1 / 40

WS8A- 1

WORKSHOP 8A TENSION COUPON. NAS120, Workshop 8A, November 2003. WS8A- 1. Problem Description A tension coupon is constructed from aluminum with E = 10 x 10 6 psi and n = 0.3 The coupon thickness is 0.125 in An edge load of 50 lb is applied to the tension coupon. 10 in. 4 in. 50 lb.

juanitat
Download Presentation

WS8A- 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 8A TENSION COUPON NAS120, Workshop 8A, November 2003 WS8A-1

  2. Problem Description • A tension coupon is constructed from aluminum with E = 10 x 106 psi and n = 0.3 • The coupon thickness is 0.125 in • An edge load of 50 lb is applied to the tension coupon

  3. 10 in 4 in 50 lb 2.0 DIA Hole

  4. Workshop Objectives • Build the tension coupon geometry • Control the mesh by using techniques discussed in class • Compare FEA stress results to theoretical results From “Stress Concentration Factors” by R. E. Peterson, Figure 86: smax = 432 psi

  5. Suggested Exercise Steps • Create a new database. • Create a geometry model of the tension coupon. • Use Mesh Seeds to define the mesh density. • Create a finite element mesh. • Verify the finite element mesh. • Define material properties. • Define element properties and apply them to the model. • Apply boundary conditions to the model. • Apply loads to the model. • Submit the model to MSC.Nastran for analysis. • Post Process results using MSC.Patran.

  6. Step 1. Create New Database a a • Create a new database called tension_coupon_a.db. • File / New. • Enter tension_coupon_a 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 • Create the first curve. • Geometry: Create / Curve / XYZ. • Enter <0 4 0> for the Vector Coordinate List. • Enter [0 0 0] for the Origin Coordinate List. • Click Apply. a b c d

  8. Step 2. Create Geometry Create the second curve by translating the first curve. • Geometry: Transform / Curve / Translate. • Enter <10 0 0> for the Translation Vector. • Click in the Curve List box and screen pick the first curve. a b c

  9. Step 2. Create Geometry Create two more curves • Geometry: Create / Curve / Point. • Screen pick the point at the bottom of the left curve. • Screen pick the point at the bottom of the right curve. A curve is automatically created because Auto Execute is checked. • Screen pick the top of the left curve. • Finish creating the top curve by screen picking the point at the top of the right curve as shown. a d e b c

  10. Step 2. Create Geometry Create a chain curve • Geometry: Create / Curve / Chain. • Rectangular pick all four curves. • Click Apply. • When the message box appears, choose Yes to delete the original curves. a b c d

  11. Step 2. Create Geometry Create a circle • Geometry: Create / Curve / 2D Circle. • For the circle radius, enter 1.0. • For the Center Point List, enter [5 2 0]. • Click Apply. a b c d

  12. Step 2. Create Geometry h Create a trimmed surface • Geometry: Create / Surface / Trimmed / Option: Planar. • Click in the Outer Loop List box. • Screen pick the outer curve. • Click in the Inner Loop List box. • Screen pick the inner circle. • Click Apply. • When the message boxes appear, choose Yes to delete the original curves. • Click the Refresh Graphics icon a c e b d f g

  13. Step 2. Create Geometry Create two more circles • Geometry: Create / Curve / 2D Circle. • For the circle radius, enter 1.1. • For the Center Point List, enter [5 2 0]. • Click Apply. • Repeat this procedure for a circle with a radius of 1.2. a b c d

  14. Step 2. Create Geometry Associate the two curves to the surface • Geometry: Associate / Curve / Surface. • Select the Curve filter. • Rectangular pick both circles. • Screen pick the trimmed surface. a b c d

  15. Step 3. Create Mesh Seeds Create a uniform mesh seed • Elements: Create / Mesh Seed / Uniform. • Enter 48 for the Number of Elements. • Click in the Curve List box. • Select the Curve or Edge element filter. • Rectangular pick the two circles and the edge of the hole. a d e b c

  16. Step 3. Create Mesh Seeds Create a biased mesh seed • Elements: Create / Mesh Seed / Two Way Bias. • Enter 20 for the Number of Elements. • Enter 0.25 for L2/L1. • Click on the Curve List box. • Screen pick the top edge of the surface, as shown. • Screen pick the bottom edge of the surface to apply the mesh seed there as well. a e b c f d

  17. Step 4. Create Mesh Create a finite element mesh • Elements: Create / Mesh / Surface. • Set the Element Shape to Quad, Mesher to Paver, and Topology to Quad4. • Click in the Surface List box. • Screen pick the surface as shown. • Enter 1.0 as the value for Global Edge Length. • Click Apply. a b d c e f

  18. Step 5. Verify Mesh Verify the quality of the finite elements • Elements: Verify / Quad / All. • Click Apply. • Review the summary table. a c b

  19. Step 5. Verify Mesh Perform specific quality tests on the elements. • Elements: Verify / Quad / Aspect. • Click Apply. • Review the fringe plot. • Repeat for Warp, Skew, and Taper tests. • Reset Graphics. a c d e b

  20. Step 6. Create Material Properties Create an isotropic material • Materials: Create / Isotropic / Manual Input. • Enter aluminum as the Material Name. • Click Input Properties. • Enter 10e6 for the elastic modulus and 0.3 for the Poisson Ratio. • Click OK. • Click Apply. a d b c f e

  21. Step 7. Create Element Properties Create element properties • Properties: Create / 2D / Shell. • Enter plate as the Property Set Name. • Click Input Properties. • Click on the Select Material Icon. • Select aluminum as the material. • Enter 0.125 for the thickness. • Click OK. a d f b c e g

  22. Step 7. Create Element Properties Select application region • Click in the Select Members box. • Screen pick the surface as shown. • Click Add. • Click Apply. b a c d

  23. Step 8. Apply Boundary Conditions Create the boundary condition • Loads/BCs: Create / Displacement / Nodal. • Enter fixed as the New Set Name. • Click Input Data. • Enter <0 0 0> for Translations and <0 0 0> for Rotations. • Click OK. a d b c e

  24. Step 8. Apply Boundary Conditions Apply the boundary condition • Click Select Application Region. • Select the Curve or Edge filter. • Select the left edge of the surface as the application region. • Click Add. • Click OK. • Click Apply. b c d e a f

  25. Step 8. Apply Boundary Conditions The boundary condition should agree with what’s shown on the right

  26. Step 9. Apply Loads Create the load • Loads/BCs: Create / Total Load / Element Uniform. • Enter force as the New Set Name. • Set the Target Element Type to 2D. • Click Input Data. • Enter <50 0 0> for the Edge Load. • Click OK. a e b c d f

  27. Step 9. Apply Loads Apply the load • Click Select Application Region. • For the application region select the right edge of the surface as shown. • Click Add. • Click OK. • Click Apply. b c a d e

  28. Step 9. Apply Loads The loads and boundary condition should agree with what’s shown on the right.

  29. Step 10. Run Linear Static Analysis Analyze the model • Analysis: Analyze / Entire Model / Full Run. • Click Solution Type. • Choose Linear Static. • Click OK. • Click Apply. a c b d e

  30. Step 11. Post Process with MSC.Patran Attach the results file • Analysis: Access Results / Attach XDB / Result Entities. • Click Select Results File. • Choose the results file tension_coupon_a.xdb. • Click OK. • Click Apply. a c d b e

  31. Step 11. Post Process with MSC.Patran a Erase geometry • Display: Plot/Erase. • Under Geometry click Erase. • Click OK. b c

  32. Step 11. Post Process with MSC.Patran Create a general Quick Plot • Results: Create / Quick Plot. • Select Stress Tensor as the Fringe Result. • Select Von Mises as the Fringe Result Quantity. • Click Apply. a b c d

  33. Step 11. Post Process with MSC.Patran Create a Quick Plot of X Component Stress • Results: Create / Quick Plot. • Select Stress Tensor as the Fringe Result. • Select X Component as the Fringe Result Quantity. • Click Apply. • Record the maximum X component stress. Max X Stress = ________ a b c d

  34. Step 11. Post Process with MSC.Patran Create a fringe plot of X Component Stress • Results: Create / Fringe. • Select Stress Tensor as the Fringe Result. • Select X Component as the Fringe Result Quantity. • Click Apply. • Record the maximum X component stress. Max X Stress = ________ a b c d

  35. Step 11. Post Process with MSC.Patran • By default, MSC.Nastran presents element stress results in the element coordinate system. • For the Fringe Plot option, MSC.Patran takes the MSC.Nastran results and plot them as is. • For the Quick Plot option, MSC.Patran automatically transforms the stress results into the basic coordinate system first before plotting them.

  36. Step 11. Post Process with MSC.Patran Show the element coordinate systems • Elements: Show / Element / Coord.Sys • Rectangular pick the entire surface. • Note the various orientations of the X direction. • Click reset graphics. a b d

  37. Step 11. Post Process with MSC.Patran Create another fringe Plot • Results: Create / Fringe. • Select Stress Tensor as the Fringe Result. • Select X Component as the Fringe Result Quantity. • Click on the Plot Options Icon. • Set the coordinate transformation to CID. • Screen pick coordinate frame 0. • Click Apply. a d e b f c g

  38. Step 11. Post Process with MSC.Patran View the revised results • Note the change in maximum stress. Max X Stress = _________

  39. Step 11. Post Process with MSC.Patran Turn off averaging • Set the Averaging Definition Domain to None. • Click Apply. a b

More Related