《复合材料层合板分析.ppt》由会员分享，可在线阅读，更多相关《复合材料层合板分析.ppt（25页珍藏版）》请在三一文库上搜索。
1、,WS-1,WORKSHOP Define a Composite Material,NAS121, Workshop , May 6, 2002,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 w
2、ith 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 its fibers coming out of the page in the Y direction. Note that while the positive sense of th
3、e 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.) The composite plies are graphite/epoxy tape with a thickness of 0.0054 in. The elastic
4、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 pro
5、perties. 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.
6、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,Create a new database called composite1.db: In File select New Enter composite1 as the file name Click OK Choose Default Tolerance Select MS
7、C.Nastran as the Analysis Code Select Structural as the Analysis Type Click OK,a,b,c,d,e,f,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,a,b
8、,c,d,Step 2. Use mesh seeds to define the mesh density,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,a,b,c,Step 3. Create a finite element mesh,In the Elements menu create surface mesh based o
9、n the mesh seeds assigned in the previous steps. Select Create / Mesh / Surface Select Quad as the Elem Shape Click on surface 1 Click Apply,a,b,c,d,Step 4. Apply boundary conditions to the model,a,b,c,d,e,g,f,In Loads/BCs Select Create / Displacement / Nodal For New Set Name enter “constraints” In
10、Input Data, enter for Translations, 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,Step 5. Apply loads to the model,On the top menu click Reset Graphics Select Create / Distributed Loa
11、ds / Element Uniform Enter “Dist. Load Y” for New Set Name In Input Data, Enter for Edge Distr Load , then OK In Select Application Region, click on the top curve of the surface Click Add then OK Click Apply,b,c,d,e,g,f,a,Step 5a. Apply loads to the model (cont.),In a similar way create Dist. Load X
12、: Enter “Dist. Load X” for New Set Name. In Input Data, Enter , then OK In Select Application Region, click on the right hand side curve of the surface, then Add, then OK. Click Apply,a,b,c,And then create Dist. Load XY: Enter “Dist. Load XY” for New Set Name. In Input Data, Enter , then OK In Selec
13、t 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,d,e,Step 6. Define ply material properties,Go to Material menu Select Create / 2d Orthotropic / Manual Input For Material Nam
14、e 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 OK Click Apply again,a,b,c,d,e,f,g,h,Step 7. Check
15、Element Normals,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,a,b,c,d,e,Step 8. Define composite material properties,Go
16、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 Click on ply 1s empty Orientation cell Enter the following into the Insert Orientations
17、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,a,b,c,d,e,h,f,g,Step 9. Define a material coordinate system,Go to Geometry: Select Create / Co
18、ord / 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 “com
19、posite1” 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 A
20、dd Click Apply,a,b,d,e,f,g,h,c,g,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,VONM
21、ISES,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,b,c,e,f,g,h,i,j,d,Step 12. Attach xdb Results File,Go to Analysis: Select Attach XDB
22、 / 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,b,c,d,e,Step 13. Display ply stresses using MSC.Patran,To display the ply 8s 1 direction stresses: go
23、 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,b,c,d,e,f,g,a,F A I L U R E I N D I C E
24、 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 0
25、.0000 3 6.4169 0.0000 4 7.3154 0.0000 5 7.3154 0.0000 6 6.4169 0.0000 7 7.7170 0.0000 8 6.1711 7.7170 * . . .,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: Elem
26、ent 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),a,b,c,d,e,f,Note that Patran does not display composite failure indices.,Hand calculations Element 1, ply 2, a 45 degree
27、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 Hills theorem may tell us: Substituting values: Shows that the 1 direction is the largest contributor to the failure a
28、nd 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 15. Change layup to make
29、 failure indices below 1.0,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 pop
30、up 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
31、Layers enter .0054 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,a,b,c,d,e,g,k,j,i,h,n,m,l,f,Step 16. Analyze the model with the new composite layup,Go to Analysis
32、: Select Analyze / Entire Model / Full Run Click Apply Click Yes on both overwrite messages.,a,b,c,c,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
33、 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 0.0000 3 0.7709 0.0000 4 0.7709 0.0000 5 0.7709 0.0000 6 0.6580 0.0000 7 0.6580 0.0000 8 0.7494 0.0000 9 0.7494 0.0000 10 0.7494 0.0000 11 0.7494 0.0000 12 0.7494 0.0000 13 0.7494 0.0000 14 0.6580 0.0000 15 0.6580 0.0000 16 0.7709 0.0000 17 0.7709 0.0000 18 0.7709 0.0000 19 0.7709 0.0000 20 0.6422 0.7709,