ansys面与面接触分析实例.docx
《ansys面与面接触分析实例.docx》由会员分享，可在线阅读，更多相关《ansys面与面接触分析实例.docx（14页珍藏版）》请在冰豆网上搜索。
ansys面与面接触分析实例
面与面接触实例：
插销拨拉问题分析
定义单元类型
Element/add/edit/delete
定义材料属性
MaterialProps/MaterialModels
Structural/Linear/Elastic/Isotropic
定义材料的摩擦系数
建立几何模型
Modeling/Create/Volumes/Block/ByDimensions
X1=Y1=0，X2=Y2=2，Z1=2.5，Z2=3.5
Modeling/Create/Volumes/Cylinder/ByDimensions
Modeling/Operate/Booleans/Subtract/Volumes
先拾取长方体，再拾取圆柱体。
Modeling/Create/Volumes/Cylinder/ByDimensions
划分掠扫网格
Meshing/SizeCntrls/ManualSize/Lines/PickedLines
拾取插销前端的水平和垂直直线，输入NDIV=3
再拾取插座前端的曲线，输入NDIV=4
PlotCtrls/Style/SizeandShape，在Facets/elementedge列表中选择2facets/edge
建立接触单元
Modeling/Create/Contactpair，弹出ContactManager对话框，如图所示。
单击最左边的按钮，启动ContactWizard（接触向导），如图所示。
单击PickTarget，选择目标面。
选择接触面
定义位移约束
施加对称约束，DefineLoads/Apply/Structural/Displacement/SymmetricB.C/OnAreas，选择对称面。
再固定插座的左侧面。
设置求解选项
AnalysisType/Sol’sControl
求解：
Solve/CurrentLS
绘制装配应力图
GeneralPostproc/PlotResults/ContourPlot/NodalSolution，选择Stress/vonMisesstress
求解拨拉过程
选择Z=4.5处的所有节点。
DefineLoads/Apply/Structural/Displacement/OnNodes，弹出ApplyU，ROTonNodes拾取框，单击PickAll按钮，选择UZ，在Displacementvalue输入1.7
Select/Everything
AnalysisType/Sol’sControl
Solve/CurrentLS
结果后处理
扩展模型：
Style/SymmetryExpansion/Priodic/CyclicSmmetry，在弹出的对话框中选择1/4DihedralSym
选择GeneralPostproc/ReadResults/Bytime/frequency，在TIME域输入120。
选择插销中与插座接触的单元，在SelectEntities中选择Element，在列表中选择ByElementname，再ElementName域输入174
Plot/Elements
GeneralPostproc/PlotResults/ContourPlot/NodalSolution，在对话框中选择Contact/ContactPressure
读入载荷步2结果。
ReadResults/ByLoadStep
绘制拨拉过程的应变变化动画
PlotCtrls/Animate/OverResults，弹出如图所示的对话框。
命令流操作：
（1）建立几何模型
/filename,bolt
/title,bolt_pullinganalysis
/PREP7
Block,-2,2,-2,2,2.5,3.5
/view,1,1,1,1
/ang,1
/rep,fast
Cylind,0.49,,2.5,3.5,0,360
Vsbv,1,2
Cylind,0.5,,2,4.5,0,360
/pnum,volu,1
Wpstyle,0.05,0.1,-1,1,0.003,0,0,,5
Wpstyle,,,,,,,,1
Wpro,,,90
Wsbw,all
Vdele,4,,,1
Vdele,6,,,1
Wpcsys,-1,0
Wpro,,90
Vsbw,all
Vdele,p51x,,,1
Wpcsys,-1,0
Wpstyle,,,,,,,,0
（2）定义单元类型、材料模型和网格划分
Et,1,solid185
Mptemp,,,,,,,,
Mptemp,1,0
Mpdata,ex,1,,36e6
Mpdata,prxy,1,,0.3
Lesize,4,,,3,,,,,0
Lesize,10,,,3,,,,,0
Lesize,18,,,4,,,,,0
Vsweep,all
/shrink,0
/eshape,0.0
/Efacet,2
/ratio,1,1,1
/cformat,32,0
（3）定义接触单元
/com,contactpaircreation-start
Cm,_nodecm,node
Cm,_elemcm,elem
Cm,_kpcm,kp
Cm,_linecm,line
Cm,_areacm,area
Cm,_volucm,volu
/gsav,cwz,gsav,,temp
Mp,mu,1,0.2
Mat,1
Mp,emis,1,7.88860905221e-031
R,3
Real,3
Et,2,170
Et,3,174
R,3,,,0.1,0.1,0
Rmore,,,1.0e20,0.0,1.0
Rmore,0.0,0,1.0,0.5
Rmore,0,1.0,1.0,0.0,,1.0
Keyopt,3,4,0
Keyopt,3,5,0
Nropt,unsym
Keyopt,3,7,0
Keyopt,3,8,0
Keyopt,3,10,1
Keyopt,3,11,0
Keyopt,3,12,0
Keyopt,3,2,0
Keyopt,3,5,0
Asel,s,,,23
Cm,_target,area
Type,2
Nsla,s,1
Esln,s,0
Esurf
Cmsel,s,_elemcm
Asel,s,,,27
Cm,_contact,area
Type,3
Nsla,s,1
Esln,s,0
Esurf
Allsel
Esel,all
Esel,s,type,,2
Esel,a,type,,3
Esel,r,real,,3
/psymb,esys,1
/pnum,type,1
/num,1
Eplot
Esel,all
Esel,s,type,,2
Esel,a,type,,3
Esel,r,real,,3
Cmsel,a,_nodecm
Cmdel,_nodecm
Cmsel,a,_elemcm
Cmdel,_elemcm
Cmsel,s,_kpcm
Cmdel,_kpcm
Cmsel,s,_linecm
Cmdel,_linecm
Cmsel,s_areacm
Cmdel,_areacm
Cmsel,s,_volucm
Cmdel,_volucm
/gres,cwz,gsav
Cmdel,_target
Cmdel,_contact
/com,contactpaircreation-end
（4）定义位移约束
Finish
aplot
/solu
Flst,2,4,5,orde,4
Fitem,2,3
Fitem,2,7
Fitem,2,11
Fitem,2,14
Da,p51x,symm
Flst,2,1,5,orde,1
Fitem,2,19
Da,p51x,all,0
（5）求解装配预应力
Antype,0
Nlgeom,1
Nsubst,1,0,0
Autots,0
Time,100
/status,solu
Solve
Finish
/post1
/efacet,1
Avprin,0
Plnsol,s,eqv,0,1.0
Save
（6）求解拨拉过程
Aplot
Nsel,s,loc,z,4.5
Finish
/sol
Antype,rest
D,all,,1.7,,,,uz,,,,,
Allsel,all
Nsrbst,100,10000,10
Outres,erase
Outres,all,all
Outots,1
Time,200
/status,solu
Solve
Finish
（7）结果后处理
/expand,4,polar,half,,90
Eplot
/post1
Set,,,1,,120
Esel,s,ename,,174
Eplot
/efacet,1
Avprin,0
Plnsol,cont,pres,0,1.0
Allsel,all
Set,2,last,1
/efacet,1
Avprin,0
Plnsol,s,eqv,0,1.0
Plns,s,eqv
Andata,0.5,,0,0,0,1,1,1
finish
/exit,all
升级会员 