加筋板静力分析.ppt

WORKSHOP 5Stiffened Plate Subjected to Pressure Load,Workshop 5,Stiffened Plate ModelGOAL:model a stiffened panel using plate elements for the panel and BEAM elements for the stiffener,Workshop 5(cont.),Stiffened Plate ModelWe 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 loadingThe model has pinned supports at the corners,Workshop 5(cont.),Stiffened Plate ModelMaterial properties:E=10.3E+6 psiPoissons Ratio=.3Density=.101 lb/in3(weight density)The stiffener will be modeled using a BEAM with a PBEAML to define the cross-sectionThe GRID points will lie at the mid-plane of the plate,so the BEAM must be offset from the GRID points by 1.05(half the BEAM height pus half the plate thickness),Workshop 5(cont.),Stiffened Plate Model,Workshop 5(cont.),Stiffened Plate ModelPBEAML EntryPBEAML,2,1,I,2.,1.,1.,.1,.1,.1Sample CBEAMCBEAM 21 2 31 32 0.0.1.0.0.1.05 0.0.1.05,Workshop 5(cont.),Stiffened Plate Model-Pressure Load DefinitionPressure loads on plate and shell elements are defined using PLOAD2 or PLOAD4 entriesSID=Static Loading Set IDEIDi=Element IDP=Pressure(applied in element coordinate system)PLOAD2,1,-.5,1,THRU,20,Workshop 5(cont.),Suggested Exercise Steps:Create a finite element model of the plate made of CQUAD4 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.,Create the first surfaceGeometry:Create/Surface/XYZ.Enter for the Vector Coordinate List.Use 0 0 0 as the Origin Coordinate List.Click Apply.,Step 1:Create Finite Element Model,a,b,c,d,Create the second surfaceGeometry: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 Model,a,b,c,Create mesh seeds that will be used to guide the mesh.Elements:Create/Mesh Seed/Uniform.For the Number of Elements,input 5.Select Surface 1.2 as the Curve List.,Step 1:Create Finite Element Model,Surface 1.2,Surface 1.1,Surface 2.1,a,b,c,Repeat the previous procedures to create 2 more sets of mesh seeds.Input 2 use the Number of Elements.Select Surface 1.1 as the Curve List.Select Surface 2.1 as the Curve List.,Step 1:Create Finite Element Model,a,b,c,Step 1:Create Finite Element Model,Create surface mesh based on the mesh seeds assigned in the previous steps.Elements:Create/Mesh/Surface.Select Quad as the Elem Shape.Select IsoMesh as the Mesher.Enter Surface 1 2 for Surface List.Click Apply.,a,b,c,d,e,Step 1:Create Finite Element Model,Create a curve mesh for the plate stiffeners.Elements:Create/Mesh/Curve.Select Bar2 as the Element Shape.Enter the curves by selecting the curves off the screen Surface 1.4 1.2 2.2 for Curve List.Click Apply.,a,b,c,d,Step 1:Create Finite Element Model,Merge all the coincident nodes by using Equivalence function.Elements:Equivalence/All/Tolerance Cube.Click Apply.,a,b,Step 2:Define Material Properties,Create the material aluminum.Materials:Create/Isotropic/Manual Input.Type in alum for the Material Name.Click on the Input Properties button to bring up the Input Option window.Enter 10.3E6 for the Elastic Modulus,and 0.3 for Poisson Ratio,and 0.101 for the density.Click OK to return to the main material menu.Click Apply.,a,b,c,d,e,f,Step 3:Define Element Properties,Create the element properties.Properties:Create/2D/Shell.Enter plate as the Property Set Name.Click on the Input Properties button.Click on alum in the window that appears when you click the Select Material Icon.Enter 0.1 as the thickness for the plate.Click OK.Select element 1:20 for the Application Region.(pick the element icon)Click Add.Click Apply.,a,b,c,e,f,g,h,i,d,Step 3:Define Element Properties,Create the element properties.Properties:Create/1D/Beam.Enter beam as the Property Set Name.Toggle the option from General section to Tapered Section.General section in NASTRAN means the CBAR element whereas Tapered section means CBEAM element.Click on the Input Properties button.Click on the alum in the Material Prop Name box.Enter the Bar Orientation and Offsets as shown.Click on the Beam Library Icon.,a,b,c,d,e,f,g,Step 3:Define Element Properties,Create the beam cross section.Enter ibeam as the Section Set Name.Click on Ibeam button.Input H,W1,W2,t,t1,t2 as 2,1,1,0.1,0.1,0.1Click on Calculate/Display,then you will see the section diagram on the next page.Click OK.Select element 21:35 for the Application Region.(Pick the element icon)Click Add.Click Apply.,a,b,c,d,e,f,g,h,Step 3:Define Element Properties,Step 4:Apply Loads and Boundary Conditions,Create the boundary condition for the model.Loads/BCs:Create/Displacement/Nodal.Enter translations as the New Set Name.Click on the Input Data.Enter for the Translation field.Click OK.Click on Select Application Region.Select FEM as the geometry filter.Select Node 1,6,31,36 for the Application Region.These are the four corner nodes in the model.Click Add.Click OK.Click Apply.,a,b,c,d,e,f,g,h,i,j,k,Step 4:Apply Loads and Boundary Conditions,Step 4:Apply Loads and Boundary Conditions,Apply pressure load to the model.Loads/BCs:Create/Pressure/Element Uniform.Enter pressure as the New Set Name.Click on the Input Data button.Enter 0.5 in the Top Surf Pressure box.Click OK.Click on Select Application Region button.Select FEM as the Geometry Filter.Select Element 1:20 for the Application Region.Click Add.Click OK.Click Apply.,a,b,c,d,e,f,g,h,i,k,j,Step 4:Apply Loads and Boundary Conditions,Step 5:Analyze the Model,Submit the model for analysis.Analysis:Analyze/Entire Model/Full Run.Click on the Solution Type.Select LINEAR STATIC as the Solution Type.Click OK.Click Apply.,a,b,c,d,e,Step 8.Analysis:Access Results/Attach XDB/Result Entities,Attach the XDB result file.Analysis:Access Results/Attach XDB/Result Entities.Click on Select Result File.Select the file called w5.xdbClick OK.Click Apply.,a,b,c,d,e,Step 8(cont.)Results:Create/Quick Plot,Create a Quick Plot of the results.Results:Create/Quick Plot.Select SC1 result case.Select Displacement,Translational for the Deformation Result.Click Apply.,a,b,c,Step 9(cont.)Fringe Results:Create/Quick Plot,Create a Quick Plot of the results.Results:Create/Quick Plot.Select SC1 result case.Select Stress Tensor for the Fringe ResultSelect Displacement,Translational for the Deformation Result.Click Apply.,