WS16-1 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation WORKSHOP 16 STIFFENED PLATE

WS16-2 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation

WS16-3 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Workshop Objectives l Practice modeling a stiffened plate.

WS16-4 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description l A thin plate is reinforced with two types of stiffeners. l The outer edges of the plate are reinforced with I-beam stiffeners. l The interior of the plate is reinforced with three hat stiffeners. l The structure is simply supported at two edges. l A uniform pressure of 5 psi is applied to the surface of the plate TYP 20.0

WS16-5 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description (cont.) l The plate and stiffeners are constructed from aluminum alloy T73 with the following properties: l E = 10 x 10 6 psi = 0.3 l The plate is in thick.

WS16-6 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description (cont.) l The I-beam stiffener has the following cross section: TYP

WS16-7 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Problem Description (cont.) l The rolled hat stiffener has the following cross section: BB A A Cross-Sectional Area in 2 I AA in 4 I BB in 4 J in 4

WS16-8 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation l Suggested Exercise Steps 1. Create surface geometric representing the plate. 2. Mesh the geometry to create plate (CQUAD4) and bar (CBAR) elements. 3. Define material (MAT1) and element properties (PSHELL and PBAR). 4. Verify the Y-element axis and offset vectors for the bar elements. 5. Define simply-supported boundary constraints (SPC1) and apply a uniform pressure load to the plate (PLOAD4). 6. Submit the model to MSC.Nastran for a linear static analysis. 7. Post process the results.

WS16-9 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation CREATE NEW DATABASE Create a new database called stiffened_plate.db. a.File / New. b.Enter stiffened_plate 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 c d e f g

WS16-10 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 1. Geometry: Create / Surface / XYZ Create the surface. a.Geometry: Create / Surface / XYZ. b.Enter for the Vector Coordinate List. c.Click Apply. a b c

WS16-11 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 1. Geometry: Create / Curve / XYZ Turn on the Show Parametric Direction feature. a.Display / Geometry... b.Check the Show Parametric Direction box. c.Click Apply. d.Click Cancel. b c d a

WS16-12 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 1. Geometry: Edit / Surface / Break Break the surface in the u-direction. a.Geometry: Edit / Surface / Break. b.Change the Option to Parametric. c.Choose Constant u Direction as the Break Direction. d.Enter 0.5 as the Break Curve value. e.Screen pick the surface created earlier. f.Answer Yes when the question Do you wish to delete the original surfaces? appears. a b c d e e

WS16-13 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 1. Geometry: Edit / Surface / Break Break the surfaces again in the u-direction. a.Screen pick the bottom surface. b.Answer Yes when the question Do you wish to delete the original surfaces? appears. c.Screen pick the top surface. d.Answer Yes when the question Do you wish to delete the original surfaces? appears. e.Click on the Show labels icon. e c a

WS16-14 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Finite Elements: Create / Mesh / Surface Generate plate elements using IsoMesh. a.Elements: Create / Mesh / Surface. b.Select Quad as the Element Shape. c.Select IsoMesh as the Mesher. d.Select Quad4 Element Topology. e.Select all the surfaces. f.Enter 2.0 as the Global Edge Length. g.Click Apply. h.Click on Hide labels icon. a h b c g d e f

WS16-15 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Finite Elements: Create / Mesh / Curve Generate bar elements along the longitudinal edges of the surfaces. a.Elements: Create / Mesh / Curve. b.Choose Bar2 as the element Topology. c.Select 5 horizontal surface edges. d.Click Apply. a b c d

WS16-16 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 2. Finite Element: Equivalence / All / Tolerance Cube Equivalence the model nodes to connect elements along surface edges. a.Elements: Equivalence / All / Tolerance Cube. b.Click Apply. a b

WS16-17 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Material: Create / Isotropic / Manual Input Define a material for the model. a.Material: Create / Isotropic / Manual Input. b.Type in alum for the Material Name. c.Click on the Input Properties button to bring up the Input Options window. d.Enter 10E6 for the Elastic Modulus and 0.3 for Poisson Ratio. e.Enter for the Density. f.Click OK to return to the main material menu. g.Click Apply. d e f a b g c

WS16-18 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Element Properties: Create / 2D / Shell Create element properties for the plate elements. a.Properties: Create / 2D / Shell. b.Enter plate as the Property Set Name. c.Click on the Input Properties button. d.Click on the Matl Prop Name icon. e.Click on the alum in the Select Existing Material window. f.Enter 0.1 as the thickness. g.Click OK. h.Select all surfaces for the Application Region. i.Click Add. j.Click Apply. d f e g a b c h i j

WS16-19 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Element Properties: Create / 1D / Beam Create element properties for the hat stiffeners. a.Properties: Create / 1D / Beam. b.Enter hat_stiffener as the Property Set Name. c.Click on the Input Properties button. d.Click on the Matl Prop Name icon. e.Click on alum in the Select Existing Material window. f.Enter for the Bar Orientation. g.Enter for the offset at Node 1 and Node 2. d f e g a b c

WS16-20 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation a Step 3. Element Properties: Create / 1D / Beam a.Scroll down the properties window to enter the following section properties: Area = Inertia 1,1 = Inertia 2,2 = Torsion Constant = b.Scroll further down to enter stress recovery point coordinates as shown to the right. c.Click OK. b c

WS16-21 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Element Properties: Create / 1D / Beam a.Click on Select Members, then click on the beam element filter. b.For the application region select three rows of bar elements. c.Click Add. d.Click Apply. a c d a

WS16-22 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Element Properties: Create / 1D / Beam Next, create element properties for the I-beam stiffeners. a.Properties: Create / 1D / Beam. b.Enter i_stiffener as the Property Set Name. c.Click on the Input Properties button. d.Click on the Matl Prop Name icon. e.Click on alum in Select Existing Material window. f.Enter for Bar Orientation. g.Enter for the Offset at both nodes. h.Click on Beam Library icon. d f g e h a b c

WS16-23 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Element Properties: Create / 1D / Beam a.Enter i_section for New Section Name. b.Select the I-Beam shape option. c.Enter dimensions for the I- Beam as shown. d.Click on Calculate/Display to view the cross section. e.Click OK. f.Click OK again. g.Select the curve or edge filter. h.For the application region, select the top and bottom edges of the plate. i.Click Add. j.Click Apply. a b c d e g h i j

WS16-24 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 3. Viewing / Angles … Change the viewing angle. a.Viewing/ Angles... b.Select Model Absolute. c.Input as the Angles. d.Click Apply. e.Click Cancel b c d e a

WS16-25 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Display / Load/BC/Elem Props… Change the display settings to show beam offset. a.Display / Load/BC/Elem Props... b.Change Beam Display from 1D line to 1D line + offsets c.Click Apply. d.Change Beam Display to 2D Mid- Span + Offsets e.Click Apply. f.Change Beam Display to 3D Full- Span + Offsets. g.Change Beam Display to 3D Full- Span + Offsets + Equivalent I. h.Click Apply. i.Click Cancel. b c d f i g a

WS16-26 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Display / Load/BC/Elem Props… 1D + Offsets 2D + Offsets 3D + Offsets 1D 3D + Offsets + Equivalent I

WS16-27 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Element Properties: Show Verify the orientation of the hat sections by plotting the element y axis. a.Properties: Show b.Select Bar Orientation in the properties window. c.Select the default_group. d.Click Apply. a b c d

WS16-28 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 4. Display / Load/BC/Elem Props… Change the display of loads, boundary conditions, and element properties from geometry to finite elements. a.Display / Load/BC/Elem Props... b.Check the Show on FEM only box. c.Click Apply. d.Click Cancel. e.Repeat steps from previous page to plot the element y axis for the stiffeners. b c d a

WS16-29 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 5. Loads/BCs: Create / Displacement / Nodal Create the boundary condition for the model. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Simple_Support as the New Set Name. c.Click on the Input Data button. d.Enter for the Translations. e.Click OK. f.Click on Select Application Region. g.Select Geometry as the geometry filter. h.Set the picking filter to Curve or Edge. i.Select the left and right edges of the plate. j.Click Add. k.Click OK. l.Click Apply. d e g h i j k a b c f l

WS16-30 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 5. Loads/BCs: Create / Displacement / Nodal Stiffened plate with two edges constrained.

WS16-31 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 5. Loads/BCs: Create / Pressure / Element Uniform Apply pressure to the model. a.Loads/BCs: Create / Pressure / Element Uniform. b.Enter pressure as the New Set Name. c.Select 2D as the Target Element Type. d.Click on the Input Data button. e.Enter 5 in the Top Surf Pressure field. f.Click OK. g.Click on Select Application Region button. h.Select Geometry as the Geometry Filter. i.Set the picking filter to Surface. j.Select all the surfaces for the Application Region. k.Click Add, and OK. l.Click Apply. e f h i j k a b c d g l

WS16-32 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 5. Loads/BCs: Create / Pressure / Element Uniform Stiffened plate model with applied pressure.

WS16-33 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 6. Analysis: Analyze / Entire Model / Full Run 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. a b c d e

WS16-34 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 7. Analysis: Attach XDB / Result Entities / Local After the job is completed, attach the XDB result file. a.Access Results / Attach XDB / Result Entities. b.Click on Select Result File. c.Select the file called stiffened_plate.xdb. d.Click OK. e.Click Apply. a c d e b

WS16-35 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 7. Results: Create / Quick Plot Plot plate stress and deformation results. a.Results: Create / Quick Plot. b.Select the Default result case. c.Select Stress Tensor for the Fringe Result. d.Select Displacement, Translational for the Deformation Result. e.Click Apply. a b c d e

WS16-36 NAS120, Workshop 16, May 2006 Copyright 2005 MSC.Software Corporation Step 7. Results: Create / Quick Plot Plot bar stress results. a.Select Bar Stresses, Maximum Combined for the Fringe Result. b.Click Apply. c.Plot the remaining bar stress components one at at time. a b c