WORKSHOP 3 FLAT PLATE USING MSC.LAMINATE MODELER WS3-1 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS3-2 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS3-3 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Problem Description Model a 1x1 meter plate. Use millimeters as units of length. The plate is 4 mm thick and is a laminate made up of 16 plies with equal thickness. The laminate is uniform. The plies have two orientations, 0 and 90 degrees, i.e. parallel to the plate edges. The material properties of the lamina are E-modulus: E 11 = 181 GPa, E 22 = 10.3 GPa Shear modulus: G 12 = 7.17 GPa, G 23 = 5.00 GPa, G 13 = 7.17 GPa Poisson Ratio: 0.28 Density: 1.6E-9 The plate is fixed along one edge, and supported laterally at one of the two opposite corners. The plate is loaded with a uniform pressure of 0.1 KPa, giving a total force acting on the plate of 100 Newtons. We want to investigate the occurring stresses in the layers and the maximum deflection of the plate.

Mar120, Workshop 10, March 2001 WS3-4 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Suggested Exercise Steps 1. Create a new database 2. Create the model surface 3. Mesh the surface to create the model elements 4. Constrain an edge and an opposite point 5. Create pressure loading for the plate 6. Create 2D orthotropic material for lamina 7. Modify 2D orthotropic material to include failure model 8. Create laminate modeler material 9. Create laminate modeler plies 10. Create laminate modeler layup of plies 11. Analyze the model using MSC.Nastran 12. Access results.XDB File and look at results 13. Create laminate modeler failure results 14. Look at LM failure results using MSC.Patran

Mar120, Workshop 10, March 2001 WS3-5 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation d e f b c Open a new database. Name it Flatplate.db. a.File / New. b.Enter Flatplate_2 as the file name. c.Click OK. d.Select MSC.Nastran as the Analysis Code. e.Select Structural as the Analysis Type. f.Click OK. a Step 1. Create a New Database

Mar120, Workshop 10, March 2001 WS3-6 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Create the flatplate geometry. a.Geometry: Create / Surface / XYZ b.Enter as the Vector Coordinates List. c.Enter [0 0 0] as the Origin Coordinates List. d.Click –Apply-. e.Click Iso 3 View. Step 2. Create the Model Surface e b c d a

Mar120, Workshop 10, March 2001 WS3-7 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 3. Mesh the Surface to Create the Model Elements Create a mesh for the model. a.Elements: Create / Mesh / Surface. b.Select IsoMesh as the Mesher. c.Select Quad4 as the Topology. d.Uncheck the Automatic Calculation. e.Enter 125 as the Global Edge Length Value. f.Select Surface 1 for the Surface List. g.Click –Apply-. d e c b a f g

Mar120, Workshop 10, March 2001 WS3-8 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 4. Constrain an Edge and an Opposite Point Define constraints. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Fixed Edge as the New Set Name. c.Click Input Data. d.Enter as the Translations. e.Click OK. f.Click Select Application Region. g.Select Edge Icon. h.Select Surface 1.4 for Select Geometry Entities. i.Click Add. j.Click OK k.Click –Apply-. d e g h i j b c a f k

Mar120, Workshop 10, March 2001 WS3-9 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Define constraints. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Supported Point as the New Set Name. c.Click Input Data. d.Enter as the Translations. e.Click OK. f.Click Select Application Region. g.Select Point Icon. h.Select Point 2 for Select Geometry Entities. i.Click Add. j.Click OK k.Click –Apply-. b c d e a f g h i j k Step 4. Constrain an Edge and an Opposite Point (Cont.)

Mar120, Workshop 10, March 2001 WS3-10 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Define Loading. a.Loads/BCs: Create / Pressure / Element Uniform. b.Enter Pressure Load as the New Set Name. c.Select 2D as Target Element Type d.Click Input Data. e.Enter as the Top Surf Pressure. f.Click OK. g.Click Select Application Region. h.Select Surface Icon. i.Select Surface 1 for Select Surface or Edges. j.Click Add. k.Click OK l.Click –Apply-. Step 5. Create Pressure Loading for the Plate b d e f a g h i j k l c

Mar120, Workshop 10, March 2001 WS3-11 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Note that the pressure is in MegaPascals. Until now this exercise has been quite straight forward, but the next step is to define the laminate. The model should look like this after clicking –Apply-. Step 5. Create Pressure Loading for the Plate (Cont.)

Mar120, Workshop 10, March 2001 WS3-12 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 6. Create 2D Orthotropic Material for Lamina Define lamina material properties. a.Materials: Create / 2D Orthotropic / Manual Input. b.Enter ud_t300_n5208 as the Material Name. c.Click Input Properties. d.Select Linear Elastic as the Constitutive Model. e.Enter as the Elastic Modulus 11. f.Enter as the Elastic Modulus 22. g.Enter 0.28 as the Poisson Ratio 12. h.Enter 7170 as the Shear Modulus 12. i.Enter 5000 as the Shear Modulus 23. j.Enter 7170 as the Shear Modulus 13. k.Enter 1.6E-9 as the Density. l.Click OK. m.Click Apply. b c d e a f g h i j k l m These material properties will be used later for other workshops. Thus, a session file, material.ses, is provided with the workshop files. This can be played into MSC.Patran creating the properties quickly and easily.

Mar120, Workshop 10, March 2001 WS3-13 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Define constitutive failure model. a.Materials: Modify / 2D Orthotropic. b.Select ud_t300_n5208 as the Existing Materials. c.Click Input Properties. d.Select Failure as the Constitutive Model. e.Select Tsai-Wu as the Composite Failure Theory. f.Enter 1500 as the Tension Stress Limit 11. g.Enter 40 as the Tension Stress Limit 22. h.Enter 1500 as the Compress Stress Limit 11. i.Enter 246 as the Compress Stress Limit 22. j.Enter 68 as the Shear Stress Limit. k.Enter –3.36e-6 as the Interaction Term.. l.Enter 50 as the Bonding Shear Stress Limit. m.Click OK. n.Click Apply. d e f g h i j k l m a b c n Step 7. Modify 2D Orthotropic Material to Include Failure Model

Mar120, Workshop 10, March 2001 WS3-14 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 8. Create Laminate Modeler Material Now it is finally time to enter the Laminate Modeler. a.Tools: Laminate Modeler / Layup/Laminate. b.Click New Layup File… c.Enter Flatplate_LM as the File Name. d.Click OK. e.Create / LM_Material / Add. f.Select ud_t300_n5208 from the Analysis Material. g.Enter 0.25 as the Thickness. h.Click –Apply-. Now have made a Laminate Modeler material. More about this later. a b cd e f g h

Mar120, Workshop 10, March 2001 WS3-15 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Create the plies. a.Laminate Modeler: Create / LM_Ply / Add. b.Select Mat_1 from the Select LM_Material list. c.Select Surface 1 as the Select Area. d.Click anywhere on the surface for Start Point. e.Enter Coord 0.1 for the Reference Direction. f.Click –Apply-. g.Enter 90 for the Reference Angle. h.Click –Apply-. The first ply has been created. The second ply has been created. b a c d e f g h Step 9. Create Laminate Modeler Plies

Mar120, Workshop 10, March 2001 WS3-16 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 10. Create Laminate Modeler Layup of Plies Create the Layup. a.Laminate Modeler: Create / LM_Layup / Add. b.Click Layup Definition… c.Select Ply_2 then Ply_1 four times, thus creating 8 plies in the layup. d.Click on the Upper Left Icon to mirror the 8 plies to create a total of 16 plies in the layup. e.Click OK. f.Click –Apply-. g.Click Yes. c d e a b f g

Mar120, Workshop 10, March 2001 WS3-17 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 11. Analyze the Model Using MSC.Nastran Set up and run the analysis. a.Analysis: Analyze / Entire Model / Full Run b.Click Subcases. c.Select Default as an Available Subcases. d.Click Output Request. b c a d

Mar120, Workshop 10, March 2001 WS3-18 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation a.Select Advanced as the Form Type. b.Select Element Stresses as the Select Result Type. c.Select Ply Stresses as the Composite Plate Opt. d.Click OK. a b c d Step 11. Analyze the Model Using MSC.Nastran (Cont.) b

Mar120, Workshop 10, March 2001 WS3-19 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation a.Click Apply in the Subcase Menu. b.Click Cancel. c.Click Apply in the Analysis Menu. a b c Step 11. Analyze the Model Using MSC.Nastran (Cont.)

Mar120, Workshop 10, March 2001 WS3-20 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 12. Access Results.XDB File and Look at Results Create a link to the MSC.Nastran analysis results file a.Analysis: Access Results / Attach XDB / Result Entities. b.Click Select Results Files. c.Select Flatplate.xdb. d.Click OK. e.Click Apply. b c d e a Look at the results. Notice that the maximum displacement is still 164 mm.

Mar120, Workshop 10, March 2001 WS3-21 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation For non-layered shell elements, postprosess either top or bottom stresses: Z1 (Top) Z2 (Bottom) For composite shell elements postprosess stresses for each layer. These stresses are output at the center (in the thickness direction) of each layer: If there are thick layers the extreme stress value may be significantly larger than the value reported. If it is desired to have top and bottom stresses for certain layers, one way to get this is to add very thin layers over and under them. For these layers the middle stress can be used as a top/bottom stress for the structural layers. Comments Layer 1 Layer 2 Layer 3

Mar120, Workshop 10, March 2001 WS3-22 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 13. Create Laminate Modeler Failure Results Do a failure calculation in LM. a.Laminate Modeler: Create / Results / Failure Calc. b.Select SC1: DEFAULT, A1: Static Subcase for the Select Result Cases. c.Select Stress Tensor for the Select Layered Result. d.Select All the Elements for the Select Area. e.Select Tsai-Wu as the Criterion. f.Click Material Allowables... g.Click OK. h.Enter Failure as the Create Result Name. i.Uncheck Margin of Safety, Critical Component and Critical Ply. j.Click –Apply-. These are retrieved from Patran by Laminate Modeler. a b c d e f g h i j

Mar120, Workshop 10, March 2001 WS3-23 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Step 14. Look at LM Failure Results Using MSC.Patran View the LM derived results. a.Results: Create / Quick Plot. b.Select SC1: DEFAULT, Static Subcase for Selected Result Cases. c.Select LM_Fail_Ind, Failure, Tsai-Wu for the Select Fringe Result. d.Click Apply. Note that the failure Index is equal to the earlier value, a b c d

Mar120, Workshop 10, March 2001 WS3-24 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Comments The two approaches give the same results both in terms of stresses, deflections and failure indices. Look at the position of the maximum failure index for Tsai-Wu. Is it the same position as the minimum margin of safety? Is the failure index plot an easy way of understanding component strength? The different failure criteria give: The failure indices are greatly different between Tsai-Wu, Hill and Maximum. Hence if quoting failure indices it is necessary to specify the failure theory used. Max FIMin Margin Tsai-Wu Hill Maximum Hoffman Hankinson Cowin

Mar120, Workshop 10, March 2001 WS3-25 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation Differences In this exercise, Failure Index is done by Laminate Modeler on the fly, the static analysis does not need to be re-run The user can select any subset of the model to perform Failure Analysis on Three more Failure Criteria models are available in Laminate Modeler: Hankinson, Cowin and User-Defined Notes Geometry, Mesh, Loads, boundary conditions are still done in MSC.Patran. The composite material and the properties are the actual product of Laminate Modeler. If you have any questions, please do not hesitate to ask!

Mar120, Workshop 10, March 2001 WS3-26 PAT325, Workshop 3, February 2004 Copyright 2004 MSC.Software Corporation