风力发电机组有限元分析(FEA)Finite Element Analysis (FEA) for wind turbines2007年7月4日4th July 2007风机的有限元分析（FEA）–越来越重要FEA for wind turbines -increasingly important仅仅是几年前，有限元分析还仅仅用于相对简单的模型的计算。
Only a few years ago, FEA was used for relatively simple models目前：Presently:•越来越多的风机部件使用有限元进行分析Increasing number wind turbine components analysed using FEA•越来越多的细节在有限元模型中的体现，例如Increasing amount of detail in FE model for instance°变接触角轴承的表示法variable-contact-angle bearing representation°部件间具有有限摩擦的接触面的表示法（法兰表面的张开和移位）representation of contact between parts with finite friction (opening/ sliding of flange surfaces)°已装配螺栓的详细表示法detailed representation of bolts in assemblies•越来越多的复杂的非线性有限元Increasing number of complex, non-linear FEAFE analysis for wind turbinesFE analysis for wind turbines风机的FEA –在设计中的位置FEA for wind turbines -place in the design processGH 有限元分析过程GH FEA process规范regulations制造限制manufacturing limits 客户经验/偏好client experience/ preference质量quality人员通过Personnel access安装/安全assembly/safety与其他部件的接口interfaces with other components材料限制material limits最优/可接受的设计Optimal /acceptable design设计性能指标Design performance indicators:成本（材料，产品，运输，操作）Cost (material, production,transport, handling)重量Weight 强度StrengthFE analysis for wind turbinesMain bearing assemblyNacelle structureRotor headNacelle extenderBlade sectionPitch bearingPitch bearing plates(on top and bottom of inner race)同一组载荷下不同设计概念的比较comparison of different concepts under identical load sets最终设计尺寸强度的详细分析detailed analysis of strength of final design geometry风机的FEA –在设计中的位置FEA for wind turbines -place in the design process风机的FEA –最新的分析技术FEA for wind turbines -state of art technology德国劳埃德船级社2003版规范GL (Germanisher Lloyd) 2003 regulations有很大一章是对有限元分析的原则性和细节的要求Extensive chapter with general and detailed FEA requirements挪威船级社（丹麦规范）DNV (Danish regulations)对有限元分析的要求很少，认证更具一般性Fewer FEA requirements, more generic in certificationGarrad Hassan的工作符合GL的要求或更进一步Garrad Hassan work to GL requirements or furtherGL 规范GL regulationsGH 分析发展GH analysis development 某个部件的有限元分析—模型和实际之间的小差距FEA for certain components –narrow gap between model and realityGL接受新的或者改进的有限元分析方法acceptance and adoption by GLof new or improved FEAFE analysis for wind turbines叶片Blade•叶片blade•叶根连接blade root connection机械部件Machinery components•轮毂hub•主轴mainshaft•轮毂主轴连接hub to mainshaft connection •锁定销locking pin•其他螺栓连接other bolted connections 机舱结构Nacelle structure•主机架/底盘main frame/ bed plate•发电机架generator frame•轴承座bearing housings塔架Tower•塔顶（包括偏航轴承的影响）tower top (including influence of yaw bearing)•通道口（门，电缆，航空灯）access openings (door, cables, aviation light)•屈曲分析（仅限于非标准门）buckling analysis (only: non-standard doors)风机的有限元分析-模型总结FEA for wind turbines -FE models summarisedFE analysis for wind turbines风机的有限元分析-模型总结FEA for wind turbines -FE models summarised叶片bladeFE analysis for wind turbinesFE analysis for wind turbines风机的有限元分析-模型总结FEA for wind turbines -FE models summarisedNLR线性非线性包括其它结构分析中的刚度影响螺栓的疲劳和极限失效，包括法兰表面的张开/滑移（所以螺栓弯曲）和变桨轴承的影响叶片叶根叶片NLR非线性关系non-linear relationshipSCFBladeblade include stiffness effects in analysis of other structureslinear blade rootfatigue and ultimate failure in bolts, including effects of opening/ sliding of flange surfaces (hence: bolt bending) and pitch bearingnon-linearNLR除了热点应力（计算应力集中系数），还需要对照设计极限应力检查绝对应力σudas well as hot spotstresses (to calculate SCF),absolute stresses are checked against the design ultimatestress, σud应力集中系数stress concentrationfactor对于非线性分析，应力范围I 近似关系适合于用于计算SCF 的载荷循环for non-linear analyses,approximate relationship for stress ranges appropriate for applied fatigue cyclesto calculate SCFFE analysis for wind turbinesyellow = normal contact (friction coefficient 0.2)red = bonded contact ÆMPC algorithm风机的有限元分析-模型总结FEA for wind turbines -FE models summarised机械部件machinery componentsFE analysis for wind turbines风机的有限元分析-模型总结FEA for wind turbines -FE models summarisedNLR非线性非线性非线性螺栓的疲劳和极限失效，包括法兰表面的张开/滑移（所以螺栓弯曲）和任意附近轴承的影响螺栓的疲劳和极限失效，包括法兰表面的张开/滑移（所以螺栓弯曲）和任意附近轴承的影响包括其它结构分析中的刚度影响和非线性接触轮毂对主轴的连接其它螺栓连接主轴成SCF 非线性非线性线性疲劳和极限破坏的应力热点，包括变桨轴承的非线性影响轴上的热点，凹槽或螺纹处的应力集中，包括轴承的非线性影响销和盘的热点轮毂主轴锁定销和锁定盘机械部件(g)pgMachinery componentshubstress hot spots for fatigue and ultimate failure, including non-linear effects of pitch bearings and bolted connectionsnon-linearSCF mainshafthot spots in shaft, stress concentrations at grooves or threads, including non-lineareffects of bearingsnon-linear SCF locking pin and disk hot spots in pin and disk linear SCF hub to mainshaft connection fatigue and ultimate failure in bolts, including effects of opening/ sliding of flange surfaces (hence: bolt bending) and any nearby bearings non-linear NLR other bolted connections fatigue and ultimate failure in bolts, including effects of opening/ sliding of flange surfaces (hence: bolt bending) and any nearby bearings non-linear NLR main bearinginclude stiffness effects and non-linear contact in analysis of other structuresnon-linear风机的有限元分析-模型总结FEA for wind turbines -FE models summarised机舱结构nacellestructureFE analysis for wind turbinesFE analysis for wind turbinesNLR/SCF SCF SCF非线性线性线性线性焊缝疲劳破坏和其它热点，包括法兰张开和偏航轴承的非线性接触焊缝的疲劳破坏模态分析包括其它结构分析中的刚度影响主机架/底盘副属机架/发电机架副属机架/发电机架轴承座机舱结构Nacelle structuremain frame/ bed platefatigue damage at welds and other hot spots, including effects of flange opening and non-linear contact in yaw bearing non-linearNLR/ SCFauxiliary frame/ generator frame fatigue damage at welds linear SCF auxiliary frame/ generator frame modal analysislinear SCF bearing housingsinclude stiffness effects of bearing housing in analysis of other structureslinearTFE analysis for wind turbines塔架tower8-point contactbearing (slewing ring)three bolted connections风机的有限元分析-模型总结FEA for wind turbines -FE models summarisedFE analysis for wind turbines风机的有限元分析-模型总结FEA for wind turbines -FE models summarisedSCF非线性非线性塔筒底部法兰焊缝的疲劳破坏，包括法兰张开的影响焊缝疲劳破坏，洞周围的应力集中，包括法兰张开的效果塔底法兰塔筒地基嵌入环线性压曲抗力系数线性特征值分析，分析方法不限，非均匀或非锥形壳屈居分析SCF非线性线性塔头法兰焊缝疲劳破坏，包括法兰张开和偏航轴承的非线性接触焊缝的疲劳破坏塔头通道口塔架Towertower top fatigue damage at top flange weld including effects of flange opening and non-linear contact in yaw bearing non-linearSCFaccess openings fatigue damage at weldslinear SCFbuckling analysis eigen-analysis of doors outside limits of analytical method, non-uniform or non-conical shellslinearlinear bucklingresistance factortower base flange fatigue damage at bottom flange weld including effects of flange openingnon-linear SCFtower foundation insert fatigue damage at welds, stress concentrations around holes including effects of flange openingnon-linearSCF有限元建模讨论FE modelling Workshop FE modelling讲到的有限元分析有：The following FEA will be presented:•塔筒底部的入口Access door in tower base•塔头法兰焊缝分析Tower top flange weld analysis•主轴分析Mainshaft analysis•轮毂和主轴之间的螺栓连接Bolted connection between hub and mainshaftFE analysis for wind turbinesFE analysis for wind turbines主要有限元目标Main FE modelling goals-重新获得焊趾位置的应力（疲劳分析）Retrieving stresses at weld toe locations (fatigue analysis)-重新获得门位置的von Mises 应力最大值（检查屈服）Retrieving the maximum von Mises stress at door location (check on yield)有限元模型细节FE model specifics-使用体单元而不是壳单元（GL 的要求）solid elements not shells (required by GL)-塔筒截段的高度最小为2.5 ×Dtower section height of minimum 2.5 ×D有限元建模塔筒入口FE modellingTower access door1/12重新获得焊趾位置的应力Retrieving stress results from the FE model at weldlocation推荐EuroCode3/ 国际焊接协会(IIW)Recommendations from EuroCode3/ International Institute of Welding (IIW)reference pointsstructural stresshot spot Fcomputed total stressF0.4*t0.4*t1*tt有限元建模塔筒入口FE modelling Tower access door2/12FE analysis for wind turbinesFE analysis for wind turbinesStep 1•在CAD (SolidWorks).软件中创建3维门模型3D door model created in CAD (SolidWorks).•在CAD 软件中创建面（用于切割焊缝位置的体）surfaces (to be used for cutting the solid at weld locations) created in CAD.•导入CAE 软件imported into CAE.切割CAD 模型中创建的面Cutting surfaces created in CAD package有限元建模塔筒入口FE modellingTower access door3/12Step 2•用导入的面切割导入的体imported solid cut using imported surfaces•创建新体new solids created•用从塔筒向外复制小面（操作后会删除）的方法切割法兰顶部区域（法兰侧焊接位置）flange top area (flange side weld locations) cut by copying small area offset from tower wall (cut areas are deleted after operation)用导入的面切割体Solid is cut by imported areas 顶部区域用复制的面切割（6个）Top area is cut bycopied areas (6 areas)有限元建模塔筒入口FE modelling Tower access door4/12FE analysis for wind turbinesFE analysis for wind turbiness w e e p m e s hStep 3用工作面切割体以便得到扫略网格The solid is also cut by the workplane to make a sweep mesh possible用水平工作面切割Cut by ‘horizontal’workplane有限元建模塔筒入口FE modellingTower access door5/12有限元建模塔筒入口FE modelling Tower access door6/12Step 41 门区域之外的主要塔筒截面是扫略得到的solid95高阶单元The main tower sections outside the door area are sweep meshed with solid95 higher order elements2 门区域截面用面单元(Mesh200)细化The door area cross section is finely meshed with surface (Mesh200) elements3 焊缝附近的位置面网格细化In the vicinity of the weld the surface mesh is refined网格细化Mesh refinementFE analysis for wind turbines有限元建模塔筒入口FE modelling Tower access door7/12Step 5门和周围直接连接的壳用扫略划分网格door and shell immediatelyaround it are sweep meshed门框架区域和塔架主体之间的壳用四面体单元直接划分shell between door frame region and main towermeshed automatically with tetrahedra15200个Solid95单元15200 Solid95 elementsFE analysis for wind turbinesFE analysis for wind turbinesX T Pointing South.Z T Vertically upwards.Y TPointing East.OriginAt each tower station.塔架载荷和挠曲的坐标系协调Co-ordinate systems for tower loads and deflections在CAD 例子中指定的轴和原点axes and origin designated in CAD,example shown here改变坐标系change system of coordinates有限元建模塔筒入口FE modellingTower access door8/12FE analysis for wind turbines对称条件Symmetry condition所有自由度约束Fixed in all DOFM y =1NmStep 6施加单位载荷Mx=1Nm 求解模型model solved with a unit load M x =1Nm应力Stress: vonMises变形比例Scale deformation =1e9有限元建模塔筒入口FE modellingTower access door9/12FE analysis for wind turbines不对称条件Asymmetry condition所有自由度约束Fixed in all DOFM z =1NmStep 7施加单位载荷M y = 1Nm 求解模型model solved with a unit load M y = 1Nm应力Stress: vonMises变形比例Scale deformation =1e9有限元建模塔筒入口FE modellingTower access door10/12FE analysis for wind turbines应力结果用沿焊缝的“移动的”随动局部坐标系Stress results are read in “moving”local coordinate system aligned with weldStep 8焊趾处的3个应力分量three stress components are read at weld toe:1.与焊趾平行的应力stress parallel with weld 2.与焊趾垂直的应力stress perpendicular with weld 3.面内剪应力in plane shear stress有限元建模塔筒入口FE modellingTower access door11/12FE analysis for wind turbinesS tre s s e s a t d o o r w e ld , o u ts id e to w e r w a llAA-6-4-2024681000.511.522.53T o w er h eig h t [m ]S t r e s s [P a ]S x_Mx S y_Mx S xy_Mx S x_My S y_My S xy_My P 1_Mx P 3_MxPosition Name Node X Pos Y Pos MaxPS_Mx Sx_Mx Sx_My Sy_Mx Sy_My [-][-][no][m][m][N/m 2][N/m 2][N/m 2][N/m 2][N/m 2]Door tower wall, outside A 137500.40 2.08-6.31-5.61-2.96-0.188.01Door tower wall, inside B 136260.37 2.19-9.22-6.08-12.04-2.93-13.92Door flange, outside C 199780.40 2.02-7.51-7.38-7.11-6.39-5.92Door flange, inside D 205820.37 2.13-8.09-6.40-8.93-5.08-7.86Base flange, outside E 623090.820.08-8.75-2.55 1.21-8.74 3.58Base flange, insideF622180.550.09-3.93-0.980.36-3.931.20Step 91计算M x 引起的主应力（PS ）Principal Stresses (PS) due to M x load calculated 2 画应力结果图Graphs plotted of stress results3 Mx 引起的主应力（PS ）的最大值决定热点max. (abs) PS due to the M x load determines hotspot position4 生成影响线矩阵Influence matrix generated有限元建模塔筒入口FE modellingTower access door12/12有限元建模塔顶法兰焊缝分析FE modelling Tower top flange weld analysis1/15Main FE modelling goal决定关联载荷和焊缝的应力（疲劳和极限分析）Determination of the relationship load and stress in weld (fatigue andextreme analysis)FE model specifics有限元模型细节-使用体单元Solid elements will be used-模型中包括部分塔架，法兰，偏航轴承Part of tower, flange, yaw bearing is modelled-非线性分析ÆNon linear analysisÆ-可能有（局部）连接的张开possible (partial) opening of connection-活动支座滚珠接触shifting bearing ball contact-变化的轴承滚珠刚度changing bearing ball stiffnessFE analysis for wind turbines有限元建模塔顶法兰焊缝分析FE modelling Tower top flange weld analysis2/15Step 1导入SolidWorks2维面模型SolidWorks2D model of areas is imported Step 2在轴承座圈位置，模型是由多线组成的面（90根线组成圆）At bearing race positions, areas formed from poly lines (90 lines forming circle) are modelled部分机舱底座part of nacelle bed plate偏航轴承yaw bearing刹车盘brake disk塔头法兰tower top flange塔筒tower sectionFE analysis for wind turbines有限元建模塔顶法兰焊缝分析FE modelling Tower top flange weld analysis3/15 Step 31 用圆来切割模型The circles are used to cut the model2 螺栓的位置需要切割（工作面切割）Cuts are made for bolt position (work plane cut)3法兰焊缝的位置需要切割（工作面切割）Cuts are made at flange weld location (work plane cut)螺栓位置bolt location多线组成的轴承座圈bearing race formed by poly lines螺栓位置bolt location焊缝位置收缩法兰weld locationnecked flangeFE analysis for wind turbinesFE analysis for wind turbinesStep 41 用表面单元划分面的网格areas meshed with surface elements 2 焊缝位置网格细化（关心的区域）mesh refined in weld area (area of interest)网格细化M e sh r e fin e m e nt有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis4/15有限元建模塔顶法兰焊缝分析FE modelling Tower top flange weld analysis5/15Step 5网格沿轴向旋转mesh rotated around axis28000个Solid45 单元28000 Solid45 elementsFE analysis for wind turbinesFE analysis for wind turbinesd ir e cti o n o f i n i t i a l c on t a c td ir e c t i o n o f i n i t i a lc o n t a c t 使用Li n k 10单元的初始应变特性表示间隙R e p r e s e n t a t i o n o f g a p m o d e l l e d u s i n g i n i t i a l s t r ai n p r o p e r t y o fL I N K 10 e le m e nt sStep 7用Link10单元（单元仅受压）表示轴承滚珠Link10 (compression only elements) are modelled to represent the bearing balls有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis6/15FE analysis for wind turbinesStep 8用Beam 4单元表示螺栓Beam 4 elements are modelled to represent the boltsStep 91 模型中包括接触Contact is modelled2 模型中包括“载荷伞”Load umbrella is modelled塔头=载荷施加Tower top =load applicationcontact有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis7/15FE analysis for wind turbinesStep 10载荷步1：通过给螺栓设置温度（收缩梁）实现螺栓预加载Load step 1: Bolt preload step is solved by applying temperature on bolts (contracting beams)结果显示：仅螺栓预载荷(M z =0kNm)Results shown: Only bolt pre load (M z =0kNm)变形比例= 500Scale deformation = 500有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis8/15Step 11载荷步3：分5个子步施加实际Mz弯矩(7000kNm)求解模型Load step 3: Model is solved with realistic Mz moment (7000kNm) in 5 sub steps结果显示：Mz =7000kNmResults shown: Mz =7000kNm变形比例= 100Scale deformation = 100失去接触Loss of contact有限元建模塔顶法兰焊缝分析FE modelling Tower top flange weld analysis9/15FE analysis for wind turbinesFE analysis for wind turbines受压侧Compression side M z =7000kNm Sy stress 受拉侧Tensile side M z =7000kNm Sy stressLoc1Loc2焊趾位置应力最大weld toe location highest stressed有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis10/15FE analysis for wind turbinesNLR between stress and moment at 4 tower top locations-150.00-100.00-50.000.0050.00100.00150.00200.00-8000000-6000000-4000000-20000002000000400000060000008000000moment [Nm]S t r e s s [M P a ]Outside 1Inside 1Outside 2Inside 2-螺栓应力和弯矩的非线性关系Non linear relationship bolt stress and applied moment -M y ,hub 或M z ,hub 载荷时程（旋转坐标系）Load time history M y ,hub or M z ,hub (rotating coordinate sys.)Step 11生成应力/ Nm 焊趾非线性影响关系non linear influence relationship weld toe stress / Nm is generated螺栓应力时程（使用Bladed ）bolt stress time history (using Bladed)极限螺栓应力extreme bolt stress寿命周期内疲劳损伤lifetime fatigue damage有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis11/15FE analysis for wind turbinesR e s u lt a n t c o n t a c t a n g le-80.00-60.00-40.00-20.000.0020.0040.0060.0080.0020406080100120140160180200R a d ia l p o s it io n [d e g ]C o n t a c t a n g l e [d e g ]T e n s i le s i d eC o m p r e s s i o n s i d e对于每一个载荷步，可以计算得到合成的接触角For each load step, a resultant contact angle can be calculated接触结果与前面使用固定45度接触角建模时得到的结果十分不同Æ对焊缝位置应力结果影响很大（大概减少20%）Contact results are very different compared to previous modelling with a fixed contact angle of 45 degrees Ælarge influence on stress results weld location (around 20%reduction)Loc1, 受拉侧tensile side Loc2, 受压侧compression side有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis12/15FE analysis for wind turbines检查轴承滚珠接触Check on realism of bearing ball contact轴承面外所有自由度完全约束Outside bearing areais fully constraint in all DOF刚度很高的载荷伞Very stiff load umbrellaF radial = 8000 kN对称条件Symmetry conditions有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis13/15FE analysis for wind turbines无量纲力无量纲位移有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis14/15FE analysis for wind turbines8点接触轴承（回转支承）8-point contactbearing (slewing ring)3个螺栓连接three bolted connections有限元建模塔顶法兰焊缝分析FE modellingTower top flange weld analysis15/15有限元建模主轴FE modelling Mainshaft 1/11主要有限元建模目的Main FE modelling goal指定主轴表面“热点”的位置Allocate hotspot locations on shaft surface产生“热点”周围的影响线矩阵Produce influence matrix for all the foundhotspots有限元模型细节FE model specifics-静态分析（“热点”分析）Static analysis (hotspot analysis)-使用体单元Solid elements will be applied-模型中包括部分轮毂Part of hub is modelled-模型中包括轴承状态（双球滚子形式）Bearing behaviour (double spherical rollerlay-out) is modelledFE analysis for wind turbinesStep 1主轴的SolidWorks3维模型，轮毂和内轴承座圈很重要SolidWorks3D model of mainshaft, hub and inner bearing races is imported Step 2体模型被切开，沿主轴轴向的截面和部分轮毂被留下Solid model is cut and cross section over the length of the shaft and part of hub is left有限元建模主轴FE modelling Mainshaft2/11FE analysis for wind turbinesFE analysis for wind turbinesStep 3Mesh200单元划分面的网格area meshed with Mesh200 elementsStep 4在关键区域首次细化网格initial mesh refined in critical areasStep 5在关键区域二次细化网格（轮毂侧和齿轮箱侧轴承位置）second mesh refined in critical areas (hub side and gearbox side bearings positions)网格细化1Mesh refinement 1网格细化2Mesh refinement 2有限元建模主轴FE modellingMainshaft3/11有限元建模主轴FE modelling Mainshaft4/11 Step 6面网格绕主轴轴线旋转生成solid 95（高阶）体单元模型area mesh revolved around shaft axis to generate asolid model with solid 95 (higher order) elements36200个Solid95单元36200 Solid95 elementsFE analysis for wind turbines有限元建模主轴FE modelling Mainshaft5/11 Step 6用非常细（没有刚度）的shell 93单元划分体模型网格The solid model is meshed with very thin (nostiffness) shell 93 elements.这些单元会在后处理中用于获取模型表面的应力These elements will be used in the postprocessing phase to extract stresses from thesurface of the model6200个shell 93 单元6200 Shell93 elementsFE analysis for wind turbinesFE analysis for wind turbinesStep 7用非线性Link10单元的“蛛网”表示轴承滚子（刚度建模）Spider webs of non linear Link10 elements are modelled to represent the bearing rollers (stiffness is modelled)Link10单元仅用于承受拉伸载荷的建模The Link10 elements are modelled only to take loading under tensile432个非线性Link10单元（仅受拉伸）432 non linear Link10 elements (tensile only option)轴承中心位置的中心节点Central node at bearing centre position把Link 单元连接到内轴承座圈的外表面Link elements are connected to the outside surface of the inner bearing race有限元建模主轴FE modellingMainshaft6/11FE analysis for wind turbinesStep 81 载荷施加点和“载荷伞”建模1 Load application node and load umbrella is modelled2 齿轮箱安装刚度建模（具有恰当刚度的梁单元）2 Gearbox mounting stiffness is modelled (Beam elements with correct stiffness)3 施加边界条件3 Boundary conditions are applied边界条件Boundary conditions齿轮箱安装刚度Gearbox mounting stiffness施加齿轮箱重量Gearbox weight application施加载荷Load application边界条件Boundary conditions有限元建模主轴FE modellingMainshaft7/11FE analysis for wind turbinesStep 9模型上施加了下列载荷：The following loads have been applied to the model 11个单位载荷：11 unit loads:+F x , -F x , +F y , -F y , +F z , -F z +M x , +M y , -M y , +M z , -M z4个变速箱载荷（实际重力载荷）：4 Gearbox loads (real gravity loads):+F y , -F y , +F z , -F zShell 93 单元M y = 1NmvonMises 应力Solid 95 单元M y = 1NmvonMises 应力Shell 93 elements M y = 1NmStress=vonMisesSolid 95 elements M y = 1NmStress=vonMises有限元建模主轴FE modellingMainshaft8/11。
