WORKSHOP 7B MODELING HONEYCOMB WITH SOLID AND SHELL ELEMENTS WS7B-1 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS7B-2 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation

Mar120, Workshop 10, March 2001 WS7B-3 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Problem Description Unlike the previous workshop that involved modeling the honeycomb structure using the MSC.Laminate Modeler, this workshop is used to show how to model the honeycomb structure using solid and shell elements. Solid hexahedral elements are to be used to represent the core, and shell elements are to used to represent the laminate backing. Similar constraints and loading are to be applied to the model. After the MSC.Nastran analysis the results are to be looked at, and perhaps compared to those for the previous laminate model.

Mar120, Workshop 10, March 2001 WS7B-4 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Suggested Exercise Steps 1. Create a new database 2. Import two surfaces from an IGES File 3. Create a solid from the two imported surfaces 4. Mesh the solid using IsoMesh 5. Mesh at surfaces of the solid using IsoMesh 6. Equivalence the solid and surface meshes 7. Cantilever one end of honeycomb model 8. Apply the force load at the free end of the model 9. Create material properties using a session file 10. Create the isotropic material for the core 11. Create a composite material using laminate in MSC.Patran 12. Create 3D element property set for core material 13. Create element property for upper lamina 14. Create element property for lower lamina 15. Analyze the model and attach the results file 16. Verify the stress tensor and displacement results

Mar120, Workshop 10, March 2001 WS7B-5 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation d e f b c Step 1. Create a New Database Create a new database. a.File / New. b.Enter 2 nd _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 WS7B-6 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 2. Import two Surfaces From an IGES File Import two surfaces from an IGES file. a.File / Import b.Select IGES from the Source. c.Select exercise7b.igs. d.Click –Apply-. e.Click OK when the IGES Import Summary appears. a b c d e

Mar120, Workshop 10, March 2001 WS7B-7 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation This is how the geometry should look like after importing the file. Step 2. Import two Surfaces From an IGES File (Cont.)

Mar120, Workshop 10, March 2001 WS7B-8 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 3. Create a Solid From the two Imported Surfaces Create a parametric solid using the two surfaces. a.Geometry: Create / Solid / Surface. b.Select 2 Surfaces as the Option. c.Uncheck the Auto Execute toggle. d.Select Surface 1 as the Starting Surface List. e.Select Surface 2 as the Ending Surface List. f.Click –Apply. a b c d e f

Mar120, Workshop 10, March 2001 WS7B-9 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 4. Mesh the Solid Using IsoMesh Mesh the geometric solid. a.Elements: Create / Mesh / Solid. b.Select Hex as the Elem Shape. c.Select IsoMesh as the Mesher. d.Select Hex8 as the Topology. e.Uncheck the Automatic Calculation. f.Enter 5.0 as the Global Edge Length Value. g.Select Solid 1 as the Solid List. h.Click –Apply-. a b c d e f g h

Mar120, Workshop 10, March 2001 WS7B-10 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 5. Mesh at Surfaces of the Solid Using IsoMesh Mesh the surfaces (at inner and outer free faces of the hex elements) with shell elements. 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 Value. g.Select Surface 1 as the Surface List. h.Click –Apply-. i.Select Surface 2 as the Surface List. j.Click –Apply-. a b c d e f g h i j Note that both surfaces could have been meshed simultaneously.

Mar120, Workshop 10, March 2001 WS7B-11 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 5. Mesh at Surfaces of the Solid Using IsoMesh (Cont.) Shell element Solid element

Mar120, Workshop 10, March 2001 WS7B-12 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 6. Equivalence the Solid and Surface Meshes Equivalence the solid and surface mesh nodes. a.Elements: Equivalence / All / Tolerance Cube. b.Click –Apply-. a b

Mar120, Workshop 10, March 2001 WS7B-13 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 7. Cantilever one end of Honeycomb Model Fixed nodes at one end using a solid face as the application region.. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Fixed_surface 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 Surface Picking Icon. i.Select Solid 1.1 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 WS7B-14 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation The nodes at solid face Solid 1.1 are constrained. Step 7. Cantilever one end of Honeycomb Model (Cont.)

Mar120, Workshop 10, March 2001 WS7B-15 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 8. Apply the Force Load at the Free end of the Model Apply loads at four points. a.Loads/BCs: Create / Force / Nodal. b.Enter Load as the New Set Name. c.Click on Input Data…. d.Enter as the Force. e.Click OK. f.Click Select Application Region… a b c d e f

Mar120, Workshop 10, March 2001 WS7B-16 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation a.Select Point Picking Icon. b.Select Point from the geometry as the Select Geometry Entities. c.Click Add. d.Click OK. a b c d Step 8. Apply the Force Load at the Free end of the Model (Cont.)

Mar120, Workshop 10, March 2001 WS7B-17 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation a.Click –Apply-. Now the model has been assigned a load of 0.5 at four different points, a total of 2. a Step 8. Apply the Force Load at the Free end of the Model (Cont.)

Mar120, Workshop 10, March 2001 WS7B-18 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 9. Create Material Properties Using a Session File Read(play) session file materials.ses. a.File / Session / Play.. b.Select materials.ses. c.Click –Apply-. a b c

Mar120, Workshop 10, March 2001 WS7B-19 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 10. Create the Isotropic Material for the Core Create a material to represent the core of the honeycomb structure. 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 WS7B-20 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 11. Create a Composite Material Using Laminate in MSC.Patran Create an inner(upper) laminate in MSC.Patran. a.Materials: Create / Composite / Laminate. b.Enter upper_ply as the Material Name. c.Click ud_t300_n5208 four times to upload to the Stacking Sequence Definition. d.Select Overwrite as the Text Entry Mode. e.Click Thicknesses. f.Enter 4(0.12) in the Overwrite Thickness. g.Click Load Text Into Spreadsheet. h.Select Overwrite as the Text Entry Mode. i.Click Orientations. j.Enter -45 / 90 / 45 / 0 in the Insert Orientations. k.Click Load Text Into Spreadsheet. l.Click –Apply-. a b c d e f g h i j k l f j

Mar120, Workshop 10, March 2001 WS7B-21 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation a.Enter lower_ply as the Material Name. b.Click on Delete Selected Rows many times so that the Stacking Sequence Definition becomes empty. c.Select ud_t300_n5208 four times as the Material. d.Select Overwrite as the Text Entry Mode. e.Click on Thicknesses. f.Enter 4(0.12) in the Overwrite Thickesses. g.Click Load Text Into Spreadsheet. h.Select Overwrite as the Text Entry Mode. i.Click Orientations. j.Enter 0 / 45 / 90 / -45 in the Overwrite Orientations. k.Click Load Text Into Spreadsheet. l.Set the Offset to –0.48 m.Click –Apply- a b c d e f g h i j k m Step 11. Create a Composite Material in MSC.Patran (Cont.) f j l

Mar120, Workshop 10, March 2001 WS7B-22 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 12. Create 3D Element Property set for Core Material Create element properties for 3D solid core. a.Properties: Create / 3D / Solid. b.Enter 3D_solid as the Property Set Name. c.Select Standard Formulation as the Options. d.Click Input Properties… e.Select Core as the Material Name from the Material Property Sets. f.Click OK. g.Select Solid 1 for the Select Members. h.Click Add. i.Click Apply. e f a b c d g h i

Mar120, Workshop 10, March 2001 WS7B-23 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 13. Create Element Property for Upper Lamina Create 2D element properties for plies above the core. a.Properties: Create / 2D / Shell b.Enter 2D_upper_shell as the Property Ser Name. c.Select Laminate and Standard Formulation as the Options. d.Click Input Properties… e.Select upper_ply as the Material Name from the Material Property Sets. f.Click OK. g.Select Surface 1 for the Select Members. h.Click Add. i.Click Apply. e f a b c d g h i

Mar120, Workshop 10, March 2001 WS7B-24 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Create 2D element properties for plies below the core. a.Properties: Create / 2D / Shell b.Enter 2D_bottom_shell as the Property Set Name. c.Select Laminate and Standard Formulation as the Options. d.Click Input Properties… e.Select lower_ply as the Material Name from the Material Property Sets. f.Click OK. g.Select Surface 2 for the Select Members. h.Click Add. i.Click Apply. e f a b c d g h i Step 14. Create Element Property for Lower Lamina

Mar120, Workshop 10, March 2001 WS7B-25 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 15. Analyze the Model and Attach the Results File Run the analysis and attach the results file. a.Analysis: Analyze / Entire Model / Full Run. b.Click Apply. c.Analysis: Access Results / Attach XDB / Result Entities. d.Click Select Results File… e.Select 2 nd _Honeycomb. f.Click OK. g.Click Apply. a b c d e f g

Mar120, Workshop 10, March 2001 WS7B-26 PAT325, Workshop 7B, February 2004 Copyright 2004 MSC.Software Corporation Step 16. Verify the Stress Tensor and Displacement Results Check the deformation and stress results. a.Results: Create / Quick Plot. b.Select SC1.DEFAULT,A1 Static Subcase from the Select Result Cases. c.Select Stress Tensor as the Select Fringe Result. d.Select Layer 1, or some other layer. e.Select Displacement, Translational as the Select Deformation Result. f.Click Apply. a b c e f d