WORKSHOP 7 MODELING HONEYCOMB USING MSC.LAMINATE MODELER WS7-1 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS7-2 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS7-3 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Problem Description This workshop is for modeling a honeycomb structure (homogeneous center with lamina backing) using the MSC.Laminate Modeler 2D capability. The core is to be represented as a lamina ply without any fiber orientation (painted draping). The backing of the core is to be represented as lamina plies with fiber orientation in either 0, 45, 90, or –45 degrees. An analysis with MSC.Nastran is to be performed, and stresses and displacements observed.

Mar120, Workshop 10, March 2001 WS7-4 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Suggested Exercise Steps 1. Create a new database 2. Import geometry from an IGES file 3. Mesh the surface using Isomesh 4. Constrain an edge of the surface 5. Create a force load on two points of the surface 6. Create 2D orthotropic materials by playing a session file 7. Create an isotropic material manually 8. Create a new layup file in MSC.Laminate Modeler 9. Create LM_Materials 10. Create LM_Plies for the lamina and core 11. Create a LM_Layup from five plies 12. Perform the analysis using MSC.Nastran 13. Attach the MSC.Nastran results.XDB file 14. View the stress tensor and displacement results

Mar120, Workshop 10, March 2001 WS7-5 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation d e f b c Step 1. Create a New Database Create a new database. Name it Honeycomb.db. a.File / New. b.Enter Honeycomb 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

Mar120, Workshop 10, March 2001 WS7-6 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 2. Import Geometry From an IGES File Import the file exercise7a.igs. a.File / Import b.Select Source: IGES. c.Select exercise7a.igs. d.Click –Apply-. e.Click OK when IGES Import Summary appears. a b c d e

Mar120, Workshop 10, March 2001 WS7-7 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 3. Mesh the Surface using Isomesh Mesh the Imported Surface a.Elements: Create / Mesh / Surface. b.Select Quad as the Elem Shape. c.Select Isomesh as the Mesher. d.Select Quad4 as the Topology. e.Uncheck the Automatic Calculation. f.Enter 5.0 as the Global Edge Length Value. g.Select Surface 1 as the Surface List. h.Click –Apply-. a b c d e f g h

Mar120, Workshop 10, March 2001 WS7-8 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 4. Constrain an Edge of the Surface Apply constraint by fixing the edge. 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.Enter as the Rotations. f.Click OK. g.Click Select Application Region…. h.Select Geometry as the Geometry Filter. i.Select Curve picking Icon. j.Select Suface 1.1 as the Select Geometry Entities. k.Click Add. l.Click Ok. m.Click –Apply-. a b c d e f g h i j k l m

Mar120, Workshop 10, March 2001 WS7-9 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation This is how the geometry should look like after fixing the edge. Step 4. Constrain an Edge of the Surface (Cont.)

Mar120, Workshop 10, March 2001 WS7-10 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 5. Create a Force Load on two points of the Surface Apply Loads to the model at points. a.Loads/BCs: Create / Force / Nodal. b.Enter Loads as the New Set Name. c.Click Input Data… d.Enter as the Force. e.Click OK. f.Click Select Application Region…. g.Select Geometry as the Geometry Filter. h.Select Point picking icon. i.Select Point 2 and 4 as the Select Geometry Entities. j.Click Add. k.Click OK. l.Click –Apply-. a b c d e f g h i j k l

Mar120, Workshop 10, March 2001 WS7-11 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation This is how the model should look after applying loads at the points Step 5. Create a Force Load on two points of the Surface (Cont.)

Mar120, Workshop 10, March 2001 WS7-12 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 6. Create 2D Orthotropic Materials by Playing a Session File Play materials.ses file. a.File / Session / Play.. b.Select materials.ses. c.Click –Apply-. a b c

Mar120, Workshop 10, March 2001 WS7-13 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 7. Create an Isotropic Material Manually Create a material and name it Core. a.Materials: Create / Isotropic / Manual Input. b.Enter Core as the Material Name. c.Click Input Properties… d.Select Linear Elastic as the Constitutive Model. e.Enter 215 as the Elastic Modulus. f.Enter 150 as the Shear Modulus. g.Click OK. h.Click Apply. a b c d e f g h

Mar120, Workshop 10, March 2001 WS7-14 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 8. Create a New Layup File in MSC.Laminate Modeler Open laminate modeler and create a new layup file. a.Tools / Laminate Modeler / Layup/Laminate. b.Click New Layup File… c.Enter Honeycomb_LM as the File Name. d.Click OK. a b c d

Mar120, Workshop 10, March 2001 WS7-15 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 9. Create LM_Materials Create LM_materials using analysis material and other inputs. a.Laminate Modeler: Create / LM_Material / Add. b.Mat_1 for LM_Material Name c.Type: Drape(Scissor) d.Select ud_t300_n5208 from the Analysis Material. e.Enter 0.12 as the Thickness. f.Click –Apply-. g.Mat_2 for LM_Material Name h.Type: Painted i.Select core from the Analysis Material. j.Enter 20 as the Thickness. k.Click –Apply-. a d e f i j k h b c g

Mar120, Workshop 10, March 2001 WS7-16 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 10. Create LM_Plies for the Lamina and Core Create LM_Plies on each side of the core to represent the laminate. a.Laminate Modeler: Create / LM_Ply / Add. b.Select Mat_1 from the Select LM_Material. c.Select Surface 1 as the Select Area. d.Pick a node at a corner of the surface as the Start Point. e.Click on Reference Direction. f.Click on Tip and base points picking icon. g.Select the two points shown in the figure. h.Enter 0 as the Reference Angle. i.Click –Apply-. j.Create three more plies, changing the Reference Angle to 45, 90 then –45 deg, while keeping all the other entries the same. a b c d e f h i g

Mar120, Workshop 10, March 2001 WS7-17 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Create a LM_Ply to represent the core material. a.Laminate Modeler: Create / LM_Ply / Add. b.Type: Painted c.Select Mat_2 from the Select LM_Material. d.Click –Apply-. a c d Step 10. Create LM_Plies for the Laminate and Core (Cont.) b

Mar120, Workshop 10, March 2001 WS7-18 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 11. Create a LM_Layup From Five Plies Create a LM_Layup to represent the 4 plies on each side of the core and the core. a.Laminate Modeler: Create / LM_Layup / Add. b.Click Layup Definition… c.Select ply_1 through ply_5, then select ply_4 through ply_1. (there should be total of 9 plies). d.Click OK. e.Click –Apply-. f.Click Yes when the message about creating properties, etc. appears. a b c d e

Mar120, Workshop 10, March 2001 WS7-19 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation This is how the model should look like after laying out the plies. The red markers represent the face- to-face thickness of the layout materials. Step 11. Create a LM_Layup (Cont.)

Mar120, Workshop 10, March 2001 WS7-20 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 12. Perform the Analysis Using MSC.Nastran Run the Analysis. a.Analysis: Analyze / Entire Model / Full Run. b.Click –Apply-. a b

Mar120, Workshop 10, March 2001 WS7-21 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 13. Attach the MSC.Nastran Results.XDB File Attach the result file (.XDB). a.Analysis: Access Results / Attach XDB / Result Entities. b.Click Select Results File… c.Select Honeycomb. d.Click OK. e.Click Apply. a b c d e

Mar120, Workshop 10, March 2001 WS7-22 PAT325, Workshop 7, February 2004 Copyright 2004 MSC.Software Corporation Step 14. View the Stress Tensor and Displacement Results Look at the results. a.Results: Create / Quick Plot. b.Select SC1.DEFAULT,A1 Static Subcase as the Select Result Cases. c.Select Stress Tensor as the Select Fringe Result. d.Select Layer 1, or some other layer. e.Select Displacements, Translational as the Select Deformation Result. f.Click Apply. The maximum value of the deformation should be with symmetrical stress variations. a b c e f d