Ansys培训_随机振动分析

TrainingManual欢迎进入ANSYS技培训第五天TrainingManual随机振动(PSD)分析TrainingManualDYNAMICS11.0主要内容•定义和目的•Workbench随机振动分析功能•分析流程TrainingManualDYNAMICS11.0随机振动分析定义和目的什么是随机振动分析–基于概率的谱分析.–典型应用如火箭发射时结构承受的载荷谱，每次发射的谱不同，但统计规律相同.Reference:RandomvibrationsinmechanicalsystemsbyCrandall&MarkTrainingManualDYNAMICS11.0•和确定性谱分析不同，随机振动不能用瞬态动力学分析代替.•应用基于概率的功率谱密度分析，分析载荷作用过程中的统计规律Imagefrom“RandomVibrationsTheoryandPractice”byWirsching,PaezandOrtiz.随机振动分析定义和目的TrainingManualDYNAMICS11.0什么是PSD?•PSD是激励和响应的方差随频率的变化。–PSD曲线围成的面积是响应的方差.–PSD的单位是方差/Hz(如加速度功率谱的单位是G2/Hz).–PSD可以是位移、速度、加速度、力或压力.随机振动分析定义和目的TrainingManualDYNAMICS11.0输入:–结构的自然频率和阵型–功率谱密度曲线输出:–1s位移和应力（用于疲劳分析）.随机振动分析定义和目的TrainingManualDYNAMICS11.0•载荷:–单点激励•得到结果:–相对或绝对的1s输出–整体结构的结果，可以进行云图显示.–1s位移,速度或加速度•后处理:–1s可以进行云图显示.随机振动分析Workbench随机振动功能TrainingManualDYNAMICS11.0•Model:输电铁架•Analysis:地面激励PSD分析.•Steps:进行模态和随机振动分析，并显示结果.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0打开,Tower.dsdb.•Browsetofileifnotinlist随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•打开分析向导…随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•利用分析向导可以简单地建立分析流程.可以看到运行随机振动分析之前需要进行模态分析.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•点击OK可以看到如图所示信息•当提示“SpecifyNumberofModes”，输入12随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•下一步是插入约束，插入fixedsupport.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•模态分析结束.•可以查看模态结果，如右图所示.•可以查看动画.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•可以看到在谱分析中的初始条件已经自动设置成模态分析的结果.•设置阻尼（恒定阻尼比）0.05随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•插入一个PSDBaseExcitation.•在弹出的PSDBaseExcitation详情串口，选择新的PSD载荷.•选择带G的加速度PSD，单位G^2/Hz.•设置PSD曲线随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•选择激励方向为Y.•选择Solve.•求解结束后可以查看结果，可以选择1sigma到3sigma结果.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•如果列出了结果•更改阻尼比为0.05，查看结果.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0•按阻尼比0.05重新计算.随机振动分析随机振动分析流程TrainingManualDYNAMICS11.0练习•查看如图所示桁架结构在加速度PSD激励下的响应TrainingManualDYNAMICS11.0Workshop–目标•目标是研究桁架结构的振动特性.•这个练习将检查钢结构桁架由于加速度谱产生的位移和应力.•PSD谱可分为加速度、速度和位移.•Thespectrumwilltypicallybemeasuredduringphysicaltestsordocumentedinawrittenspecificationrelatingtothesystemorcomponent.–ThedatapointscanbeenteredforeachFreq&Amplitude,orafunctioncanbeentered.AccelerationFrequencyF1F2F3F4A2A3A4A1TrainingManualDYNAMICS11.0Workshop–假定•TheGirderhasfixedconstraintsalongallloweredges.•Theboundaryconditionswillbeappliedtoedges.TrainingManualDYNAMICS11.0Workshop–起始页•FromtheWorkBenchProjectLauncherstartSimulation.–ifalreadyinSimulationuseFileNew•Fortrainingpurposes,choose“No:donotsaveanyitems”•OnceinSimulationclickonGeometryFromFile…tobrowseforandopengirder.agdbTrainingManualDYNAMICS11.0Workshop–设置1.WhentheGeometryhasloaded,choose“RandomVibration”fromtheMapofAnalysisTypes1.Note,themapwillautomaticallyhighlight“Modal”toosincemodalisaprecursortoRandomVibrationsimulation.2.ClickOK,thusacceptingthedefaultnumberofmodes3.ChoosetheU.S.inchpoundunitsystem.–“UnitsU.S.Customary(in,lbm,lbf,…)”123TrainingManualDYNAMICS11.0Workshop–前处理-壳体厚度•TheGirdergeometryconsistsofsurfacebodies(forshellmeshing)•Thefirstpreprocessingtaskistospecifythethicknessofallthesurfaces.•ClicktofullyexpandtheGirder“Geometry”branch.–IntheDetailspane,noticethatthe“Thickness”fieldaredisplayedinyellowtoindicatetheyareundefined.4.Selectallthebodiestoassignauniformthickness1.LMBtoselectthetopBodyinthePartlist.2.HoldshiftandLMBonthelastSurfaceBody.–Note:Byhighlighting“all”,wecansetthethicknessonthefirstone,andthesamethicknessgetsassignedtoallofthem.•Ofcourseoneormoreindividualbodiescanberedefinedtodifferentthicknesseslaterifnecessary.5.Leftclickinthethicknessfieldandsetthethickness=0.5”54TrainingManualDYNAMICS11.0Workshop–前处理-接触•Theassemblytobeshellmeshedconsistsofmultiplesurfacebodiesseparatedbysmalloffsetsthataccountforthephysicalspacingbetweentheneutral(axis)planesofeachpieceofsteel.•Weneedtouse“Bonded”Contactinordertosimulatetheeffectofweldedand/orboltedassemblyconnectivity.6.ClickonConnectionsCreateAutomaticContact•TheDefaultdefinitionis“Bonded”6TrainingManualDYNAMICS11.0Workshop–前处理-网格尺寸•TheassemblyconsistsofmultipleslenderbodiesplusalargeflatRoofplate.•Wewanttospecifyarelativelyfinemeshsizeontheslendermembersbutalargerelementuptop.–Byassigninglargerelementsonthelargeroof,wepreserveCPUtimeandareabletousefiner(usuallymoreaccurate)elementselsewhere.7.ChangetoBodySelect.•OntheOutlineTree,RMBontheMeshobject8.InsertSizing(forslenderbodies)1.InDetails,Replace“Default”sizewith2(inches)2.RMBinGraphicsWindow,SelectAll3.ButthenholdCTRLandLMBsingleselectonthe“roofbody”tounselectthatpartfromthisSizeobject.4.Apply9.InsertSizing(forthelarge“roof”body)1.Enter“4”forsizeinDetails(forthelargetopplate).2.UseSingleSelectandLMBonthelargeBody.3.Apply10.Previewthemesh,MeshGenerateMesh1.Ifdesired,repeatthestepsabovetoincreaseordecreaseelementsizesasdesiredtoenhancethemodelorreduceCPUtime.78,910TrainingManualDYNAMICS11.0Workshop–环境11.Fortheloweredgesofthetruss,highlightthe“Modal”branchintheOutlineandInsertFixedSupports.12.Switchtoedgeselectionmodeasnecessary1.Reorientmodelasnecessarythroughout.2.anendviewmightbemostconvenient.13.SwitchtoBoxSelect1.DragtheLMBtoselecttheedgesatthebottomofthel