ANSYS參數(shù)化設(shè)計(jì)（APDL）在均布荷載簡(jiǎn)支梁中的應(yīng)用實(shí)例分析目錄TOC\o"1-3"\h\u19783ANSYS參數(shù)化設(shè)計(jì)（APDL）在均布荷載簡(jiǎn)支梁中的應(yīng)用實(shí)例分析 -1-165681.1建立模型 -1-235871.2GUI操作步驟 -1-284381.3計(jì)算結(jié)果及分析 -7-295241.4APDL代碼 -9-105681.5形函數(shù)對(duì)計(jì)算結(jié)果的影響 -10-44971.5.1三種形函數(shù)對(duì)應(yīng)的計(jì)算結(jié)果（更改上述命令流的第八行參數(shù)） -10-9561.5.2結(jié)論 -10-1.1建立模型簡(jiǎn)支梁梁斷面（10mm×10mm）兩端鉸接10mm 10mm圖3-1簡(jiǎn)支梁平面模型及其界面尺寸1.2GUI操作步驟預(yù)處理Openpreprocessormenu打開預(yù)處理界面GiveexampleaTitle設(shè)置標(biāo)題為distributeloadingUtilityMenu>File>ChangeTitle…CreateKeypoints創(chuàng)建關(guān)鍵點(diǎn)Preprocessor>Modeling>Create>Keypoints>InActiveCS1、2節(jié)點(diǎn)坐標(biāo)如下圖3-2關(guān)鍵點(diǎn)位置坐標(biāo)DefineLines定義線Preprocessor>Modeling>Create>Lines>Lines>StraightLine在節(jié)點(diǎn)1和2之間連接線段DefineElementTypes定義類型Preprocessor>ElementType>Add/Edit/Delete...選擇beam188Sections選擇截面圖3-3選擇梁截面形狀DefineElementMaterialProperties定義材料屬性Preprocessor>MaterialProps>MaterialModels>Structural>Linear>Elastic>Isotropic彈性模量EX=200000泊松比PRXY=0.3圖3-4定義材料屬性DefineMeshSize定義網(wǎng)格尺寸網(wǎng)格尺寸為10mm圖3-5定義網(wǎng)格尺寸Meshtheframe網(wǎng)格化框架Preprocessor>Meshing>Mesh>Lines>click'PickAll' 施加荷載及求解DefineAnalysisType定義求解類型Solution>AnalysisType>NewAnalysis>StaticApplyConstraints施加約束Solution>DefineLoads>Apply>Structural>Displacement>OnKeypoints圖3-6增加支座ApplyLoads施加荷載SelectSolution>DefineLoads>Apply>Structural>Pressure>OnBeams點(diǎn)擊box選項(xiàng)，框選整段梁，點(diǎn)擊ok輸入均布荷載為1N/mm圖3-7ANSYS施加荷載輸入界面圖3-8施加荷載后的模型SolvetheSystem求解Solution>Solve>CurrentLS 顯示結(jié)果PlotDeformedShape繪制變形圖GeneralPostproc>PlotResults>DeformedShape圖3-9簡(jiǎn)支梁受彎后的變形圖PlotPrinciplestressdistribution顯示應(yīng)力GeneralPostproc>PlotResults>ContourPlot>NodalSolu進(jìn)入界面后點(diǎn)擊Stress>StressintensityUndisplacedshapekey選擇Deformedshapewithundeformedmodel 顯示單元形狀 PlotCrls>Style>SizeandShape… 將Displayodelement后的選項(xiàng)off切換為on最終結(jié)果圖3-10最終分析得出的應(yīng)力圖（圖中DMX為最大撓度）圖3-11簡(jiǎn)支梁左端應(yīng)力圖圖3-12簡(jiǎn)支梁中段應(yīng)力圖1.3計(jì)算結(jié)果及分析最大撓度驗(yàn)算：距離左端支座x處的截面彎矩為M=EI逐步積分得EIEIy=?由邊界條件y0=0，y故撓度最大為y通過(guò)ANSYS有限元分析得到最大撓度D誤差為78.156?78.133撓度有限元分析值和手算值近似相等最大正應(yīng)力驗(yàn)算：σmax圖3-13Excel計(jì)算數(shù)據(jù)如圖1-13中，ANSYS有限元分析得到的最大正應(yīng)力位置也在跨中的上下邊緣，為SMX，值為749.85MPa。750?749.85故最大正應(yīng)力電算、手算結(jié)果近似相等，精確度很高

1.4APDL代碼List>Files>LogFiles…打開APDL命令流界面，到最底端，復(fù)制出每步操作對(duì)應(yīng)的命令流即可。/CLEAR,START/title,DistributedLoadingofaBeam/PREP7K,1,0,0!DefinethekeypointsK,2,1000,0L,1,2!CreatethelineET,1,BEAM188!Beam188elementtypeKEYOPT,1,3,2MP,EX,1,200000!Young'sModulusMP,PRXY,1,0.33!Poisson'sratioSECTYPE,1,BEAM,RECT,,0SECOFFSET,CENTSECDATA,10,10,0,0,0,0,0,0,0,0,0,0ESIZE,10,0,LMESH,1FINISH/SOLUANTYPE,0!StaticanalysisDK,1,,,,0,UX,UY,UZ,ROTX,ROTY,,DK,2,,,,0,UY,,,,,,SFBEAM,all,2,PRES,1,,,,,,0/STATUS,SOLUSOLVEFINISH/POST1PLDISP,2!Plotdeformedshape/SHRINK,0/ESHAPE,1.0/EFACET,1/RATIO,1,1,1/CFORMAT,32,0/REPLOTPLNSOL,S,INT,1,1.0

1.5形函數(shù)對(duì)計(jì)算結(jié)果的影響1.5.1三種形函數(shù)對(duì)應(yīng)的計(jì)算結(jié)果（更改上述命令流的第八行參數(shù)）KEYOPT,1,3,0!形函數(shù)默認(rèn)為L(zhǎng)inearform線性計(jì)算結(jié)果