内容文本msc.patran courses课程plate

1、WORKSHOP 16STIFFENED PLATEWorkshop ObjectivesCreate a model of a plate with two types of stiffeners. For one type of stiffener, the arbitrary beam section calculator in Patran will be used to obtain the cross-section properties. For the other type of stiffener, the Patran standard beam Library will

2、be used to obtain the cross-section properties. The model is finished, i.e. create constraints and pressure loading. An analysis of the model is performed, and the results viewed using MD Nastran and Patran.Problem DescriptionShow the stress for the plate or beam elements on the deformed shape of th

3、e modelAll material: Aluminum with E = 10 x 106 psi and n = 0.3Pressure on piston = 5 psiSoftware VersionPatran v2008r1MSC Nastran 2008r1Key Concepts and StepsDatabase: create a new database with Analysis Code = MD Nastran and Analysis Type = StructuralGeometry: create the surfaces that are to repre

4、sent the plateElements: mesh the surfaces with plate elements, and mesh select edges of the surfaces with bar elementsLoads/BCs: apply a simply supported constraint on two opposing edges of the plate, and apply a pressure to the surface of the plateMaterials: specify an isotropic material for Alumin

5、umProperties: create a 2D plate property for the plate, and a 1D beam property for each of the two types of stiffenersAnalysis: Solution Type = Nastran Linear Static, Solution Sequence = 101, Method = Full RunAnalysis: access analysis results by attaching the XDB file to databaseResults: plot von Mi

6、ses stress for plate elements, bar stress for bar elements, and displacement results for eachCreate New DatabaseCreate a new database called stiffened_plate.db:File / NewEnter stiffened_plate as the File name.Click OK.Choose Default Tolerance.Select MSC.Nastran as the Analysis Code.Select Structural

7、 as the Analysis Type. Click OK. bcdefagStep 1. Geometry: Create / Surface / XYZCreate the surface:Geometry: Create / Surface / XYZEnter for the Vector Coordinate List.Click Apply.abcStep 1. Geometry: Create / Curve / XYZ (Cont.)Turn on the Show Parametric Direction feature:Display : Geometry.Check

8、the Show Parametric Direction box.Click Apply.Click Cancel.bcdaStep 2. Geometry: Edit / Surface / BreakBreak the surface in the u-direction: Geometry : Edit / Surface / Break Change the Option to Parametric.Choose Constant u Direction as the Break Direction.Enter 0.5 as the Break Curve value.For Sur

9、face List screen pick the surface created earlier.Answer Yes when the question “Do you wish to delete the original surfaces?” appears.abcdeeStep 2. Geometry: Edit / Surface / Break (Cont.)Break the surfaces again in the u-direction. Screen pick the bottom surface.Answer Yes when the question “Do you

10、 wish to delete the original surfaces?” appears.Screen pick the top surface.Answer Yes when the question “Do you wish to delete the original surfaces?” appears.Click on the Cycle Show labels icon.caeacStep 3. Finite Elements: Create / Mesh / SurfaceGenerate plate elements using IsoMesh: Elements: Cr

11、eate / Mesh / SurfaceSelect Quad / IsoMesh / Quad4.For Surface List select all the surfaces.Uncheck Automatic Calculation and enter 2.0 as the Global Edge Length Value.Click Apply.Click the Cycle Show labels icon to hide labels.abcdehStep 3. Finite Elements: Create / Mesh / Curve (Cont.)Generate bar

12、 elements along the longitudinal edges of the surfaces:Elements: Create / Mesh / CurveChoose Bar2 as the element Topology. Shift select 5 horizontal surface edges as shown.Uncheck: Automatic Calculation, and enter 2.0 as the Global Edge Length Value.Click Apply. abcdceStep 4. Finite Element: Equival

13、ence / All / Tolerance CubeEquivalence the model nodes to connect elements along surface edges:Elements: Equivalence / All / Tolerance Cube Click Apply. Display : GeometryUncheck: Show Parametric Direction.Click Apply then CancelabdceStep 5. Material: Create / Isotropic / Manual InputDefine a materi

14、al for the model: Material: Create / Isotropic / Manual Input Enter alum for the Material Name.Click on Input Properties.Enter: Elastic Modulus: 10e6 Poisson Ratio: 0.3 Density: 0.101Click OK. Click Apply. deabcgStep 6. Element Properties: Create / 2D / ShellCreate element properties for the plate e

15、lements: Properties: Create / 2D / Shell Enter plate as the Property Set Name. Click on the Input Properties. Click on the Mat Prop Name icon.Click on alum in the Select Existing Material window. Enter 0.1 as the Thickness. Click OK.Click on Select Application Region.fabchdgStep 6. Element Propertie

16、s: Create / 2D / Shell (Cont.)For Select Members select all surfaces.Click Add and OK.Click Apply.ikjjiStep 7. Element Properties: Create / 1D / BeamCreate element properties for the hat stiffeners: Properties: Create / 1D / Beam Enter hat_stiffener as the Property Set Name. Change Options to Genera

17、l Section (CBEAM).Click on the Input Properties. Click on the Mat Prop Name icon.Click on alum in the Select Existing Material window. Enter for the Bar Orientation.Click on the Beam Library Icon.gabcehdStep 7. Element Properties: Create / 1D / BeamChange the Object to Arbitrary Shape.Type a new sec

18、tion name of hat_section.ijStep 7. Element Properties: Create / 1D / BeamGo to Group Create.Type a new group name of cross_section.Check box next to Unpost All Other Groups.Press the Apply button.klmnStep 7. Element Properties: Create / 1D / BeamGo to File Import.Make sure the Object is Model and th

19、e Source is Parasolid xmt.Select the file called hat_sect_surface.xmt.Apply.This will import a pre-defined geometry file containing a surface representing the cross-section of the hat stiffener.qsoprStep 7. Element Properties: Create / 1D / BeamReturn to the Beam Library window, make sure your Optio

20、n is on Select Surface and select the imported surface from step r.Click OK and notice the X-Y point locations that have been discretized from the surface selected.Click the Calculate/Display button.After reviewing the calculated section properties, close the section display window.tuvwStep 7. Eleme

21、nt Properties: Create / 1D / BeamNow define the stress recovery points on the sectionClick on Display BoundaryThe picture that comes up shows the positions on the section of the points in the spreadsheet. Scroll down to point 45 and click in its cell in the Stress Rec columnChoose Point C from the S

22、tress Recovery drop-downRepeat for spreadsheet points 24, 22 and 1, selecting Point D, Point E and Point F respectivelyClick OKxzaaybbStep 7. Element Properties: Create / 1D / BeamddccffNotice that the name of the section you just created is now in the Section Name databox.Input the offsets of node

23、1 and 2 as to adjust the section location relative to the location on the panel itself.Scroll down to see the locations of the C, D, E and F stress recovery pointsClick OK on the Input Properties form.eeStep 7. Element Properties: Create / 1D / Beam (Cont.)Go to Group/Post and post only default_grou

24、pClick on Select Application Region.Click under Select Members, then click on the Beam element filter.For the application region select the three rows of bar elements as shown. Click Add and OK.Click Apply.hhiijjkkkklliijjggStep 7. Element Properties: Create / 1D / Beam (Cont.)Next, create element p

25、roperties for the I-beam stiffeners: Properties: Create / 1D / Beam Enter i_stiffener as the Property Set Name. Make sure the Options setting is on General Section (CBEAM).Click on the Input Properties button.Click on the Mat Prop Name icon and select alum in the Select Existing Material window. Ent

26、er for Bar Orientation. Enter for the Offset Node1 and 2.Click on the Beam Library icon.fgabcehdStep 7. Element Properties: Create / 1D / Beam (Cont.)Enter i_section for New Section Name. Select the I-Beam shape option. Enter dimensions for the I-Beam as shown in the table.Click on Calculate/Display

27、 to view the cross section. Close the display window after reviewing.Click OK.Click OK in the Input Properties form.Click on Select Application Region.iklmojDimensionValueH2.0W11.0W21.0t0.1t10.1t20.1kStep 7. Element Properties: Create / 1D / Beam (Cont.)Click under Select Members and select the Curv

28、e or Edge icon.For the application region, select the top and bottom edges of the plate.Click Add then OK.Click Apply.rrsqppqqStep 8. Viewing / Angles Change the viewing angle:Viewing : Angles. Select Model Absolute.Input 23.0 34.0 0.0 as the Angles.Click Apply.Click CancelbcdeaStep 9. Display / Loa

29、d/BC/Elem PropsChange the display settings to show beam offset:Display : Load/BC/Elem. Props Change Beam Display from 1D:Line to 1D:Line+Offsets and click Apply. Change Beam Display to 2D:MidSpan+Offsets and click Apply.Change Beam Display to 3D:FullSpan+Offsets and click Apply.Click Cancel. bcdabeS

30、tep 9. Display / Load/BC/Elem Props (Cont.)1D + Offsets2D + Offsets3D + Offsets1DStep 9. Element Properties: ShowVerify the orientation of the sections by plotting the element y axis:Properties : ShowSelect Bar Orientation in the properties window.Select the default_group.Click Apply.abcdaStep 9. Di

31、splay / Load/BC/Elem Props (Cont.)Change the display of loads, boundary conditions, and element properties from geometry to finite elements.Display/Load/BC/Elem. Props. Check the Show on FEM only box.Click Apply.Click Cancel.Repeat steps from previous page. The y-axis of the stiffener elements will

32、be plotted.bcdStep 10. Loads/BCs: Create / Displacement / NodalCreate the boundary condition for the model: Loads/BCs: Create / Displacement / Nodal Enter Simple_Support as the New Set Name. Click on the Input Data button. Enter for the Translations. Click OK. Click on Select Application Region. Sel

33、ect Geometry as the Geometry Filter. Set the picking filter to Curve or Edge.For Select Geometry Entities shift select the left and right edges of the plate.Click Add.Click OK. Click Apply. deikabcfljhgStep 10. Loads/BCs: Create / Displacement / NodalStiffened plate with two edges constrained.Step 1

34、1. Loads/BCs: Create / Pressure / Element UniformApply pressure to the model:Loads/BCs: Create / Pressure / Element Uniform Enter pressure as the New Set Name.Select 2D as the Target Element Type. Click on the Input Data button.Enter 5 in the Top Surf Pressure field. Click OK. Click on Select Applic

35、ation Region button. Select Geometry as the Geometry Filter. Set the picking filter to Surface or Face.Select all the surfaces for the Application Region. Click Add, and OK. Click Apply. efhkabcdlkgijStep 11. Loads/BCs: Create / Pressure / Element Uniform (Cont.)Stiffened plate model with applied pressure.Step 12. Analysis: Analyze / Entire Model / Full RunSubmit the model for analysis: Analysis: Analyze / Entire Model / Full Run Click on the Solution Type