Define a Composite Material WORKSHOP Define a Composite Material NAS121, Workshop , May 6, 2002 WS-1

Problem Description A 1 in. x 1 in. composite plate is loaded with 2000 #/in. in the Y direction on the top edge, 1000 #/in. in both the X direction and Y direction on the right hand side edge. The left side reacts the loads with X, Y, Z, and Ry constraints.

Problem Description The layup is made of graphite/epoxy tape and is shown to the right. The angles shown are relative to the global axis shown. Thus, the 0 degree ply 1 has it’s fibers coming out of the page in the Y direction. Note that while the positive sense of the angles are right hand rule around the Z global axis in this layup definition, in the Nastran definition, it is around the Z element axis and thus dependent on the element GRID order.

Problem Description (cont.) U12 .35 G12 1e6 G13 G23 Xt 120 ksi Xc 110 ksi Yt 13 ksi Yc 16 ksi S 14 ksi Sb 5 ksi Problem Description (cont.) The composite plies are graphite/epoxy tape with a thickness of 0.0054 in. The elastic and strength properties are shown on the right. The failure theorem to be used is Hill.

Suggested Exercise Steps Create a geometry model. Use mesh seeds to define the mesh density. Create a finite element mesh. Apply boundary conditions to the model. Apply loads to the model. Define ply material properties. Check element normals Define composite material properties. Define a material coordinate system Apply the material coordinate system to the elements. Submit the model to MSC.Nastran for analysis. Attach xdb Results File Display ply stresses using MSC.Patran. View ply failure indices in MSC.Nastran Change layup to make failure indices below 1.0. Analyze the model with the new composite layup View the changed ply failure indices

CREATE NEW DATABASE a d e f c g b Create a new database called composite1.db: In File select New Enter composite1 as the file name Click OK Choose Default Tolerance Select MSC.Nastran as the Analysis Code Select Structural as the Analysis Type e f b c g

Step 1. Create a geometry model In Geometry create the first curve. Select Create / Surface / Vertex On the Surface Vertex “n” Lists enter [0 0 0], [1 0 0], [1 1 0], [0 1 0] Click Apply Click the Show Label icon b c

Step 2. Use mesh seeds to define the mesh density a b In Elements, create mesh seeds. Select Create / Mesh Seed / Uniform Click on the top edge of the plate to create a mesh seed Then click on the right edge c

Step 3. Create a finite element mesh b In the Elements menu create surface mesh based on the mesh seeds assigned in the previous steps. Select Create / Mesh / Surface Select Quad as the Elem Shape Click on surface 1 Click Apply c d

Step 4. Apply boundary conditions to the model In Loads/BCs Select Create / Displacement / Nodal For New Set Name enter “constraints” In Input Data, enter <0,0,0> for Translations, <,0,> for Rotations then OK On the top menu click on the Curve or Edge icon In Select Application Region click lefthand edge of the surface Click Add and OK Click Apply e c b f g

Step 5. Apply loads to the model On the top menu click Reset Graphics Select Create / Distributed Loads / Element Uniform Enter “Dist. Load Y” for New Set Name In Input Data, Enter <0 –2000 0> for Edge Distr Load <f1 f2 f3>, then OK In Select Application Region, click on the top curve of the surface Click Add then OK Click Apply b e d c f g

Step 5a. Apply loads to the model (cont.) In a similar way create Dist. Load X: Enter “Dist. Load X” for New Set Name. In Input Data, Enter <0 –1000 0>, then OK In Select Application Region, click on the right hand side curve of the surface, then Add, then OK. Click Apply And then create Dist. Load XY: Enter “Dist. Load XY” for New Set Name. In Input Data, Enter <–1000 0 0>, then OK In Select Application Region, again click on the right hand side curve of the surface, then Add, then OK. Click Apply Note that since the same edge was picked, the loads are combined a e b c d

Step 6. Define ply material properties Go to Material menu Select Create / 2d Orthotropic / Manual Input For Material Name enter “graphite-epoxy_tape” Click Input Properties, Select Linear Elastic, enter 20e6, 2e6, .35, 1e6, 1e6, 1e6 Click OK Click Apply Click Input Properties again, Select Failure / Stress / Hill and enter 120e3, 13e3, 110e3, 16e3, 13e3, 5000. Click Apply again c f b g e h d

Step 7. Check Element Normals b Check element normals to determine the location of ply 1. Select the Element menu: At the top menu click Reset Graphics At the top menu click Hide Labels Select Verify / Element / Normals Click Draw Normal Vectors Click Apply c d e

Step 8. Define composite material properties Go to Materials: Select Create/ Composite/ Laminate At Material Name enter 8_ply_symmetric_quasi Click tape property name (graphite-epoxy_tape) slowly 8 times to make 8 plies At Thickness for all layers enter .0054<cr> Click on ply 1’s empty Orientation cell Enter the following into the Insert Orientations box: 0 -45 45 90 90 45 -45 0 . Note that the +-45 degree plies have changed sign due to the element Z axis being in the opposite direction to the global Z axis. Click Load Text Into Spreadsheet Click Apply e c b f d g h

Step 9. Define a material coordinate system Go to Geometry: Select Create / Coord / 3Point Enter Coord ID (99 in this case) you want at Coord ID list At Origin enter [0 0 0] At Point on Axis 3 enter [0 0 1] At Point on Plane 1-3 enter [0 1 0] Click Apply a b c d e f

Step 10. Apply the material coordinate system to the elements Go to Properties: Select Create / 2D / Shell Enter “composite1” at Property Set Name At Options select Laminate In Input Properties click on the composite material name (8_ply_symmetric_quasi) At Material Orientation select CID and then click the material coordinate system 99 on the screen Click OK Click Application Region and click on Surface 1 Click Add Click Apply a e b c d g f g h

Step 11. Submit the model to MSC.Nastran for analysis Go to Analysis: Select Analyze / Entire Model / Full Run Click Subcases At Available Subcases click Default Click Output Requests At Form Type select Advanced At Output Requests, click twice STRESS(SORT1,REAL,VONMISES,BINLIN)=ALL;PARAM,NOCOMPS,-1 At Composite Plate Opt: select Ply Stresses. Note that PARAM, NOCOMPS,-1 has now changed to 1. Click OK Click Apply at Subcases and then Cancel And click Apply at the Analyze menu a e c g f b h d j i

Step 12. Attach xdb Results File Go to Analysis: Select Attach XDB / Result Entities / Local Click Select Results File Use the Select File tool to find your xdb file in your local Patran directory and click it, in this case, “composite1.xdb” Click OK Click Apply a c d b e

Step 13. Display ply stresses using MSC.Patran b To display the ply 8’s 1 direction stresses: go to the Results menu: First turn off the geometry in Plot/Erase Geometry Erase Select Create / Quick Plot Click Stress Tensor Click Position then select Layer 8 and click Close Click Quantity and select X Component Click Displacements Translational Click Apply d c e f g

Step 14. View ply failure indices in MSC.Nastran To view the failure indices, open the composite1.f06 file in an editor and search for the following section. It is organized as follows: Element number Ply number Ply failure index Ply interlaminar failure index Highest failure index in element Flag if highest failure index is greater than 1.0 (indicating ply failure) F A I L U R E I N D I C E S F O R L A Y E R E D C O M P O S I T E E L E M E N T S ( Q U A D 4 ) ELEMENT FAILURE PLY FP=FAILURE INDEX FOR PLY FB=FAILURE INDEX FOR BONDING FAILURE INDEX FOR ELEMENT FLAG ID THEORY ID (DIRECT STRESSES/STRAINS) (INTER-LAMINAR STRESSES) MAX OF FP,FB FOR ALL PLIES 1 HILL 1 6.1711 0.0000 2 7.7170 3 6.4169 4 7.3154 5 7.3154 6 6.4169 7 7.7170 8 6.1711 7.7170 *** . c d a b e f Note that Patran does not display composite failure indices.

Step 15. Change layup to make failure indices below 1.0 Hand calculations Element 1, ply 2, a –45 degree ply, has the highest failure index of 7.72 but all of the plies have similar values, thus it is difficult to determine which direction to add plies. However, looking at the terms of Hill’s theorem may tell us: Substituting values: Shows that the 1 direction is the largest contributor to the failure and thus the composite needs more -45 degree plies. Using this same method, it was found that a 20 ply symmetric layup will give failure indices less than 1.0. The layup is a 0 ply, 4 45 plies, 2 –45 plies, and 3 90 plies and then a symmetric layup for the other 10 plies.

Step 15a. Change layup to make failure indices below 1.0 To change to a new layup: go to Materials: Select Modify / Composite / Laminate In Laminated Comp. To Modify click 8_ply_symmetric_quasi At New Material Name enter 0_4x45_2x-45_3x90_sym In the Laminated Composite popup click on ply 1 and then shift click on ply 8 to select all the plies Click on Delete Selected Rows Select Text Entry Mode Insert. In the Modify Menu on the right, click slowly on graphite-epoxy_tape 10 times, once for each ply On Stacking Sequence Convention select Symmetric At Thickness For All Layers enter .0054<cr> Click on the empty ply 1 Orientation cell Select Text Entry Mode Overwrite In Overwrite Orientations enter 0 45 45 45 45 -45 -45 90 90 90 Click Load Text Into Spreadsheet Click Apply h d j g b f k e l c i m n

Step 16. Analyze the model with the new composite layup Go to Analysis: Select Analyze / Entire Model / Full Run Click Apply Click Yes on both overwrite messages. a c c b

Step 17. View the changed ply failure indices To view the changed failure indices, again open the composite1.f06 file. Note that the failure indices are all below 1.0. F A I L U R E I N D I C E S F O R L A Y E R E D C O M P O S I T E E L E M E N T S ( Q U A D 4 ) ELEMENT FAILURE PLY FP=FAILURE INDEX FOR PLY FB=FAILURE INDEX FOR BONDING FAILURE INDEX FOR ELEMENT FLAG ID THEORY ID (DIRECT STRESSES/STRAINS) (INTER-LAMINAR STRESSES) MAX OF FP,FB FOR ALL PLIES 1 HILL 1 0.6422 0.0000 2 0.7709 3 0.7709 4 0.7709 5 0.7709 6 0.6580 7 0.6580 8 0.7494 9 0.7494 10 0.7494 11 0.7494 12 0.7494 13 0.7494 14 0.6580 15 0.6580 16 0.7709 17 0.7709 18 0.7709 19 0.7709 20 0.6422 0.7709