ANSYS實(shí)例1-四邊簡(jiǎn)支板模態(tài)分析命令流

1、復(fù)合材料四邊簡(jiǎn)支板模態(tài)分析摘要：本文介紹了復(fù)合材料四邊簡(jiǎn)支板的模態(tài)分析過(guò)程，介紹了ANSYS復(fù)合材料結(jié)構(gòu)分析的基本方法、步驟和過(guò)程，并介紹了單元類型的選擇、建模及后處理等多方面的內(nèi)容。關(guān)鍵詞：有限元；彈塑性；簡(jiǎn)支板；模態(tài)分析Modal Analysis of Composite Material Plate with Four Simply Supported EdgesAbtract: This paper introduces the modal analysis process of composite material plate with four simply supported

2、edges.This paper introduces the basic methods, steps and process of the ANSYS composite structure analysis , and introduces the unit type selection, modeling and post-processing and other aspects of content.Key Words: Finite element；Elastic plastic；Simply supported plate；Modal analysis一、前言如圖1所示的四邊簡(jiǎn)支

3、復(fù)合材料疊層方板，邊長(zhǎng)為8m,厚為0.04m,密度為2.16。疊層板共8層，鋪層為0/45/-45/90s,單層厚度為0.005m，各層材料屬性和厚度均相同，其中 ，試對(duì)其進(jìn)行模態(tài)分析。圖1 四邊簡(jiǎn)支復(fù)合材料疊層板示意圖二、 基于圖形界面(GUI)的交互式操作(step by step)過(guò)程如下 2.1定義工作環(huán)境（1）直接啟動(dòng)ANSYS，進(jìn)入ANSYS Multiphysics Utility Menu界面，利用File菜單下的Change Diretory、Change Jobname和Change Titile命令分別定義文件工作路徑、文件名和文件標(biāo)題。2.2定義單元類型和材料屬性（1）

4、選擇命令Main MenuPreferences，在Individual discipline to show in the GUI欄中選中Structural復(fù)選框，過(guò)濾掉ANSYS GUI菜單中與結(jié)構(gòu)分析無(wú)關(guān)的選項(xiàng)，單擊OK按鈕關(guān)閉該對(duì)話框。（2）選擇Main MenuPreprocessorElement TypeAdd/Edit/Delete命令，彈出Element Types對(duì)話框，單擊Add按鈕，彈出Library of Element types 對(duì)話框，在Library of Element types列表框中選擇Solidlayered46單元，即SOLID46 elemen

5、t type options對(duì)話框，如圖所示，保持默認(rèn)設(shè)置。單擊OK按鈕，彈出MoreSOLID46 element type options對(duì)話框，如圖所示，保持默認(rèn)設(shè)置，單擊OK按鈕關(guān)閉對(duì)話框，單擊Close按鈕關(guān)閉Element Types對(duì)話框。（3）選擇Main menuPreprocessorMaterial PropsMaterial Models命令，彈出Define Material Model Behavior對(duì)話框，在Material Models Available欄中依次展開StructruaLinear Elasticorthotropic選項(xiàng)，彈出對(duì)話框，設(shè)置參數(shù)

6、，單擊OK按鈕關(guān)閉該對(duì)話框。在Material Models Available 欄中依次展開StructuralDensity選項(xiàng)，彈出對(duì)話框，進(jìn)行參數(shù)設(shè)置，單擊OK按鈕關(guān)閉該對(duì)話框。在Define Material Model Behavior 對(duì)話框中選擇MaterialExit命令，關(guān)閉該對(duì)話框。（3）選擇Main MenuPreprocessorReal ConstantsAdd/Edit/Delete命令，彈出Real Constants對(duì)話框，單擊Add按鈕，選擇SOLIDE46單元，單擊OK按鈕，彈出對(duì)話框，設(shè)置實(shí)常數(shù)編號(hào)。單擊OK按鈕，彈出對(duì)話框，設(shè)置鋪層數(shù)及對(duì)稱性，Numb

7、er of layers為8,Layer Symmetry Key為1.單擊OK按鈕，返回Real Constants 對(duì)話框，單擊Close 按鈕結(jié)束實(shí)常數(shù)設(shè)置。（4）選擇ANSYS ToolbarSAVE_DB命令，保存上述操作。2.3創(chuàng)建幾何模型（1）選擇Main menuPreprocessorModelingCreateVolumesBlockBy Dimensions命令，彈出對(duì)話框，設(shè)置參數(shù)，單擊OK按鈕關(guān)閉該對(duì)話框。（2）選擇Utility MenuPlotCtrlsView SettingView Direction命令，彈出View Direction對(duì)話框，設(shè)置參數(shù)，單擊

8、OK按鈕關(guān)閉該對(duì)話框，此時(shí)，ANSYS顯示窗口顯示如圖2所示的生成塊的結(jié)果。圖3 網(wǎng)格劃分結(jié)果圖2 生成塊的結(jié)果（3）選擇ANSYS ToolbarSAVE_DB命令，保存上述操作。2.4劃分網(wǎng)格(1)選擇Main MenuPreprocessorMeshingMesh AttributesDefault Attribs命令，彈出Meshing Attributes對(duì)話框，采用默認(rèn)設(shè)置，單擊OK按鈕關(guān)閉該對(duì)話框。(2)選擇Main MenuPreprocessorMeshingSize CntrlsManualSizeGlobalSize命令，彈出Global Element Sizes對(duì)話框

9、，進(jìn)行參數(shù)設(shè)置，單擊OK按鈕關(guān)閉該對(duì)話框。(3)選擇Main MenuPreprocessorMeshingSize CntrlsManualSizeLinesPicked Lines命令，彈出線段拾取對(duì)話框，選擇塊體的4條短邊，單擊OK按鈕，彈出單元尺寸設(shè)置對(duì)話框，進(jìn)行參數(shù)設(shè)置，單擊OK按鈕關(guān)閉該對(duì)話框。(4)選擇Main MenuPreprocessorMeshingMeshVolumesMapped4 to 6 sided命令，彈出Mesh Volumes拾取菜單，用鼠標(biāo)在ANSYS顯示窗口中選擇塊體，單擊OK按鈕關(guān)閉該對(duì)話框，網(wǎng)格劃分結(jié)果如圖3所示。(5)選擇ANSYS Toolbar

10、SAVE_DB命令，保存上述操作。2.5加載求解(1)選擇Main MenuSolutionAnalysis TypeNew Analysis命令,彈出New Analysis對(duì)話框，選擇分析類型為Modal,單擊OK按鈕關(guān)閉該對(duì)話框。(2)選擇Main MenuSolutionAnalysis TypeAnalysisOptions命令,彈出Modal Analysis對(duì)話框，進(jìn)行參數(shù)設(shè)置。單擊OK按鈕，彈出Block Lanczos Method對(duì)話框，采用默認(rèn)設(shè)置,單擊OK按鈕關(guān)閉該對(duì)話框。(3)選擇Main MenuSolutionDefine LoadsApplyStruturalD

11、isplacementOn Nodes命令，彈出ApplyU,ROT on Nodes拾取菜單，拾取方式選擇Box，選擇塊體X=-4處的所有節(jié)點(diǎn)，單擊Apply按鈕，彈出ApplyU,ROT on Nodes對(duì)話框。在Lab2 DOFs to be constrained列表框中選擇UY和UZ選項(xiàng)，單擊Apply按鈕。按照該方法依次定義X=4處的約束為UY=0和UZ=0，Y=-4和Y=4處的約束為UX=0和UZ=0.定義完約束后的結(jié)果如圖4所示。圖4 定義約束后的結(jié)果(4)選擇Main MenuSolutionLoad Step OptsOut CtrlsSolu Printout命令，彈出S

12、olution PrintoutControls對(duì)話框，保持默認(rèn)設(shè)置，單擊OK按鈕關(guān)閉該對(duì)話框。(5)選擇Main MenuSolutionSolveCurrent LS命令，彈出/STATUS Command 和Solve Current Load Step對(duì)話框，單擊OK按鈕，ANSYS開始求解計(jì)算。(6)求解結(jié)束時(shí)，彈出Note對(duì)話框，單擊close按鈕關(guān)閉該對(duì)話框。(7)選擇ANSYS ToolbarSAVE_DB命令，保存上述操作。2.6查看求解結(jié)果(1)選擇Main MenuGeneral PostprocResults summary命令，查看求解結(jié)果摘要。(2)選擇Main M

13、enuGeneral PostprocRead ResultsFirst Set命令，讀入一階模態(tài)求解結(jié)果。選擇Main MenuGeneral PostprocPlot ResultsDeformed Shape命令，彈出Plot Deformed Shape對(duì)話框，在KUND Item to be plotted 欄中選擇Def+under edge 單選按鈕，單擊OK 按鈕，ANSYS顯示窗口將顯示變形后的幾何形狀和未變形的輪廓，如圖5所示。圖6 位移場(chǎng)分布等值線圖圖5 變形后的幾何形狀與未變形的輪廓(3)選擇Main MenuGeneral PostprocPlot ResultsCo

14、ntour PlotNodal Solu命令，彈出對(duì)話框，在Item to be comtoured列表框中依次展開Nodal SolutionDOF SolutionDiaplacement vector sum選項(xiàng)，其余選項(xiàng)采用默認(rèn)設(shè)置，單擊OK 按鈕，ANSYS顯示窗口將顯示如圖6所示的位移場(chǎng)分布等值線圖。(4)選擇Main MenuGeneral PostprocPlotCtrlsAnimateDeformed Results命令，彈出對(duì)話框，進(jìn)行參數(shù)設(shè)置，單擊OK按鈕，ANSYS 顯示窗口將以動(dòng)畫方式顯示一階模態(tài)振型，單擊close按鈕關(guān)閉動(dòng)畫顯示。 (5)選擇Main MenuGe

15、neral PostprocRead ResultsNext Set命令可以讀取下一模態(tài)求解結(jié)果數(shù)據(jù)，按照上訴方法可以查看相應(yīng)的求解結(jié)果。(6)選擇UtilityFileExit命令，彈出對(duì)話框，選擇Save Everything單選按鈕，單擊OK 按鈕，關(guān)閉ANSYS程序,如圖7所示最終動(dòng)態(tài)結(jié)果。圖7 最終動(dòng)態(tài)結(jié)果三、APDL命令流/clear,nostart/filename,chapter13-2,modal analysis/title,chapter13-2,simply supported laminated plate modal analysisC* using solid46

16、/prep76et,1,solid46 r,1,8,1 rmore rmore,1,0,0.005,1,45,0.005 rmore,1,-45,0.005,1,90,0.005 mp,ex,1,25e6 mp,ey,1,1e6mp,ez,1,1e6 ！定義單元類型為SOLID46！定義鋪層數(shù)位8，對(duì)稱鋪層！鋪層1和鋪層2的參數(shù)！鋪層1和鋪層2的參數(shù)！定義材料參數(shù)！假設(shè)EZ=EYmp,gxy,1,0.5e6mp,gyz,1,0.2e6mp,gxz,1,0.5e6mp,prxy,1,0.25mp,pryz,1,0.01mp,prxz,1,0.25mp,dens,1,2160 ！密度block,-

17、4,4,-4,4,0,0.04 ！建立幾何模型/view,1,1,1esize,12 ！控制總體網(wǎng)格劃分尺寸lsel,s,loc,x,-4 ！定義厚度方向網(wǎng)格劃分?jǐn)?shù)位1lsel,r,loc,y,-4lesize,all,1lsel,s,loc,x,-4lsel,r,loc,y,4lesize,all,1lsel,s,loc,x,4lsel,r,loc,y,-4lesize,all,1lsel,s,loc,x,4lsel,r,loc,y,4lesize,all,1allsel,allvmesh,1 ！網(wǎng)格劃分finish/solu ！進(jìn)入求解器antype,modal ！定義分析類型為模態(tài)分析modopt,lanb,5 ！定義模態(tài)參數(shù)提取方法為BLOCK LANCZOS法，提取前5階mxpand,5 ！定義模態(tài)擴(kuò)展數(shù)為5階outpr,1nsel,s,loc,x,4 ！定義約束d,all,uz,uynsel,s,loc,x,-4d,all,uz,uynsel,s,loc,y,-4d,all,uz,uxsolve ！求解finish /post1 ！進(jìn)入后處理器，查看求解結(jié)果set,list,2 ！查看求解結(jié)果摘要set,first ！讀取一階模態(tài)求解結(jié)果pldisp,0 ！圖形顯示一階模態(tài)振型anmode,10,.5e-1 ！