Analysis Type. h.Click OK. a e

WS9B-8 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Create two arcs a.Geometry: Create / Curve / 2D ArcAngles. b.Enter 10 for the Radius. c.Enter 90 for the Start Angle. d.Enter 135 for the End Angle. e.Enter [ ] for the Center Point List. f.Click Apply. g.Repeat this procedure for a Start Angle of 135 and an End Angle of 180. a b c d e f

WS9B-9 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Create another curve a.Geometry: Create / Curve / XYZ. b.Enter for the Vector Coordinates List. c.Enter [0 50 0] for the Origin Coordinates List. d.Click Apply. a b c d

WS9B-10 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Create another curve a.Geometry: Create / Curve / XYZ. b.Enter for the Vector Coordinate List. c.Click in the Origin Coordinates List box. d.Screen Pick the origin at the top of the left curve as shown. a c b d

WS9B-11 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Create 2 surfaces a.Geometry: Create / Surface / Curve. b.Screen Pick the arc section and opposite curve as shown. c.Repeat the procedure to create another surface between the other two curves a b c

WS9B-12 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Mirror the surfaces a.Geometry: Transform / Surface / Mirror. b.Enter Coord 0.1 for the Mirror Plane Normal. c.Enter 50 for the offset. d.Click in the surface list box and screen pick both surfaces. e.Repeat the procedure with Coord 0.2 as the mirror plane normal, 50 for the offset, and all four upper surfaces selected. a b c e d

WS9B-13 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Extrude two surfaces a.Geometry: Create / Surface / Extrude. b.Enter for the Translation Vector. c.Click in the Curve List box and select the two edges as shown. a b c

WS9B-14 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Create Surface Geometry Extrude two more surfaces a.Geometry: Create / Surface / Extrude. b.Enter for the Translation Vector. c.Click in the Curve List box and select the two edges as shown. a b c

WS9B-15 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Create Solid Geometry Create solids a.Geometry: Create / Solid / Extrude. b.Change to Iso 3 view. c.Set the solid type to IsoMeshable. d.Enter for the Translation Vector. e.Click in the Surface List box and rectangular pick to select all surfaces. f.Select the top surface of two solids, as shown. a b c d e f

WS9B-16 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Create Mesh Create mesh seeds a.Elements: Create / Mesh Seed / Uniform. b.Set the Number of Elements to 6. c.Click in the Curve List box and select the two edges, as shown. a b c

WS9B-17 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Create Mesh Create a solid mesh a.Elements: Create / Mesh / Solid. b.Select Hex as the element shape. c.Set the Mesher to IsoMesher. d.Click in the Solid List box and select all solids. e.Set the Global Edge Length to 10. f.Click Apply. a b c d e f

WS9B-18 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Create Mesh Equivalence the model a.Elements: Equivalence / All / Tolerance Cube. b.Click Apply. a b

WS9B-19 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 5. Create Boundary Condition Create the boundary condition a.Loads/BCs: Create / Displacement / Nodal. b.Enter bolt_hole as the New Set Name. c.Click Input Data. d.Enter for Translations e.Click OK. a b c d e

WS9B-20 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Apply the boundary condition a.Click Select Application Region. b.For the Geometry Filter select Geometry. c.Click on the Iso 3 View Icon. d.Zoom in using View Corners. e.Select the Surface or Face Icon. f.Pick all eight surfaces that surround the bolt hole. g.Click Add. h.Click OK. i.Click Apply. Step 5. Create Boundary Condition a h i g b c d f e

WS9B-21 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation a Step 6. Create Load Create the pressure load a.Loads/BCs: Create / Pressure / Element Uniform. b.Enter clamp_pressure as the New Set Name. c.Click Input Data. d.Enter 1 for the Pressure. e.Click OK. b e d c

WS9B-22 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Apply the pressure load a.Click Select Application Region. b.For the Geometry Filter select Geometry. c.Click on the Iso 3 View Icon. d.Click on the Fit View Icon. e.Pick the top surfaces of the solids as shown. f.Click Add. g.Click OK. h.Click Apply. Step 6. Create Load a b c d e f g h

WS9B-23 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 7. Define Material Properties Create an isotropic material a.Materials: Create / Isotropic / Manual Input. b.Enter titanium as the Material Name. c.Click Input Properties. d.Enter 109e3 for the elastic modulus and 0.3 for the Poisson Ratio. e.Click OK. f.Click Apply. d e a b c f

WS9B-24 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 8. Create Physical Properties Create element properties a.Properties: Create / 3D / Solid. b.Enter solid as the Property Set Name. c.Click Input Properties. d.Click on the Select Material Icon. e.Select titanium as the material. f.Click OK. d e f a b c

WS9B-25 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 8. Create Physical Properties Apply the element properties a.Click on the Bottom View icon. b.Click in the Select Members box. c.Rectangular pick all solids as shown. d.Click Add. e.Click Apply. c a b d e

WS9B-26 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 9. Run Linear Static Analysis Choose the analysis type a.Analysis: Analyze / Entire Model / Full Run. b.Click Solution Type. c.Choose Linear Static. d.Click OK. e.Click Apply. a e b d c

WS9B-27 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 10. Plot Displacements and Stresses Attach the results file a.Analysis: Access Results / Attach XDB / Result Entities. b.Click Select Results File. c.Choose the results file clamp_isomesh.xdb. d.Click OK. e.Click Apply. a b c e d

WS9B-28 NAS120, Workshop 9B, May 2006 Copyright 2005 MSC.Software Corporation Step 10. Plot Displacements and Stresses Create a quick plot a.Results: Create / Quick Plot. b.Select Stress Tensor as the Fringe Result. c.Select Von Mises as the Fringe Result Quantity. d.Select Displacements, Translational as the Deformation Result. e.Click Apply. a d c e b