《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）》请在三一办公上搜索。
1、,WS-1,WORKSHOP Define a Composite Material,NAS121,Workshop,May 6,2002,Problem DescriptionA 1 in.x 1 posite 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 co
2、nstraints.,Problem DescriptionThe 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 the angles are right hand rul
3、e 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 and strength properties are show
4、n on the right.The failure theorem to be used is Hill.,Suggested Exercise StepsCreate 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 normalsDefine com
5、posite material properties.Define a material coordinate systemApply the material coordinate system to the elements.Submit the model to MSC.Nastran for analysis.Attach xdb Results FileDisplay ply stresses using MSC.Patran.View ply failure indices in MSC.NastranChange layup to make failure indices bel
6、ow 1.0.Analyze the model with the new composite layupView the changed ply failure indices,CREATE NEW DATABASE,Create a new database called composite1.db:In File select NewEnter composite1 as the file nameClick OKChoose Default ToleranceSelect MSC.Nastran as the Analysis CodeSelect Structural as the
7、Analysis TypeClick OK,a,b,c,d,e,f,g,Step 1.Create a geometry model,In Geometry create the first curve.Select Create/Surface/VertexOn the Surface Vertex“n”Lists enter 0 0 0,1 0 0,1 1 0,0 1 0Click ApplyClick the Show Label icon,a,b,c,d,Step 2.Use mesh seeds to define the mesh density,In Elements,creat
8、e mesh seeds.Select Create/Mesh Seed/UniformClick on the top edge of the plate to create a mesh seedThen click on the right edge,a,b,c,Step 3.Create a finite element mesh,In the Elements menu create surface mesh based on the mesh seeds assigned in the previous steps.Select Create/Mesh/SurfaceSelect
9、Quad as the Elem ShapeClick on surface 1Click Apply,a,b,c,d,Step 4.Apply boundary conditions to the model,a,b,c,d,e,g,f,In Loads/BCsSelect Create/Displacement/NodalFor New Set Name enter“constraints”In Input Data,enter for Translations,for Rotations then OKOn the top menu click on the Curve or Edge
10、iconIn Select Application Region click lefthand edge of the surfaceClick Add and OKClick Apply,Step 5.Apply loads to the model,On the top menu click Reset GraphicsSelect Create/Distributed Loads/Element UniformEnter“Dist.Load Y”for New Set NameIn Input Data,Enter for Edge Distr Load,then OKIn Select
11、 Application Region,click on the top curve of the surfaceClick Add then OKClick Apply,b,c,d,e,g,f,a,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,then OKIn Select Application Region,click on the right hand side curv
12、e 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 OKIn Select Application Region,again click on the right hand side curve of the surface,then Add,then OK.Click ApplyNote that since the same edge was picked,th
13、e loads are combined,d,e,Step 6.Define ply material properties,Go to Material menuSelect Create/2d Orthotropic/Manual InputFor Material Name enter“graphite-epoxy_tape”Click Input Properties,Select Linear Elastic,enter 20e6,2e6,.35,1e6,1e6,1e6Click OKClick ApplyClick Input Properties again,Select Fai
14、lure/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 Element Normals,Check element normals to determine the location of ply 1.Select the Element menu:At the top menu click Reset GraphicsAt the top menu click Hide LabelsSelect Verify/Eleme
15、nt/Normals Click Draw Normal VectorsClick Apply,a,b,c,d,e,Step 8.Define composite material properties,Go to Materials:Select Create/Composite/LaminateAt Material Name enter 8_ply_symmetric_quasiClick tape property name(graphite-epoxy_tape)slowly 8 times to make 8 pliesAt Thickness for all layers ent
16、er.0054Click on ply 1s empty Orientation cellEnter 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 SpreadsheetClick Apply,a,b,c,d,
17、e,h,f,g,Step 9.Define a material coordinate system,Go to Geometry:Select Create/Coord/3PointEnter Coord ID(99 in this case)you want at Coord ID listAt Origin enter 0 0 0At Point on Axis 3 enter 0 0 1At Point on Plane 1-3 enter 0 1 0Click Apply,a,b,c,d,e,f,Step 10.Apply the material coordinate system
18、 to the elements,Go to Properties:Select Create/2D/ShellEnter“composite1”at Property Set NameAt Options select LaminateIn 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 screenClick
19、 OKClick Application Region and click on Surface 1Click AddClick 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 RunClick SubcasesAt Available Subcases click DefaultClick Output RequestsAt Form Type select AdvancedAt Output
20、 Requests,click twice STRESS(SORT1,REAL,VONMISES,BINLIN)=ALL;PARAM,NOCOMPS,-1At Composite Plate Opt:select Ply Stresses.Note that PARAM,NOCOMPS,-1 has now changed to 1.Click OKClick Apply at Subcases and then CancelAnd click Apply at the Analyze menu,a,b,c,e,f,g,h,i,j,d,Step 12.Attach xdb Results Fi
21、le,Go to Analysis:Select Attach XDB/Result Entities/LocalClick Select Results FileUse the Select File tool to find your xdb file in your local Patran directory and click it,in this case,“composite1.xdb”Click OKClick Apply,a,b,c,d,e,Step 13.Display ply stresses using MSC.Patran,To display the ply 8s
22、1 direction stresses:go to the Results menu:First turn off the geometry in Plot/Erase Geometry EraseSelect Create/Quick PlotClick Stress TensorClick Position then select Layer 8 and click CloseClick Quantity and select X ComponentClick Displacements TranslationalClick Apply,b,c,d,e,f,g,a,F A I L U R
23、 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
24、.7170 0.0000 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:Element
25、 numberPly numberPly failure indexPly interlaminar failure indexHighest failure index in elementFlag 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 calculationsElement 1,ply 2,a 45 degree ply,has the
26、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 and thus the compos
27、ite 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 failure indices below 1.0
28、,Step 15a.Change layup to make failure indices below 1.0,To change to a new layup:go to Materials:Select Modify/Composite/LaminateIn Laminated Comp.To Modify click 8_ply_symmetric_quasiAt New Material Name enter 0_4x45_2x-45_3x90_symIn the Laminated Composite popup click on ply 1 and then shift clic
29、k on ply 8 to select all the pliesClick on Delete Selected RowsSelect Text Entry Mode Insert.In the Modify Menu on the right,click slowly on graphite-epoxy_tape 10 times,once for each plyOn Stacking Sequence Convention select SymmetricAt Thickness For All Layers enter.0054Click on the empty ply 1 Or
30、ientation cellSelect Text Entry Mode OverwriteIn Overwrite Orientations enter 0 45 45 45 45-45-45 90 90 90Click Load Text Into SpreadsheetClick 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:Select Analyze/Entire Model/Full RunClick ApplyClick
31、 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 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)EL
32、EMENT 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,
