加筋板静力分析课件

1、WS5-1NAS101, Workshop 5, February 2004加筋板静力分析课件WORKSHOP 5Stiffened Plate Subjected to Pressure LoadWS5-2NAS101, Workshop 5, February 2004加筋板静力分析课件Workshop 5nStiffened Plate ModeluGOAL: model a stiffened panel using plate elements for the panel and BEAM elements for the stiffenerWS5-3NAS101, Workshop

2、 5, February 2004加筋板静力分析课件Workshop 5 (cont.)nStiffened Plate ModeluWe will model a plate which is 0.1 inches thick, 20.0 inches long, and 10.0 inches wide. The stiffener is shown below, along with the plate dimensions and loadinguThe model has pinned supports at the corners WS5-4NAS101, Workshop 5,

3、February 2004加筋板静力分析课件Workshop 5 (cont.)nStiffened Plate ModeluMaterial properties:lE = 10.3E+6 psilPoissons Ratio = .3lDensity = .101 lb/in3 (weight density)uThe stiffener will be modeled using a BEAM with a PBEAML to define the cross-sectionuThe GRID points will lie at the mid-plane of the plate,

4、so the BEAM must be offset from the GRID points by 1.05 (half the BEAM height pus half the plate thickness)WS5-5NAS101, Workshop 5, February 2004加筋板静力分析课件Workshop 5 (cont.)nStiffened Plate ModelWS5-6NAS101, Workshop 5, February 2004加筋板静力分析课件Workshop 5 (cont.)nStiffened Plate ModeluPBEAML EntryPBEAML

5、,2,1,I,2.,1.,1.,.1,.1,.1uSample CBEAMCBEAM 21 2 31 32 0. 0. 1. 0. 0. 1.05 0. 0. 1.05WS5-7NAS101, Workshop 5, February 2004加筋板静力分析课件Workshop 5 (cont.)nStiffened Plate Model - Pressure Load DefinitionuPressure loads on plate and shell elements are defined using PLOAD2 or PLOAD4 entriesuSID = Static Lo

6、ading Set IDuEIDi = Element IDuP = Pressure (applied in element coordinate system)PLOAD2,1,-.5,1,THRU,20WS5-8NAS101, Workshop 5, February 2004加筋板静力分析课件Workshop 5 (cont.)WS5-9NAS101, Workshop 5, February 2004加筋板静力分析课件nSuggested Exercise Steps:Create a finite element model of the plate made of CQUAD4

7、elements.The stiffener is made of BEAM element. Define material properties. (MAT1)Define element properties and sectional properties using the BEAM library. Apply loads and boundary conditions to the model.Submit the model to MSC.Nastran for analysis.Post-Process results using MSC.Patran.WS5-10NAS10

8、1, Workshop 5, February 2004加筋板静力分析课件Create the first surfaceGeometry: Create / Surface / XYZ.Enter for the Vector Coordinate List.Use 0 0 0 as the Origin Coordinate List.a. Click Apply.Step 1: Create Finite Element ModelabcdWS5-11NAS101, Workshop 5, February 2004加筋板静力分析课件Create the second surfaceGe

9、ometry: Create / Surface / XYZ.Leave as the Vector Coordinate List.Click in the Origin Coordinates List box and screen pick point 2 as the origin.Step 1: Create Finite Element ModelabcWS5-12NAS101, Workshop 5, February 2004加筋板静力分析课件 Create mesh seeds that will be used to guide the mesh.Elements: Cre

10、ate / Mesh Seed / Uniform.For the Number of Elements, input 5.a. Select Surface 1.2 as the Curve List.Step 1: Create Finite Element ModelSurface 1.2Surface 1.1Surface 2.1abcWS5-13NAS101, Workshop 5, February 2004加筋板静力分析课件 Repeat the previous procedures to create 2 more sets of mesh seeds.Input 2 use

11、 the Number of Elements.Select Surface 1.1 as the Curve List.a. Select Surface 2.1 as the Curve List.Step 1: Create Finite Element ModelabcWS5-14NAS101, Workshop 5, February 2004加筋板静力分析课件Step 1: Create Finite Element Model Create surface mesh based on the mesh seeds assigned in the previous steps.a.

12、 Elements: Create / Mesh / Surface.b. Select Quad as the Elem Shape.c. Select IsoMesh as the Mesher.d. Enter Surface 1 2 for Surface List.e. Click Apply.abcdeWS5-15NAS101, Workshop 5, February 2004加筋板静力分析课件Step 1: Create Finite Element Model Create a curve mesh for the plate stiffeners.a. Elements:

13、Create / Mesh / Curve.b. Select Bar2 as the Element Shape.c. Enter the curves by selecting the curves off the screen Surface 1.4 1.2 2.2 for Curve List.d. Click Apply.abcdWS5-16NAS101, Workshop 5, February 2004加筋板静力分析课件Step 1: Create Finite Element Model Merge all the coincident nodes by using Equiv

14、alence function.a. Elements: Equivalence / All / Tolerance Cube.b. Click Apply.abWS5-17NAS101, Workshop 5, February 2004加筋板静力分析课件Step 2: Define Material Properties Create the material aluminum.a. Materials: Create / Isotropic / Manual Input.b. Type in alum for the Material Name.c. Click on the Input

15、 Properties button to bring up the Input Option window.d. Enter 10.3E6 for the Elastic Modulus , and 0.3 for Poisson Ratio,and 0.101 for the density.e. Click OK to return to the main material menu.f.Click Apply.abcdefWS5-18NAS101, Workshop 5, February 2004加筋板静力分析课件Step 3: Define Element Properties C

16、reate the element properties.a. Properties: Create / 2D / Shell.b. Enter plate as the Property Set Name.c. Click on the Input Properties button.d. Click on alum in the window that appears when you click the Select Material Icon.e. Enter 0.1 as the thickness for the plate.f.Click OK.g. Select element

17、 1:20 for the Application Region.(pick the element icon)h. Click Add.i.Click Apply.abcefghidWS5-19NAS101, Workshop 5, February 2004加筋板静力分析课件Step 3: Define Element Properties Create the element properties.a. Properties: Create / 1D / Beam.b. Enter beam as the Property Set Name.c. Toggle the option fr

18、om General section to Tapered Section. General section in NASTRAN means the CBAR element whereas Tapered section means CBEAM element.d. Click on the Input Properties button.e. Click on the alum in the Material Prop Name box. f.Enter the Bar Orientation and Offsets as shown.g. Click on the Beam Libra

19、ry Icon.abcdefgWS5-20NAS101, Workshop 5, February 2004加筋板静力分析课件Step 3: Define Element Properties Create the beam cross section.a. Enter ibeam as the Section Set Name.b. Click on Ibeam button.c. Input H,W1,W2,t,t1,t2 as 2, 1, 1, 0.1, 0.1, 0.1d. Click on Calculate/Display, then you will see the sectio

20、n diagram on the next page.e. Click OK.f.Select element 21:35 for the Application Region. (Pick the element icon)g. Click Add.h. Click Apply.abcdefghWS5-21NAS101, Workshop 5, February 2004加筋板静力分析课件Step 3: Define Element PropertiesWS5-22NAS101, Workshop 5, February 2004加筋板静力分析课件Step 4: Apply Loads an

21、d Boundary Conditions Create the boundary condition for the model.a. Loads/BCs: Create / Displacement / Nodal.b. Enter translations as the New Set Name.c. Click on the Input Data.d. Enter for the Translation field.e. Click OK.f.Click on Select Application Region.g. Select FEM as the geometry filter.

22、h. Select Node 1,6,31,36 for the Application Region.These are the four corner nodes in the model.i.Click Add.j.Click OK.k. Click Apply.abcdefghijkWS5-23NAS101, Workshop 5, February 2004加筋板静力分析课件Step 4: Apply Loads and Boundary Conditions After you have completed previous steps, then you should see t

23、he constraints on the model as shown below:WS5-24NAS101, Workshop 5, February 2004加筋板静力分析课件Step 4: Apply Loads and Boundary Conditions Apply pressure load to the model.a. Loads/BCs: Create / Pressure / Element Uniform.b. Enter pressure as the New Set Name.c. Click on the Input Data button.d. Enter 0

24、.5 in the Top Surf Pressure box.e. Click OK.f.Click on Select Application Region button.g. Select FEM as the Geometry Filter.h. Select Element 1:20 for the Application Region.i.Click Add.j.Click OK.k. Click Apply.abcdefghikjWS5-25NAS101, Workshop 5, February 2004加筋板静力分析课件Step 4: Apply Loads and Boun

25、dary ConditionsYou can see the pressure load value of 0.5 is imposed on top of the plate.WS5-26NAS101, Workshop 5, February 2004加筋板静力分析课件Step 5: Analyze the Model Submit the model for analysis.a. Analysis: Analyze / Entire Model / Full Run.b. Click on the Solution Type.c. Select LINEAR STATIC as the Solution Type.d. Click OK.e. Click Apply.abcdeWS5-27NAS101, Workshop 5, February 2004加筋板静力分析课件Step 8. Analysis: Access Results / Attach XDB/ Result Entities Attach the XDB result file.a. Analysis: Access R