1 / 42

WS6- 1

WORKSHOP 6 BRIDGE TRUSS. NAS120, Workshop 6, November 2003. WS6- 1. Problem Description The preliminary design of a steel truss bridge has just been finished. You are asked to evaluate the structural integrity of this bridge.

luther
Download Presentation

WS6- 1

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. WORKSHOP 6 BRIDGE TRUSS NAS120, Workshop 6, November 2003 WS6-1

  2. Problem Description • The preliminary design of a steel truss bridge has just been finished. You are asked to evaluate the structural integrity of this bridge. • The truss is made from steel with E = 30 x 106 psi and n = 0.3 • The truss members are I-beams with H = 18 in, W = 12 in, Tf = 0.5 in, and Tw = 0.5 in • The bridge needs to be able to support a 23,000 lb truck traveling over it. The truck weight is supported by two planar trusses. Model one planar truss with half the truck weight applied to it. • One end of the truss is pinned while the other end is free to slide horizontally.

  3. y x 11,500 lb (Subcase 2) 11,500 lb (Subcase 1)

  4. Workshop Objectives • Learn to mesh line geometry to generate CBAR elements • Become familiar with setting up the CBAR orientation vector and section properties • Learn to set up multiple load cases • Learn to view the different CBAR stress components in Patran

  5. Suggested Exercise Steps • Create a new database. • Create a geometry model of the truss using the table on the previous page. • Use Mesh Seeds to define the mesh density. • Create a finite element mesh. • Define material properties. • Create Physical Properties using the beam library. • Create boundary conditions. • Create loads. • Set up load cases. • Run the finite element analysis using MSC.Nastran. • Plot displacements and stresses.

  6. Step 1. Create New Database a a • Create a new database called bridge_truss.db • File / New. • Enter bridge_truss as the file name. • Click OK. • Choose Default Tolerance. • Select MSC.Nastran as the Analysis Code. • Select Structural as the Analysis Type. • Click OK. d e f b c g

  7. Step 2. Create Geometry d • Create the first point • Geometry: Create / Point / XYZ. • Enter [0 0 0] for the Point Coordinate List. • Click Apply. • Turn Point size on. a b c

  8. Step 2. Create Geometry Finish creating all 12 points.

  9. Step 2. Create Geometry Create curves to represent the truss members • Geometry: Create / Curve / Point. • Screen pick the bottom left point as shown. • Screen pick the top left point. A curve is automatically created because Auto Execute is checked. a c b

  10. Step 2. Create Geometry Finish creating all 21 curves.

  11. Step 3. Create Mesh Seeds Create a uniform mesh seed • Elements: Create / Mesh Seed / Uniform. • Enter 6 for the Number of Elements. • Click in the Curve List box. • Rectangular pick the bottom of the truss. a d b c

  12. Step 3. Create Mesh Seeds Create another mesh seed • Elements: Create / Mesh Seed / Uniform. • Enter 2 for the Number of Elements. • Click in the Curve List box. • Rectangular pick the rest of the truss, as shown. a d b c

  13. Step 4. Create Mesh Create a finite element mesh • Elements: Create / Mesh / Curve. • Set Topology to Bar2. • Click in the Curve List box. • Rectangular pick all of the curves as shown. • Click Apply. a b d c e

  14. Step 4. Create Mesh Equivalence the model • Elements: Equivalence / All / Tolerance Cube. • Click Apply. a b

  15. Step 5. Create Material Properties Create an isotropic material • Materials: Create / Isotropic / Manual Input. • Enter steel as the Material Name. • Click Input Properties. • Enter 30e6 for the elastic modulus and 0.3 for the Poisson Ratio. • Click OK. • Click Apply. a d b c f e

  16. Step 6. Create Physical Properties Create element properties • Properties: Create / 1D / Beam. • Enter i_beam as the Property Set Name. • Click Input Properties. • Click on the Select Material Icon. • Select steel as the material. • Click on the Beam Library button. a d b c f e

  17. Step 6. Create Physical Properties Define the beam section • Enter i_section for the New Section Name. • Enterthe appropriate values to define the beam’s dimensions. • Click Calculate/Display to view the beam section and its section properties. • After verifying that the section is correct, Click OK. b a c d

  18. Step 6. Create Physical Properties Define the bar orientation • Enter <1 2 0> for the Bar Orientation. • Click OK. Note: Any vector in the XY plane that is not parallel to any truss member would work as well. a b

  19. Step 6. Create Physical Properties Select application region • Click in the Select Members box. • Rectangular pick the entire truss as shown. • Click Add. • Click Apply. b a c d

  20. Step 6. Create Physical Properties c e a Verify the beam section • Display- Load/BC/Element Props. • Set Beam Display to 3D:Full-Span. • Shade the model. • Rotate the model and zoom in to verify that the I-beams are oriented correctly. • Return to the front view. • Set Beam Display back to 1D:Line. d f b

  21. Step 7. Create Boundary Conditions Create a boundary condition • Loads/BCs: Create / Displacement / Nodal. • Enter left_side as the New Set Name. • Click Input Data. • Enter <0 0 0> for Translations and <0,0, > for Rotations. • Click OK. a d b c e

  22. Step 7. Create Boundary Conditions a Apply the boundary condition • Reset graphics. • Click Select Application Region. • Select the bottom left point as the application region. • Click Add. • Click OK. • Click Apply. d c b e f

  23. Step 7. Create Boundary Conditions Create another boundary condition • Loads/BCs: Create / Displacement / Nodal. • Enter right_side as the New Set Name. • Click Input Data. • Enter < ,0,0> for Translations and <0,0, > for Rotations. • Click OK. a d b c e

  24. Step 7. Create Boundary Conditions Apply the boundary condition • Click Select Application Region. • Select the bottom right point as the application region. • Click Add. • Click OK. • Click Apply. c b d a e

  25. Step 8. Create Loads Create the mid span load • Loads/BCs: Create / Force / Nodal. • Enter mid_span_load as the New Set Name. • Click Input Data. • Enter <0 –11500 0> for the Force. • Click OK. a d b c e

  26. Step 8. Create Loads Apply the mid span load • Click Select Application Region. • Set the geometry filter to FEM. • For the application region select the node in the middle of the span to the right of the center, as shown. • Click Add. • Click OK. • Click Apply. b d c a e f

  27. Step 8. Create Loads Create the truss joint load • Loads/BCs: Create / Force / Nodal. • Enter truss_joint_load as the New Set Name. • Click Input Data. • Enter <0 –11500 0> for the Force. • Click OK. a d b c e

  28. Step 8. Create Loads Apply the load • Click Select Application Region. • Set the geometry filter to Geometry. • For the application region select the point at the center of the bridge, as shown. • Click Add. • Click OK. • Click Apply. b d c a e f

  29. Step 9. Set Up Load Cases Create a load case • Load Cases: Create. • Enter mid_span as the Load Case Name. • Click Assign/Prioritize Loads/BCs. • Click on Displ_left_side, Displ_right_side, and Force_mid_span_load to add them to the Load Case. • Click OK. • Click Apply. a d b c f e

  30. Step 9. Set Up Load Cases Create another load case • Load Cases: Create. • Enter truss_joint as the Load Case Name. • Click Assign/Prioritize Loads/BCs. • Click on Displ_left_side, Displ_right_side, and Force_truss_joint_load to add them to the Load Case. • Click OK. • Click Apply. a d b c f e

  31. Step 10. Run Linear Static Analysis Choose the analysis type • Analysis: Analyze / Entire Model / Full Run. • Click Solution Type. • Choose Linear Static. • Click OK. a c b d

  32. Step 10. Run Linear Static Analysis Analyze the model • Analysis: Analyze / Entire Model / Full Run. • Click Subcase Select. • Click Unselect All. • Click on mid_span and truss_joint to add them to the Subcases Selected list. • Click OK. • Click Apply. a d c b f e

  33. Step 11. Plot Displacements and Stresses Attach the results file • Analysis: Access Results / Attach XDB / Result Entities. • Click Select Results File. • Choose the results file bridge_truss.xdb. • Click OK. • Click Apply. a c d b e

  34. Step 11. Plot Displacements and Stresses Create a deformation plot for the mid span result case • Results: Create / Deformation. • Select the Mid Span Result Case. • Select Displacements, Translational as the Deformation Result. • Check Animate. • Click Apply. • Record the maximum deformation. • Click Stop Animation and Refresh Results Tools. Max Deformation = ____________ a b c d e

  35. Step 11. Plot Displacements and Stresses Create a Fringe Plot of X Component Axial Stress • Results: Create / Fringe. • Select the Mid Span Result Case. • Select Bar Stresses, Axial as the Fringe Result. • Select X Component as the Fringe Result Quantity. • Click on the Plot Options icon. • Set the Averaging Definition Domain to None. • Click Apply. a e b c f d g

  36. Step 11. Plot Displacements and Stresses View the results • Record the maximum and minimum X component axial stress. Max X Axial Stress = _________________ Min X Axial Stress = __________________

  37. Step 11. Plot Displacements and Stresses Create Fringe Plots of maximum and minimum combined bar stresses • Results: Create / Fringe. • Select the Mid Span Result Case. • Select Bar Stresses, Maximum Combined as the Fringe Result. • Click Apply. • Record the Maximum combined stress. Max Stress= _______ • Repeat the procedure with Bar Stresses, Minimum Combined as theFringe Result and record the Minimum Stress. Min Stress = _______ a b c d

  38. Step 11. Plot Displacements and Stresses e Create a deformation plot for the truss joint result case • Results: Create / Deformation. • Select the Truss Joint Result Case. • Select Displacements, Translational as the Deformation Result. • Check Animate. • Reset Graphics. • Click Apply. • Record the maximum deformation. • Click Stop Animation and Refresh Results Tools. Max Deformation = ____________ a b c d f

  39. Step 11. Plot Displacements and Stresses Create a Fringe Plot of X Component Axial Stress • Results: Create / Fringe. • Select the Truss Joint Result Case. • Select Bar Stresses, Axial as the Fringe Result. • Select X Component as the Fringe Result Quantity. • Click on the Plot Options icon. • Set the Averaging Definition Domain to None. • Click Apply. a e b c f d g

  40. Step 11. Plot Displacements and Stresses View the results • Record the maximum and minimum X component axial stress. Max X Axial Stress = _________________ Min X Axial Stress = __________________

  41. Step 11. Plot Displacements and Stresses Create Fringe Plots of maximum and minimum combined bar stresses • Results: Create / Fringe. • Select the Truss Joint Result Case. • Select Bar Stresses, Maximum Combined as the Fringe Result. • Click Apply. • Record the Maximum combined stress. Max Stress= _______ • Repeat the procedure with Bar Stresses, Minimum Combined as theFringe Result and record the Minimum Stress. Min Stress = _______ a b c d

More Related