Workshop 5-1 NAS101 Workshops Copyright 2001 MSC.Software Corporation WORKSHOP 5 Stiffened Plate Subjected to Pressure Load

Workshop 5-2 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 1. Stiffened Plate Model 2.GOAL: model a stiffened panel using plate elements for the panel and BEAM elements for the stiffener

Workshop 5-3 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.) 1. Stiffened Plate Model 2. We will model a plate which is.1 inches thick, 20.0 inches long, and 10.0 inches wide. The stiffener is shown below, along with the plate dimensions and loading 3. The model has pinned supports at the corners

Workshop 5-4 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.) 1. Stiffened Plate Model 2. Material properties: a.E = 10.3E+6 psi b.Poissons Ratio =.3 c.Density =.101 lb/in 3 (weight density) 3. The stiffener will be modeled using a BEAM with a PBEAML to define the cross-section 4. The 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 5-5 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.) 1. Stiffened Plate Model 2. The Model

Workshop 5-6 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.) 1. Stiffened Plate Model 2. PBEAML Entry PBEAML,2,1,,I,2.,1.,1.,.1,.1,.1 1. Sample CBEAM CBEAM

Workshop 5-7 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.) 1. Stiffened Plate Model - Pressure Load Definition 2. Pressure loads on plate and shell elements are defined using PLOAD2 or PLOAD4 entries 3. SID = Static Loading Set ID 4. EIDi = Element ID 5. P = Pressure (applied in element coordinate system) PLOAD2,1,-.5,1,THRU,20

Workshop 5-8 NAS101 Workshops Copyright 2001 MSC.Software Corporation Workshop 5 (cont.)

Workshop 5-9 NAS101 Workshops Copyright 2001 MSC.Software Corporation n Suggested Exercise Steps: 1. Create a finite element model of the plate made of CQUAD4 elements.The stiffener is made of BEAM element. 2. Define material properties. (MAT1) 3. Define element properties and sectional properties using the BEAM library. Apply loads and boundary conditions to the model. 4. Submit the model to MSC.Nastran for analysis. 5. Post-Process results using MSC.Patran.

Workshop 5-10 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create the first surface a.Create / Surface / XYZ. b.Enter for the Vector Coordinate List. c.Use [0 0 0] as the Origin Coordinate List. d.Click Apply. Step 1. Create Geometry: Create/Surface/XYZ

Workshop 5-11 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create the second surface a.Create / Surface / XYZ. b.Enter for the Vector Coordinate List. c.Select the point option on the right for the origin Coordinate List and pick point 2 as the origin. d.Click Apply. Step 1A. Create Geometry: Create/Surface/XYZ

Workshop 5-12 NAS101 Workshops Copyright 2001 MSC.Software Corporation Create mesh seeds that will be used to guide the mesh. a.Create / Mesh Seed / Uniform. b.For the Number of Elements, input 5. c.Select Surface 1.2 as the Curve List. d.Click Apply. Step 2. Finite Element: Create /Mesh Seed/Uniform Surface 1.2 Surface 1.1 Surface 2.1

Workshop 5-13 NAS101 Workshops Copyright 2001 MSC.Software Corporation Repeat the previous procedures to create 2 more sets of mesh seeds Create / Mesh Seed / Uniform. a.Input 2 use the Number of Elements. b.Select Surface 1.1 and Surface 2.1 as the Curve List. c.Click Apply. Step 2A. Finite Element: Create /Mesh Seed/Uniform

Workshop 5-14 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2B. Finite Element: Create /Mesh/Surface Create surface mesh based on the mesh seeds assigned in the previous steps. a.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.

Workshop 5-15 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2C. Finite Element: Create /Mesh/Curve Create surface mesh based on the mesh seeds assigned in the previous steps. a.Create / Mesh / Curve. b.Select Bar2 as the Element Shape. c.Enter the curves by selecting the curves off the screen Surface for Curve List. d.Click Apply.

Workshop 5-16 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 2D. Finite Element: Equivalence /All/Tolerance Cube Merge all the coincident nodes by using Equivalence function. a.Equivalence / All / Tolerance Cube. b.Click Apply. a b

Workshop 5-17 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 3. Material: Create /Isotropic/ Manual Input Create the material aluminum. a.Create / Isotropic / Manual Input. b.Type in alum for the Material Name. c.Click on the Input Properties button to bring up the Input Option window. d.Enter 10.3E6 for the Elastic Modulus, and 0.3 for Poisson Ratio,and for the density. e.Click OK to return to the main material menu. f.Click Apply.

Workshop 5-18 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4. Element Properties: Create /2D/ Shell Create the element properties. a.Create / 2D / Shell. b.Enter plate as the Property Set Name. c.Click on the Input Properties button. d.Click on the alum in the Material field on the bottom section of the Input Properties window. e.Enter 0.1 as the thickness for the plate. f.Click OK. g.Select element 1:20 for the Application Region.(pick the element icon) h.Click Add. i.Click Apply.

Workshop 5-19 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4A. Element Properties: Create /1D/ Beam Create the element properties. a.Create / 1D / Beam. b.Enter beam as the Property Set Name. c.Toggle the button from 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 field on the bottom section of the Input Properties window. f.Under the section name we would select ibeam. On the next slide I will show you how to use the beam library. g.Click OK. h.Select element 21:35 for the Application Region.(pick the element icon) i.Click Add. j.Click Apply.

Workshop 5-20 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 4B. Beam library: Create /Standard Shape/NASTRAN standard Create the beam cross sectional using IBEAM. a.Enter ibeam as the Section Set Name. b.Click on Ibeam button. c.Input H,W1,W2,t,t1,t2 as d.2,1,1,0.1,0.1,0.1 e.Click on Calculate/Display, then you will see the following section diagram on the next page f.Click OK

Workshop 5-21 NAS101 Workshops Copyright 2001 MSC.Software Corporation STEP 4C: Display the Beam cross sectional area

Workshop 5-22 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5. Loads/BCs: Create/ Displacement/Nodal Create the boundary condition for the model. a.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.. 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.

Workshop 5-23 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 5A.(cont.) Loads/BCs: Create Boundary Conditions After you have completed previous steps,then you see the constraints on the model as shown below:

Workshop 5-24 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6. Loads/BCs: Create/Pressure /Element Uniform Apply pressure load to the model. a.Create / Pressure / Element Uniform b.Enter pressure as the New Set Name. c.Click on the Input Data button. d.Enter 0.5 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, and OK. j.Click Apply.

Workshop 5-25 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 6(cont.) Loads/BCs: Create Pressure Load You can see the pressure load value of 0.5 is imposed on top of the plate.

Workshop 5-26 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 7. Analysis: Analyze/ Entire Model/Full Run Submit the model for analysis. a.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.

Workshop 5-27 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8. Analysis: Attach XDB/ Result Entities/ Local Attach the XDB result file. a.Attach XDB / Result Entities / Local. b.Click on Select Result File. c.Select the file called w5. xdb d.Click OK. e.Click Apply.

Workshop 5-28 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 8 (cont.) Results: Create/Quick Plot Create a Quick Plot of the results. a.Create / Quick Plot. b.Select SC1 result case. c.Select Displacement, Translational for the Deformation Result. d.Click Apply. Note: Maximum Deformation is 6.64E-2. These information appear at the lower right hand corner of the plot.

Workshop 5-29 NAS101 Workshops Copyright 2001 MSC.Software Corporation Step 9 (cont.) Fringe Results: Create/Quick Plot Create a Quick Plot of the results. a.Create / Quick Plot. b.Select SC1 result case. c.Select Stress Tensor for the Fringe Result d.Select Displacement, Translational for the Deformation Result. e.Click Apply. Note: Maximum Stress value is 2.92E+3