Ansys碳纤维分析实例（CFRP）

2016-12-12 by:CAE仿真在线来源:互联网

针对叶片中的梁、壳等复合材料层合结构,ANSYS提供了一系列的特殊单元——结构多层复合材料单元,以模拟各种复合材料。铺层单元中可以考虑复合材料特有的铺层特性和各向异性特性。

本计算采用的是相对简单的线性铺层单元Shell99。该单元是一种八节点3D壳单元,每个节点有六个自由度,主要适用于薄到中等厚度的板和壳结构,一般要求宽厚比应大于10。Shell99可实现多达250层的等厚材料层,或者125层厚度在单元面内呈现双线性变化的不等厚材料层。如果材料层大于250,用户可通过输入自己的材料矩阵形式来建立模型,还可以通过一个选项将单元节点偏置到结构的表层或底层。

关于ansys有限元软件对复合材料的支持,可参考:ANSYS复合材料分析技术介绍

下面是ansy分析碳纤维FRP【纤维增强复合材料(Fiber Reinforced Polymer/Plastic,简称FRP)】加固混凝土实例,APDL命令流如下:

*set,h,80
*set,B,500/2
*set,L,1800
*set,LF,100
*set,LS,50
*set,a,20
*set,PI,ACOS(-1)
*set,SR,PI*16
*set,RO,PI*(6/2)**2/200/h
*set,CB,300
*set,Ch,0.167
*set,CL,L-2*LS
*set,F1,0.002
*set,F2,30/LF
!定义完参数,开始建立模型
/prep7
et,1,solid65
et,2,link8
et,3,shell41
keyopt,3,1,2
et,4,solid45
mp,ex,1,18000
mp,prxy,1,0.2
!定义MISES本构关系
tb,kinh,1,1,7
tbpt,,0.0001,1.8
tbpt,,0.0004,6.66
tbpt,,0.0008,11.84
tbpt,,0.0012,15.54
tbpt,,0.0016,17.76
tbpt,,0.002,18.5
tbpt,,0.0033,18.5
tb,conc,1,1,9
tbdata,,0.3,0.5,1.75,-1
!钢筋双线性随动强化
mp,ex,2,2.1e5
mp,prxy,2,0.3
tb,bkin,2,1,2,1
tbdata,,235,0
!碳纤维线弹性
mp,ex,3,2.35e5
mp,prxy,3,0
!支座及整体钢筋
mp,ex,4,2.1e5
mp,prxy,4,0.3
r,1,2,RO,0,0,,,
rmore,,,,,,,
r,2,SR,,
r,3,CH,,
RMORE,,
!建立板模型
block,0,-B,0,h,-LF/2,-(L/2-LS)
lplot
/pnum,line,1
/replot
lgen,2,8,,,50,,,,0
lgen,2,13,,,100,,,,0
adrag,13,,,,,,9
adrag,14,,,,,,9
/pnum,line,0
/replot
v***a,1,7
v***a,3,8
!建立受力钢筋模型
lsel,s,loc,z,-LF/2
Lsel,r,loc,Y,0
lgen,2,all,,,,a,,,0
lsel,s,loc,z,-50
lsel,r,loc,y,A
adrag,all,,,,,,9
allsel,all
v***a,2,15
v***a,4,14
v***a,1,13
lsel,s,loc,y,0
lsel,a,loc,y,A
lsel,a,loc,y,H
lesize,all,50
lsel,s,loc,z,-LF/2
lsel,a,loc,z,-(L/2-LS)
lsel,u,loc,y,0
lsel,u,loc,y,a
lsel,u,loc,y,h
lesize,all,20
allsel,all
type,1
mat,1
real,1
esys,0
mshape,0,3D
mshkey,1
vmesh,all
asel,s,loc,z,-LF/2
!完成另一半板模型
type,1
extopt,esize,LF/50,0
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,LF
asel,s,loc,z,LF/2
type,1
extopt,esize,(L/2-LF/2-LS)/50,0
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,L/2-LF/2-LS
allsel,all
!生成支座模型
asel,s,loc,z,L/2-LS
type,1
extopt,esize,1,o
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,25
asel,s,loc,z,L/2-LS+25
type,1
extopt,esize,2,o
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,LS
asel,s,loc,z,-(L/2-LS)
type,1
extopt,esize,1,o
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,-25
asel,s,loc,z,-(L/2-LS+25)
type,1
extopt,esize,2,o
extopt,aclear,1
extopt,attr,0,0,0
mat,1
real,1
esys,0
vext,all,,,0,0,-LS
allsel,all
eplot
!划分钢筋单元
lsel,s,loc,x,-200
lsel,a,loc,x,-100
lsel,r,loc,y,A
type,2
mat,2
real,2
esys,0
lmesh,all
lsel,s,loc,x,0
lsel,r,loc,y,A
type,2
mat,2
real,2
esys,0
lmesh,all
allsel,all
!划分碳纤维单元
ksel,s,loc,z,850
ksel,r,loc,y,0
ksel,r,loc,x,0
kgen,2,all,,,-CB/2,,,,0
lstr,41,97
allsel,all
lstr,41,4
adrag,221,,,,,,222
asel,s,,,168
lsla,s
lesize,all,50,,,,,,,1
type,3
mat,3
real,3
esys,0
mshape,1,2D
amesh,all
allsel,all
nummrg,node,,,,low
numcmp,node
!划分支座单元
asel,s,loc,y,0
asel,r,loc,z,L/2-25,L/2+25
type,4
extopt,esize,1,0
extopt,aclear,1
extopt,attr,0,0,0
mat,4
real,3
esys,0
vext,all,,,0,-20
asel,s,loc,y,0
asel,r,loc,z,-(L/2-25),-(L/2+25)
type,4
extopt,esize,1,0
extopt,aclear,1
extopt,attr,0,0,0
mat,4
real,3
esys,0
vext,all,,,0,-20
allsel,all
finish
!设置边界
/solu
nsel,s,loc,x,0
/go
dsym,symm,x
nsel,s,loc,z,L/2
nsel,r,loc,y,-20
/go
D,all,,,,,,UY,
nsel,s,loc,z,-L/2
nsel,r,loc,y,-20
/go
D,all,,,,,,UY,UZ,
!加载1
antype,0
nlgeom,1
nropt,full
eqslv,spar,,0
allsel,all
outres,all,all
time,1
autots,1
nsubst,10,20,5,1
cnvtol,f,,0.05,2,,
neqit,30
pred,on,,on
esel,mat,3
ekill,all
allsel,all
solve
!加载2
asel,s,loc,y,h
asel,r,loc,z,-LF/2,LF/2
/go
sfa,all,1,pres,F2
outres,all,all
time,2
autots,0
nsubst,30,,,1
pred,-1
arclen,1,10,0,
esel,mat,3
ealive,all
allsel,all
solve
finish
!查看结果
/post1
esel,mat,1
set,1,last,1,
plnsol,s,z,0,1
set,2,last,1,
plnsol,s,z,0,1
finish
!查看碳纤维结果
/post26
allsel,all
nsel,s,loc,x,0
nsel,r,loc,y,0
nsel,r,loc,z,0
*get,N1,node,0,num,max
nsol,2,N1,U,Y
prod,3,2,,,,,,-1,1,1,
xvar,3
plvar,1
finish