WS12-1 PAT301, Workshop 12, October 2003 WORKSHOP 12 CANTILEVERED BEAM USING 1D OR 2D ELEMENTS AND ANALYSIS

WS12-2 PAT301, Workshop 12, October 2003

WS12-3 PAT301, Workshop 12, October 2003 Problem Description u Model a cantilevered box beam with a static load at the free end. Create two models using 2D or 1D elements. The load is offset from the centerline of the beam – it is at a corner of the free end of the box beam. For the 1D element model use a Multi-Point-Constraint (MPC) to offset the load. Compare the results of the analysis for the two models.

WS12-4 PAT301, Workshop 12, October 2003 Suggested Exercise Steps 1. Start MSC.Patran and create a new database cant_beam_2D.db. 2. Create 5x1x1.5 parametric solid. 3. Create 2D Quad4 mesh on the four long sided faces of the solid. 4. Display element free edges. 5. Connect Quad4 elements together using equivalence. 6. Display element free edges (after equivalencing). 7. Apply concentrated force at free end of cantilevered beam and offset from beam centerline. 8. Constrain (fix) cantilevered end of beam. 9. Create material properties for beam; use aluminum properties. 10. Create properties for Quad4 elements. They include both bending and membrane properties. 11. Check load case. 12. Perform linear static analysis for 2D model. 13. Read results by attaching the MSC.Nastran xdb results file. 14. View the deformation results. 15. View both the deformation and stress results; save a copy of the database to be used later for a transient analysis of the beam. 16. Create a database for the 1D element model, cant_beam_1D.db. 17. Create a curve.

WS12-5 PAT301, Workshop 12, October 2003 Suggested Exercise Steps 18. Mesh the curve with 1D bar elements, Bar Create a rigid link (MPC) for force application at free end of cantilevered beam. 20. Create a concentrated force at the free end of the MPC. 21. Apply constraints at cantilevered end of the beam. Constrain all six degrees of freedom. 22. Create beam material properties; use aluminum properties. 23. Create element properties for 1D elements. Use the Beam Library and select the rectangular cross-section option. 24. Check load case. 25. Perform linear static analysis for 1D model. 26. Read results using the xdb file. 27. View both the deformation and stress results for the 1D model. 28. Compare the 2D and 1D model results.

WS12-6 PAT301, Workshop 12, October 2003 Step 1. Create a Database for 2D Element Model Create a new database for 2D element model. a.File / New. b.Enter cant_beam_2D 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. a b e f d c g

WS12-7 PAT301, Workshop 12, October 2003 Step 2. Create Solid Geometry a.Geometry: Create / Solid / XYZ. b.Select on Vector Coordinates List and enter. c.Apply. d.Change view to Iso 1 View. a b c d

WS12-8 PAT301, Workshop 12, October 2003 Step 3. Create 2D Element Mesh a.Elements: Create / Mesh / Surface. b.Element Shape: Quad. c.Mesher: IsoMesh. d.Topology: Quad4. e.Click on Surface List and select the four long faces of the solid, not including the end faces. f.Uncheck Automatic Calculation. g.Enter 0.5 for Global Edge Length. h. Apply. e g h f

WS12-9 PAT301, Workshop 12, October 2003 Step 4. Display Free Edges a.Elements: Verify / Element / Boundaries. b.Display Type: Free Edges. c.Apply. d.As shown in the figure, yellow lines along the solid edges should appear a b c

WS12-10 PAT301, Workshop 12, October 2003 b Step 5. Connect the Elements Together a.Elements: Equivalence / All / Tolerance Cube. b.Apply. Notice that magenta colored circles are drawn where nodes are equivalenced. a

WS12-11 PAT301, Workshop 12, October 2003 Step 6. Display Free Edges Again a.Elements: Verify / Element / Boundaries. b.Display Type: Free Edges. c.Apply. No longer do the yellow lines in the long direction appear. This means that the adjacent 2D quad elements are connected. a b c

WS12-12 PAT301, Workshop 12, October 2003 Step 7. Apply a Force at One End a.Loads / BCs: Create / Force / Nodal. b.Select on New Set Name and enter force. c.Input Data. d.Enter for Force. e.OK. f.Select Application Region. g.Geometry Filter: Geometry. h.Click on Select Geometry Entities. i.Select Point or Vertex icon from the Pick Menu. a b c d e f g h i

WS12-13 PAT301, Workshop 12, October 2003 Step 7. Apply a Force at One End (cont.) a.Turn on the Point labels. b.Select on the point(Point 7) as shown in the figure. c.Add. d.OK. e.Apply. Close-Up b c d a Note that selecting Point 7 and Vertex Solid is equivalent.

WS12-14 PAT301, Workshop 12, October 2003 Step 8. Create Constraints Constrain beam at other end, fixing all six degrees of freedom at all nodes. a.Loads / BCs: Create / Displacements / Nodal. b.Select on New Set Name: and enter fix_end. c.Select Input Data. d.Enter for Translations and Rotations. e.OK. f.Click on Select Application Region. g.Select Geometry for Geometry Filter. h.Click on Select Geometry Entities. i.Select Curve or Edge icon for the picking. a b c d e f g h i

WS12-15 PAT301, Workshop 12, October 2003 a.Select the four solid edges as shown in the figure. b.Add. c.OK. d.Apply. Step 8. Create Constraints (Cont.) Select these edges a b c

WS12-16 PAT301, Workshop 12, October 2003 Step 9. Create Material Properties a.Materials: Create / Isotropic / Manual Input. b.Select on Material Name and enter aluminum. c.Select Input Properties. d.Enter: Elastic Modulus: 10e6. Poisson Ratio: 0.3. e.OK. f.Apply. a b c d e f

WS12-17 PAT301, Workshop 12, October 2003 Step 10. Create Element Properties for the 2D Quad Topology a.Properties: Create / 2D / Shell. b.Option(s): Homogeneous / Standard Formulation. c.Select Property Set Name and enter alum_2D. d.Select Input Properties. e.Click on Material Property Name icon and select aluminum under Select Existing Material. f.Thickness: 0.1. g.OK. a b c d e f g

WS12-18 PAT301, Workshop 12, October 2003 Step 10. Create Element Properties for the 2D Quad Topology (Cont.) a.Click on Select Members. b.Select the four long solid faces. c.Add. d.Apply. e.Turn off the Point labels. a b c d

WS12-19 PAT301, Workshop 12, October 2003 Step 11. Check Assignment of Loads and BCs to Load Case a.Load Cases: Modify. b.Select Default in Select Load Case to Modify. c.Check that all Loads and BCs are selected. d.Cancel.. a b c d

WS12-20 PAT301, Workshop 12, October 2003 Step 12. Run the Analysis Run the analysis of the model. a.Analysis: Analyze / Entire Model / Full Run. b.Select Solution Type. c.Choose LINEAR STATIC for Solution Type. d.OK. e.Apply. b c d a

WS12-21 PAT301, Workshop 12, October 2003 Step 13. Read Results Under Analysis Attach the.xdb file to read the results. a.Analysis: Access Results / Attach XDB / Result Entities. b.Click on Select Results File. c.Select and attach cant_beam_2D.xdb. d.OK. e.Apply. c d a b e

WS12-22 PAT301, Workshop 12, October 2003 Step 14. View Results a.Results: Create / Deformation. b.Select Results icon. c.Select A1:Static Subcase under Select Result Cases. d.Select Displacements, Translational under Select Deformation Result. e.Show As: Resultant. f.Apply. a b c d e

WS12-23 PAT301, Workshop 12, October 2003 Step 14. View Results (Cont.) a.Results: Create / Fringe. b.Select A1:Static Subcase under Select Result Cases. c.Select Stress Tensor under Select Fringe Result. d.Quantity: X Component. e.Select Plot Options button. f.Coordinate Transformation: Global. g.Apply. a b c d e f

WS12-24 PAT301, Workshop 12, October 2003 Step 15. Stress Results and Save a Copy of the Database Display X component of stress fringe plot. Save a copy of this database for use later for a transient simulation. a.File / Save a Copy as... b.File name: cant_beam_transient.db. c.Save. d.File / Quit. a d

WS12-25 PAT301, Workshop 12, October 2003 Step 16. Create a New Database for 1D Element Model Create a new database for 1D element model. a.File / New. b.Enter cant_beam_1D 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. a b e f d c g

WS12-26 PAT301, Workshop 12, October 2003 Step 17. Create Curve Geometry a.Geometry: Create / Curve / XYZ. b.Select on Vector Coordinates List and enter. c.Apply. d.Change view to Iso 1 View. a b c d

WS12-27 PAT301, Workshop 12, October 2003 Step 18. Create 1D Element Mesh a.Elements: Create / Mesh / Curve. b.Topology: Bar2. c.Click on Curve List and select the curve. d.Enter 0.5 for Global Edge Length. e.Apply. a b c d e c

WS12-28 PAT301, Workshop 12, October 2003 Step 19. Create a Rigid Link at Force End Create a rigid link at the end of the beam where the load will be applied. That will offset the load so it will be applied equivalent to that for the prior 2D model. a.Turn on the node labels. b.Elements: Create / Node / Edit. c.Select on Node Location List and enter [5, 0.5, 0.75]. d.Apply. This will give Node 12, where the load will be applied. b d a c

WS12-29 PAT301, Workshop 12, October 2003 Step 19. Create a Rigid Link (Cont.) a.Elements: Create / MPC / RBE2. b.Select Define Terms. c.Select Create Dependent. d.Turn off Auto Execute. e.Click on Node List and select Node 11 from the figure. f.DOFs: specify UX, UY, UZ, RX, RY, RZ. g.Apply. a b c d e f g

WS12-30 PAT301, Workshop 12, October 2003 Step 19. Create a Rigid Link (Cont.) a.Notice that Create Independent is active now. b.Click on Node List and select Node 12 from the figure. c.Apply. d.Cancel. e.Apply. Notice that a magenta colored line was drawn from Node 11 to Node 12. This represents the rigid RBE2 MPC. a b c d

WS12-31 PAT301, Workshop 12, October 2003 Step 20. Create a Concentrated Force Apply a force at the free end of the MPC. a.Loads / BCs: Create / Force / Nodal. b.Select on New Set Name and enter force-1D. c.Input Data. d.Enter for Force. e.OK. f.Select Application Region. g.Geometry Filter: FEM. h.Click on Select Nodes and select Node 12. i.Add. j.OK. k.Apply. a b c d e f g h i j

WS12-32 PAT301, Workshop 12, October 2003 Step 21. Apply Constraints at Other End a.Loads / BCs: Create / Displacements / Nodal. b.Select on New Set Name: and enter fix_it. c.Select Input Data. d.Enter for Translations and Rotations. e.OK. f.Click on Select Application Region. g.Select FEM for Geometry Filter. h.Click on Select Nodes and select Node 1. i.Add. j.OK. k.Apply a b c d e f g h i j

WS12-33 PAT301, Workshop 12, October 2003 Step 22. Create Material Properties a.Materials: Create / Isotropic / Manual Input. b.Select on Material Name and enter aluminum2. c.Select Input Properties. d.Enter: Elastic Modulus: 10e6. Poisson Ratio: 0.3. e.OK. f.Apply. a b c d e f

WS12-34 PAT301, Workshop 12, October 2003 Step 23. Create Element Properties for the 1D Beam Topology a.Properties: Create / 1D / Beam. b.Option(s): General Section / Standard Formulation. c.Select Property Set Name and enter alum_1D. d.Select Input Properties. e.From the Material Property Sets, select aluminum2 for Material Name. f.Select Create Sections Beam Library. a b c d e f

WS12-35 PAT301, Workshop 12, October 2003 Step 23. Create Element Properties for the 1D Beam Topology (Cont.) a.In New Section Name: cross_sect. b.Select the rectangular cross-section button and enter: W = 1.5, H = 1.0, t1 = 0.1, t2 = 0.1. c.Calculate / Display. d.OK. e.Enter in Bar Orientation. f.OK. g.Click on Select Members and select Curve 1. h.Add. i.Apply. j.Display the cross-section to scale under Display / Load/BC /Elem. Props… using Beam Display / 3D: Full-Span + Offsets. a b c Notice that the name cross_sect now appears in the Input Properties form under Section Name. Area, Inertia and Torsional Constant have values. The values are ghosted out so that to change them it is necessary to use the Create Section button. d e f b

WS12-36 PAT301, Workshop 12, October 2003 Step 23. Create Element Properties for the 1D Beam Topology (Cont.) a.This is the entire 1D model. A representation of the cross-section is shown, even though the geometry is only 1D.

WS12-37 PAT301, Workshop 12, October 2003 Step 24. Check Assignment of Loads and BCs to Load Case a.Load Cases: Modify. b.Select Default in Select Load Case to Modify. c.Check that all Loads and BCs are selected. d.Cancel. a b c d

WS12-38 PAT301, Workshop 12, October 2003 Step 25. Run Analysis for 1D Beam a.Analysis: Analyze / Entire Model / Full Run. b.Select Solution Type. c.Choose LINEAR STATIC for Solution Type. d.OK. e.Apply. b c d a

WS12-39 PAT301, Workshop 12, October 2003 Step 26. Read Results Under Analysis Attach the.xdb file to read the results. a.Analysis: Access Results / Attach XDB / Result Entities. b.Click on Select Result File. c.Select and attach the cant_beam_1D.xdb. d.OK. e.Apply. c d a b e

WS12-40 PAT301, Workshop 12, October 2003 Step 27. View Results Create a Deformation plot. a.Results: Create / Deformation. b.Select Results icon. c.Select A1:Static Subcase under Select Result Cases. d.Select Displacements, Translational under Select Deformation Result. e.Show As: Resultant. f.Apply. a b c d e

WS12-41 PAT301, Workshop 12, October 2003 Step 27. View Results (Cont.) a.Results: Create / Fringe. b.Select A1:Static Subcase under Select Result Case(s). c.Select Stress Tensor, Bending under Select Fringe Result. d.Quantity: X Component. e.Apply. a b c d

WS12-42 PAT301, Workshop 12, October 2003 a.Compare Results. b.This ends this exercise. Step 28. Compare 2D and 1D Model Results