WS16-1 PAT301, Workshop 16, October 2003 WORKSHOP 16 CONNECTING ROD USING 1D AND 2D ELEMENTS. - презентация

1 WS16-1 PAT301, Workshop 16, October 2003 WORKSHOP 16 CONNECTING ROD USING 1D AND 2D ELEMENTS

2 WS16-2 PAT301, Workshop 16, October 2003

3 WS16-3 PAT301, Workshop 16, October 2003 Problem Description u The model to be created in this workshop is for a connecting rod that would typically be found in a large displacement internal combustion gasoline engine. The part is about 10 long, 4 wide, and 1 thick. There are several ways the con rod can be modeled. For this exercise a combination of 1D(beam) and 2D(plate) elements are to be used. The model to be created has very few nodal degrees-of-freedom. This will provide an analyst with a model that can be analyzed very quickly, making it possible to perform a parametric study with many sub-cases. u The workshop will begin by using existing parametric(green) surfaces. From these surfaces curves are to be created. Some of the surfaces are to be meshed. Then, the nodes of the 2D plate elements are to be moved. 1D beam elements are to be created on the free(external) edges of the plate elements. The workshop will proceed creating the remainder of the 1D/2D model. Finally, the model will be analyzed.

4 WS16-4 PAT301, Workshop 16, October 2003 Suggested Exercise Steps 1. Create a new database called connecting_rod.db. 2. Import an IGES file called conrod.igs. 3. Extract curves from a parametric surfaces at perimeter(outside edge of connecting rod). 4. Create several short curves to complete creating curves along the perimeter of connecting rod(rod) model. 5. Mesh the surfaces at the web portion of the rod, and equivalence. 6. Move plate element nodes at the perimeter of the web to adjacent curves at the perimeter of the rod model. 7. Project more web perimeter nodes to adjacent curves. 8. Zoom into the area of the model where plate elements are to be created manually. 9. Create plate elements manually by selecting geometric points. 10. Create beam elements on free edges of plate elements. 11. Mesh arc curves, at piston and crank shaft, with beam elements. 12. Equivalence nodes again. 13. Create constraints at the crank shaft. Not all displacements and rotations are to be constrained.

5 WS16-5 PAT301, Workshop 16, October 2003 Suggested Exercise Steps 14. Create cylindrical coordinate system at the piston(top of model). The coordinate system is to be used in defining distributed loading that will represent pressure effects on the rod. 15. Create a spatial field(function) for the distributed load. It will be a sine loading. 16. Create the distributed load. 17. Define the material property. 18. Define element properties. There will be 1D beam and 2D plate properties. For the 1D beam properties the Beam Library is to be used. 19. Run the analysis. 20. Access the MSC.Nastran results file by attaching the XDB file. 21. Create a plot of the deformed shape of the model. 22. Create stress fringe plots on the deformed shape. There will be one for the 2D plate stress and another for the 1D beam elements.

6 WS16-6 PAT301, Workshop 16, October 2003 Step 1. Create a Database Create a new database called connecting_rod.db. a.File / New. b.Enter connecting_rod 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

7 WS16-7 PAT301, Workshop 16, October 2003 Step 2. Import conrod.igs b c a d f e Import an existing IGES file. a.File / Import. b.Object : Model. c.Source : IGES. d.Current Group : default_group. e.Select conrod.igs. f.Click Apply. g.Click OK in Import Summary window.

8 WS16-8 PAT301, Workshop 16, October 2003 Step 2. Import conrod.igs (Cont.) Shade the surfaces by selecting Smooth shaded view icon.

9 WS16-9 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface Change the view port display and zoom in on the web section of the connecting rod. a.Click on the Wireframe icon. b.Use Label control to turn on surface labels. c.Select View corners icon and zoom in by picking the corners as shown in the figure. a c b

10 WS16-10 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Extract curves for the flange. a.Geometry: Create / Curve / Extract. b.Option: Parametric. c.Curve Direction: v Direction. d.Curve Position: 0.5. e.Click on Surface List and select on the following surfaces: Surface 1, 2, 4, and 5. (See figure for details) a b c d e e Note that it is not necessary to click apply when the Auto Execute is selected.

11 WS16-11 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Extract several more curves. a.Curve Direction: u Direction. b.Click on Surface List and select on the following surfaces: Surface 3 and 6. (See figure for details) a b b

12 WS16-12 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Extract curves for the piston and crank shaft sections of the model. a.Select Fit view icon. b.Set the picking to Enclose entire entity under Preferences/Picking. c.Curve Direction: u Direction. d.Click on Surface List and select all top circular surfaces as shown in the figure. (surf and 23). e.Again, click on Surface List and include all arc surfaces at the bottom, except 14 and 16. f.Curve Direction: v Direction. g.Click on Surface List to include surface 14 and 16. a c d d b e

13 WS16-13 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Observe the extracted curves, particularly the curve at the bottom of the crank shaft. a.Your figure should look like the following. Zoom into the bottom circle frame by selecting View corners icon. b.Notice how the curve extracted from surface 26 does not line up with the adjacent curves. c.This problem is solved by deleting the existing curve, refitting Surface 26, and creating a new curve. a c b

14 WS16-14 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Delete the misaligned curve. a.Geometry: Delete / Curve. b.Click on Curve List and select the curve extracted from Surface 26. c.Apply. a b c b

15 WS16-15 PAT301, Workshop 16, October 2003 Step 3. Extract Curve from Parametric Surface (Cont.) Refit the section of the model with the deleted curve and extract a curve from the refit surface. a.Geometry: Edit / Surface / Refit. b.Click on Surface List and select Surface 26. c.Click Yes when asked to create a duplicate surface, and Yes again to delete the original surface. d.Create / Curve / Extract. e.Curve Direction: u Direction. f.Click on Surface List and select Surface 31. g.Now the curve extracted from Surface 31 should match the other extracted curves. a b b

16 WS16-16 PAT301, Workshop 16, October 2003 Step 4. Create a Curve Zoom into a section of the model to create several curves. a.Select Fit view icon. b.Select View corners icon and zoom in by picking the corners as shown in the figure. c.Geometry: Create / Curve / Normal. a b

17 WS16-17 PAT301, Workshop 16, October 2003 Step 4. Create a Curve (Cont.) Create the normal curve. a.Click under Point List and select Point 50. b.Click under Curve List and select Curve 9. Curve 9 Point 50 a b

18 WS16-18 PAT301, Workshop 16, October 2003 Step 4. Create a Curve (Cont.) Break the curve at the intersection point of the normal curve and the extracted curve. a.Geometry: Edit / Curve / Break. b.Click under Curve List and select Curve 9. c.Click under Break Point List and select Point 77. d.Click Yes to delete the original curve. e.Turn on Label Control and switch to Curve. You should have three curves. a b c e e Point 77 Note that point, curve, and surface labels may not match, depending on the order certain curves are selected.

19 WS16-19 PAT301, Workshop 16, October 2003 Step 4. Create a Curve (Cont.) Create the remaining normal curves and break with them. a.Repeat these steps 3 more times in different places. In each location create a normal curve, and break a curve with it a Curve #Point used to create normal Point used to break curve Above is a table showing the curve numbers and the corresponding points to use in creating the normal and breaking the curve. Note that point, curve, and surface labels may not match, depending on the order certain curves are selected. 1 23

20 WS16-20 PAT301, Workshop 16, October 2003 Step 5. Mesh Surface Create a mesh for the web. a. Elements: Create / Mesh / Surface. b.Click on Label Control and select Surface. c.Elem Shape: Quad. d.Mesher: IsoMesh. e.Topology: Quad4. f.Click on Surface List and select Surface 8, 7, 10, 11, 12, 9. g.Global Edge Length: h.Click on Apply. a b c d e f g h b f

21 WS16-21 PAT301, Workshop 16, October 2003 Step 5. Mesh Surface (Cont.) Observe the meshed section of the model and note the duplicate nodes. Remove the duplicate nodes by equivalencing the model. a. Click on the Label control icon and turn on the Node labels. b. Click the View Corners icon and zoom in on a section of the meshed area. c. Elements : Equivalence / All / Tolerance Cube. d. Click Apply. a Note the above illustration. There are duplicate labels at the node location, indicating that there are two nodes at that location. Equivalencing the model removes the duplicate nodes, producing the model illustrated at the right.

22 WS16-22 PAT301, Workshop 16, October 2003 Step 6. Move Node to a Midway Position Move the nodes to the extracted curves. a.Elements: Modify / Node / Move. b.Use Label Control to turn off surface labels and turn on node labels. c.Make sure Auto Execute is on to make picking more rapid. d.Click on Node List and select Node 18. e.Under New Node Locations select Point 50. f.Click on Node List and select Node 12. g.Under New Node Locations select Point 53. Node 18 Point 50 Node 12 Point 53 b c e f Element edges follow element nodes. Note that the node numbers may not necessarily match those indicated in the exercise.

23 WS16-23 PAT301, Workshop 16, October 2003 Step 6. Move Node to a Midway Position (Cont.) Continue to move the nodes out to a new location. a.Click on Node List and select Node 39. b.Under New Node Locations select Point 55. c.Click on Node List and select Node 36. d.Under New Node Locations select Point 56. Node 39 Point 55 Node 36 Point 56 a b

24 WS16-24 PAT301, Workshop 16, October 2003 Step 6. Move Node to a Midway Position (Cont.) a.Your model should look like the following.

25 WS16-25 PAT301, Workshop 16, October 2003 Step 7. Project Node to a Curve a.Elements: Modify / Node / Project. b.Project onto: Curve. c.Direction: Normal. d.Click on Label Control and show curve labels. e.Turn Auto Execute on. f.Click on Input Nodes and select Node 17. g.Under Curve List, select Curve 1. h.Repeat this procedure, for Node 16, Node 15, and Node 14, projecting onto Curve 1. Curve 1 Node 17 Node 16 Node 15 a b c f g d e

26 WS16-26 PAT301, Workshop 16, October 2003 Step 7. Project Node to a Curve (Cont.) Project nodes onto the extracted curve. a.Click on Input Nodes and select Node 10. b.Under Curve List, select Curve 3. c.Repeat this procedure, for Node 8, Node 6, and Node 4, projecting onto Curve 3. Curve 3 Node 10 a b

27 WS16-27 PAT301, Workshop 16, October 2003 Step 7. Project Node to a Curve (Cont.) Project the remaining nodes onto the curve. a.Click on Input Nodes and select Node 13. b.Under Curve List, select Curve 2. c.Click on Input Nodes and select Node 25. d.Under Curve List, select Curve 2. a b

28 WS16-28 PAT301, Workshop 16, October 2003 Step 7. Project Node to a Curve (Cont.) Finish projection of the nodes. a.Click on Input Nodes and select Node 2. b.Under Curve List, select Curve 4. c.Click on Input Nodes and select Node 30. d.Under Curve List, select Curve 4. a b

29 WS16-29 PAT301, Workshop 16, October 2003 Step 7. Project Node to a Curve (Cont.) Your model should look like the following

30 WS16-30 PAT301, Workshop 16, October 2003 Step 8. Zoom Into Model Zoom in on a section of the model where Quad elements will be created manually. a.Select Fit view icon. b.Turn off the curve and node labels. c.Select View corners icon and zoom in by picking the corners as shown in the figure. a c b c

31 WS16-31 PAT301, Workshop 16, October 2003 Step 9. Create Quad Elements Create several quad elements for the upper section of the model. a.Elements: Create / Element / Edit. b.Shape: Quad. c.Topology: Quad4. d.Pattern: Standard. e.Use Label Control and turn on Point labels, and increase Point size. f.Click on Node 1 then select on Point picking icon. g.Select Point 50, Point 10, Point 57 and Point 77. h.An element has just been created. a b c d e f g f

32 WS16-32 PAT301, Workshop 16, October 2003 Step 9. Create Quad Elements (Cont.) Continue creating more quads. a.Create another element by selecting Point 10, Point 53, Point 78 and Point 57. a

33 WS16-33 PAT301, Workshop 16, October 2003 Create the quad elements for the lower section of the model. a.Select Fit view icon. b.Select View corners icon and zoom in by picking the corners as shown in the figure. a b Step 9. Create Quad Elements (Cont.) b

34 WS16-34 PAT301, Workshop 16, October 2003 Step 9. Create Quad Elements (Cont.) Finish creating the quad elements. a.Click on Node 1, and select Point 80, Point 71, Point 9 and Point 55. b.Now do the same creating another element using Point 71, Point 79, Point 56 and Point 9. a b a

35 WS16-35 PAT301, Workshop 16, October 2003 Step 9. Create Quad Elements (Cont.) b c a Observe all the created quad elements. a.Using Label Control turn off point labels and turn on element labels, and reduce point size. b.Select Fit view icon. c.Select View Corners icon and zoom in by picking the corners as needed.

36 WS16-36 PAT301, Workshop 16, October 2003 Step 10. Create Bar2 Elements on Free Edge of Quad4 Create a Bar2 element on a free edge of a Quad4 element. a.Elements: Create / Element / Edit. b.Shape: Bar. c.Topology: Bar2. d.Pattern: Elem Edge. e.Click on Edge then select on Free edge of element icon. f.Select outside edge of Element 10. g.This will create a Bar2 element on the free edge of Element 10. (Element 19) h.Create Bar2 elements on all the remaining Quad4 free edges, including those along the circular arcs at the piston and crank shaft. a b c d e f h e

37 WS16-37 PAT301, Workshop 16, October 2003 Step 10. Create Bar2 Elements on Free Edge of Quad4 (Cont.) All Bar2 elements have been created for Quad4 free edges.

38 WS16-38 PAT301, Workshop 16, October 2003 Step 11. Isomesh a Curve with Bar2 Elements Curve 13 a b d f d c e Create a mesh curve for the upper section of the connecting rod. a.Elements : Create / Mesh / Curve. b.Topology : Bar2. c.Select Curve under Label Control. d.Click on Curve List and select Curve 13. e.Secify the Global Edge Length to be f.Click on Apply.

39 WS16-39 PAT301, Workshop 16, October 2003 Step 11. Isomesh a Curve with Bar2 Elements (Cont.) a.Curve 13 is meshed. b.Now mesh all remaining circular arc curves at the piston and crankshaft. Curve 13 Meshed

40 WS16-40 PAT301, Workshop 16, October 2003 Step 11. Isomesh a Curve with Bar2 Elements (Cont.) a.Using Label Control turn off the Curve labels. b.All curves are meshed. c.Shown are the Quad4 and Bar2 elements.

41 WS16-41 PAT301, Workshop 16, October 2003 Step 12. Equivalence All Nodes Turn off all the labels and equivalence the model again. a.Under Label Control, turn off all of the labels. b.Elements: Equivalence / All / Tolerance Cube. c.Apply. b c a

42 WS16-42 PAT301, Workshop 16, October 2003 Step 13. Constrain at the Crankshaft Create the constraints for the model at the crank shaft. a.Loads / BCs: Create / Displacement / Nodal. b.Current Load Case: Default…. c.Select on New Set Name and enter fix_at_crank. d.Input Data. e.Enter for Translations and Rotations. f.OK. g.Select Application Region. a b c d e f g

43 WS16-43 PAT301, Workshop 16, October 2003 Step 13. Constrain at the Crankshaft (Cont.) a.Geometry Filter: Geometry. b.Increase the size of the Point markers. c.Click on Application Region/Select Geometry Entities and select the eight curves indicated in the figure. d.Add. e.OK. f.Apply. c a b d e c

44 WS16-44 PAT301, Workshop 16, October 2003 Step 13. Constrain at the Crankshaft (Cont.) f

45 WS16-45 PAT301, Workshop 16, October 2003 Step 14. Create Cylindrical Coordinate System a.Zoom into the top of the model. b.Turn on the point labels and increase the size of the points.. c.Geometry: Create / Coord / 3Point. d.Type: Cylindrical. e.Click on Origin and select Point 2. f.Click on Point on Axis 3 and enter [x2 y2 1]. g.Click on Point on Plane 1-3 and select Point 41. Point 2 Point 41 c d e f g b a

46 WS16-46 PAT301, Workshop 16, October 2003 Step 15. Create a Spatial Field a.Fields: Create / Spatial / PCL Function. b.Enter force under Field Name. c.Field Type: Vector. d.Coordinate System Type: Real. e.Coordinate System: Coord 1. f.Enter *sinr(T) under First Component. Choose T under Independent Variables. g.Enter 0. under Second Component. h.Enter 0. under Third Component. i.Apply. a b c d e f g h i The load to be applied is a function of the cylindrical coordinate system angle.

47 WS16-47 PAT301, Workshop 16, October 2003 Step 16. Create Distributed Load a.Loads / BCs: Create / CID Distributed Load / Element Uniform. b.Select on New Set Name and enter dis_load_CID. c.Target Element Type: 1D. d.Input Data. e.Click under Distr Force and select force under Spatial Fields. f.Analysis Coordinate Frame: Coord 1. g.OK. h.Select Application Region. a b c d e f g h e Because the node spacing is not constant, it is preferable to use a distributed load. Using the MSC.Nastran preference in Patran, it is possible to use a CID distributed load. This allows a pressure load (force per-area or length) to be specified using a local coordinate system.

48 WS16-48 PAT301, Workshop 16, October 2003 Step 16. Create Distributed Load (Cont.) a.Turn off the point labels, turn on the Bar2 element labels under Display / Finite Elements, and increase the size of the node markers.. b.Geometry Filter: FEM. c.Click under Application Region/Select 1D Elements and select elements as shown in the figure. d.Add. e.OK. f.Apply. Select these 8 elements along the arc. b c d e c a a In order to have a better view of your elements, erase all curves by using Plot/Erase.

49 WS16-49 PAT301, Workshop 16, October 2003 Step 16. Create Distributed Load (Cont.) The distributed load should resemble the load illustrated here.

50 WS16-50 PAT301, Workshop 16, October 2003 Step 17. Defining Material Specify aluminum as the material of the connecting rod. 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

51 WS16-51 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties Create element properties for the 1D Bar2 elements at the piston. a.Properties: Create / 1D / Beam. b.Select Property Set Name and enter beam_at_piston. c.Select Input Properties. d.Click on Material Property Name icon and from Select Existing Material, select aluminum. e.Bar Orientation:. f.Select on Beam Library. a b c d e f

52 WS16-52 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) Define the shape, length, and width of the beam. a.Create / Standard Shape / NASTRAN Standard. b.New Section Name: piston. c.Use the right arrow to select the solid rectangular shape. d.Enter W: H: e.Select Calculate/Display. f.OK. g.OK. a b c d e f c

53 WS16-53 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Click on Select Members. b.Select on Beam element icon. c.Select all elements along the arc at the piston. d.Add. e.Apply. a b c d c

54 WS16-54 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) Create element properties for the 1D Bar2 elements at the flange. a.Properties: Create / 1D / Beam. b.Select Property Set Name and enter beam_at_flange. c.Select Input Properties. d.Click on Material Property Name icon and select aluminum from Select Existing Material menu. e.Bar Orientation:. f.Select on Beam Library. a b c d e f

55 WS16-55 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Create / Standard Shape / NASTRAN Standard. b.New Section Name: flange. c.Use the right arrow to select the solid rectangular shape. d.Enter W: H: e.Select Calculate/Display. f.OK. g.OK. a b c d e c

56 WS16-56 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Erase the geometry using Plot/Erase. b.Click on Select Members. c.Select on Beam element icon. d.Select all mid- section(flange) elements; they are between the top and bottom circular arcs. e.Add. f.Click on Apply. b c d e a

57 WS16-57 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) Create element properties for the 1D Bar2 elements at the crankshaft. a.Properties: Create / 1D / Beam. b.Select Property Set Name and enter beam_at_crank. c.Select Input Properties. d.Click on Material Property Name icon and from the Select Existing Material, select aluminum. e.Bar Orientation:. f.As before, used the Beam Library and enter the data: W: 0.5 H: g.OK. a b c d e g f

58 WS16-58 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Click on Select Members. b.Select on Beam element icon. c.Select all elements along the bottom arc at the crank- shaft as shown in the figure. d.Add. e.Click on Apply. a c d e b

59 WS16-59 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) Create element properties for the 2D Qaud4 elements at the web. a.Properties: Create / 2D / Shell. b.Select Property Set Name and enter web. c.Select Input Properties. d.Click on Material Prop Name icon and select aluminum from Select Existing Material. e.Thickness: f.OK. a b c d e f

60 WS16-60 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Plot only 2D shell elements using Plot/Erase, and turn on the element labels. b.Click on Select Members. c.Select on Shell element icon. d.Select elements 1 through 18. e.Add. f.Click on Apply. b c e f d

61 WS16-61 PAT301, Workshop 16, October 2003 Step 18. Defining Element Properties (Cont.) a.Plot Geometry and FEM using Plot/Erase, Fit view, plot several views including Iso 1 View, plot Loads/BCs markers, and turn off all labels. b.Display / Load/BC/Elem. Props… c.Beam Display: 3D: Full- Span + Offsets. d.Click on Apply. e.This is the complete 1D/2D model of the connecting rod.

62 WS16-62 PAT301, Workshop 16, October 2003 Step 19. Analysis a.Analysis: Analyze / Entire Model / Full Run. b.Job Name: connecting_rod. c.Solution Type. d.Select LINEAR STATIC. e.OK. f.Click on Apply. a d e c b f

63 WS16-63 PAT301, Workshop 16, October 2003 Step 20. Attach.xdb File a.Analysis: Access Results / Attach XDB / Result Entities. b.Click on Select Result File. c.Select and attach the file connecting_rod.xdb. d.OK. e.Click on Apply. a b c d e

64 WS16-64 PAT301, Workshop 16, October 2003 Step 21. Deformation Plot a.Results: Create / Deformation b.Select SC1:DEFAULT… under Select Result Case(s). c.Select Displacement, Translational under Select Deformation Result. d.Show As: Resultant. e.Click on Display Attributes and remove check for Show Undeformed. f.Click on Apply. g.Change the view to Front view. a b c d e f e

65 WS16-65 PAT301, Workshop 16, October 2003 Step 21. Deformation Plot (Cont.) Illustrated here is a deformation plot along with the model geometry.

66 WS16-66 PAT301, Workshop 16, October 2003 Step 22. Fringe Plot Erase the model geometry and create a fringe plot of stress. a.Click on the Plot/Erase icon and select Erase under Geometry. b.Results: Create / Fringe. c.Select Stress Tensor under Select Fringe Result. d.Select Target Entities icon. e.Target Entity: Element Types. f.Select Quad4 under Select Element Types. g.Under Display Attributes unselect Show Title and Show Max/Min Label. h.Click on Apply. d b e f h a a g c g

67 WS16-67 PAT301, Workshop 16, October 2003 Step 22. Fringe Plot (Cont.) Illustrated here is a Stress Tensor fringe plot for the Quad4 elements of the model.

68 WS16-68 PAT301, Workshop 16, October 2003 Step 22. Fringe Plot (Cont.) Plot a stress fringe for Bar2 elements. a.Under Select Results, select Bar Stresses, Maximum Combined. b.Select Target Entities icon. c.Select Bar2 under Select Element Types. d.Click on the Display Attributes icon. e.Increase the width of the bar element stress plot. f.Click on Show Max/Min Label. g.Click on Apply. h.File / Close. This ends this exercise. c f b a d e g

69 WS16-69 PAT301, Workshop 16, October 2003 Step 22. Fringe Plot (Cont.)

70 WS16-70 PAT301, Workshop 16, October 2003