1 / 30

WS9A- 1

WORKSHOP 9A 2½ D CLAMP – SWEEP MESHER. NAS120, Workshop 9A, November 2003. WS9A- 1. Problem Description Analyze the clamp shown below:. R = 10 mm. 50 mm. 30 mm. 60 mm. 30 mm. 150 mm. 100 mm. 200 mm. Problem Description (cont.)

robertas
Download Presentation

WS9A- 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 9A 2½ D CLAMP – SWEEP MESHER NAS120, Workshop 9A, November 2003 WS9A-1

  2. Problem Description • Analyze the clamp shown below: R = 10 mm 50 mm 30 mm 60 mm 30 mm 150 mm 100 mm 200 mm

  3. Problem Description (cont.) • A pressure loading of 1 N/mm2 is applied to the top face. • Constrain the bolt hole in all three translations. • Material Properties: • E = 109 x 103 N/mm2 • n =0.3

  4. Workshop Objectives • Practice the construction of a 2 ½ D solid model by sweeping 2D elements.

  5. Suggested Exercise Steps • Create a new database. • Create surface geometry. • Mesh the surface to create CQUAD4 plate elements. • Sweep the plate elements into solid elements. • Create a boundary condition. • Create a pressure load. • Define material properties. • Create Physical Properties. • 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 clamp.db • File / New. • Enter clamp as the file name. • Click OK. • Choose Tolerance Based on Model. • Enter 200 for the Approximate Maximum Model Dimension. • Select MSC.Nastran as the Analysis Code. • Select Structural as the Analysis Type. • Click OK. d e f g b c h

  7. Step 2. Create Surface Geometry • Create the first surface • Geometry: Create / Surface / XYZ. • Enter <150 100 0> for the Vector Coordinate List. • Click Apply. a b c

  8. Step 2. Create Surface Geometry Add a hole to the surface • Geometry: Edit / Surface / Add Hole. • Enter 10 for the Hole Radius. • Click in the Surface box. • Screen Pick Surface 1. • Enter [50 50 0] for the Center Point List. • Click Apply. a b c e d f

  9. Step 2. Create Geometry Create another surface • Geometry: Create / Surface / XYZ. • Enter <50 100 0> for the Vector Coordinate List. • Click in the Origin Coordinates List box. • Screen Pick the origin as shown. a b c d

  10. Step 3. Create Mesh Create a surface mesh • Elements: Create / Mesh / Surface. • Set the Mesher to Paver. • Click on Paver Parameters. • Set the Max h/L value to 0.05. • Click OK. • Click in the Surface List box. • Rectangular pick both surfaces. • Set the Global Edge Length to 10. • Click Apply. a b g c d f h e i

  11. Step 3. Create Mesh a View the meshed surface • Click on the Iso 3 View Icon.

  12. Step 4. Create Solid Elements Sweep the plate elements into solid elements. • Elements: Sweep / Element / Extrude. • Click Mesh Control. • Set the Number of Elements to 6. • Click OK. • Set the Direction Vector to <0 0 1>. • Set the Extrude Distance to 30. • Click in the Base Entity List box. • Polygon pick the 2D elements as shown. • Click Apply. a c b h d e f g i

  13. Step 4. Create Solid Elements Sweep the plate elements into solid elements. • Elements: Sweep / Element / Extrude. • Click Mesh Control. • Set the number of elements to 12. • Click OK. • Set the Direction Vector to <0 0 1>. • Set the Extrude Distance to 60. • Click in the Base Entity List box. • Polygon pick the rest of the 2D elements as shown. • Click Apply. a c b h d e f g i

  14. Step 4. Create Solid Elements Delete the plate elements • Elements: Delete / Element. • Pick the Quad Element Filter. • Rectangular pick all elements. • Click Apply. a b d c

  15. Step 4. Create Solid Elements Verify element boundaries • Elements: Verify / Element / Boundaries. • Click Apply. a b

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

  17. Step 4. Create Solid Elements Verify element boundaries again • Elements: Verify / Element / Boundaries. • Click Apply. a a b

  18. Step 5. Create Boundary Condition a Set Picking Preferences • Select Preferences / Picking • Choose Enclose Centroid for Rectangle/Polygon Picking. • Click Close. b c

  19. Step 5. Create Boundary Condition Create the boundary condition • Loads/BCs: Create / Displacement / Nodal. • Enter bolt_hole as the New Set Name. • Click Input Data. • Enter <0 0 0> for Translations • Click OK. a d b c e

  20. Step 5. Create Boundary Condition c d Apply the boundary condition • Click Select Application Region. • For the Geometry Filter select FEM. • Click on Front View Icon. • Zoom in using View Corners. • Polygon pick nodes on the bolt hole. • Click Add. • Click OK. • Click Apply. b f c a g h

  21. Step 6. Create Load Create the pressure load • Loads/BCs: Create / Pressure / Element Uniform. • Enter clamp_pressure as the New Set Name. • Click Input Data. • Enter 1 for the Pressure. • Click OK. a d b c e

  22. Step 6. Create Load c d Apply the pressure load • Click Select Application Region. • For the Geometry Filter select FEM. • Click on Bottom View Icon. • Click on Fit View Icon. • Rectangular pick the top surface of solid elements as shown. • Click Add. • Click OK. • Click Apply. b e f g a h

  23. Step 7. Define Material Properties Create an isotropic material • Materials: Create / Isotropic / Manual Input. • Enter titanium as the Material Name. • Click Input Properties. • Enter 109e3 for the elastic modulus and 0.3 for the Poisson Ratio. • Click OK. • Click Apply. a d b c f e

  24. Step 8. Create Physical Properties Create element properties • Properties: Create / 3D / Solid. • Enter solid as the Property Set Name. • Click Input Properties. • Click on the Select Material Icon. • Select titanium as the material. • Click OK. a d b c e f

  25. Step 8. Create Physical Properties Apply the element properties • Click in the Select Members box. • Select the Solid Element filter. • Rectangular pick all elements as shown. • Click Add. • Click Apply. b c a d e

  26. Step 9. Run Linear Static Analysis Choose the analysis type • Analysis: Analyze / Entire Model / Full Run. • Click Solution Type. • Choose Linear Static. • Click OK. • Click Apply. a c b d e

  27. Step 10. Plot Displacements and Stresses Attach the results file • Analysis: Access Results / Attach XDB / Result Entities. • Click Select Results File. • Choose the results file clamp.xdb. • Click OK. • Click Apply. a c d b e

  28. Step 10. Plot Displacements and Stresses Create a deformation plot for the mid span result case • Results: Create / Quick Plot. • Select Stress Tensor as the Fringe Result. • Select Von Mises as the Fringe Result Quantity. • Select Displacements, Translational as the Deformation Result. • Click Apply. a b c d e

More Related