在早期采用ANSYS模拟混凝土时,很多时候会用到MISO本构模型,并且大部分是采用APDL来输入本构模型的应力应变曲线,如果采用Workbench来做,那么应该如何输入MISO本构曲线呢?本文略做解答。
与APDL的输入不同,我们采用常见命令TB,MISO输入的是总应变-应力曲线,而在WB中采用MISO时,要求输入的是塑性应变-应力曲线,常见的MISO混凝土本构应力-应变曲线命令流如下:
fc=26.8
Mp,ex,100,fc*0.19/0.0002
Mp,prxy,100,0.2
Mp,dens,100,2400e-12
TB,MISO,100,,11
TBPT,,0.0002,FC*0.19
TBPT,,0.0004,FC*0.36
TBPT,,0.0006,FC*0.51
TBPT,,0.0008,FC*0.64
TBPT,,0.0010,FC*0.75
TBPT,,0.0012,FC*0.84
TBPT,,0.0014,FC*0.91
TBPT,,0.0016,FC*0.96
TBPT,,0.0018,FC*0.99
TBPT,,0.002,FC
TBPT,,0.0033,FC
当然,APDL也可通过输入塑性应变-应力曲线,输入的命令抬头如下:
TB,PLAS,1,1,11,MISO
采用MISO模型时,其弹性模量不能小于应力-应变的斜率,一般取第一点的切线模量作为本构模型的弹性模量,塑性应变=总应变-弹性应变,弹性应变=应力/弹性模量,由于在WB中不能参数化,故此处在EXCEL中进行了相关计算,另外需注意,采用该本构曲线时,不能有下降段,最后计算得到的塑性应变-应力曲线如下所示:
在WB中定义的材料内容如下所示:
下面以一个简单的四周固结素混凝土板为例演示结果对比,板边长2m,厚度100mm,等级为C40,采用抗压设计值26.8Mpa,顶部受均布荷载0.5Mpa,采用185单元,APDL分析命令流如下:
finish
/clear
/prep7
et,1,solid185
etcon,set
fc=26.8
Mp,ex,100,fc*0.19/0.0002
Mp,prxy,100,0.2
Mp,dens,100,2400e-12
TB,MISO,100,,11
TBPT,,0.0002,FC*0.19
TBPT,,0.0004,FC*0.36
TBPT,,0.0006,FC*0.51
TBPT,,0.0008,FC*0.64
TBPT,,0.0010,FC*0.75
TBPT,,0.0012,FC*0.84
TBPT,,0.0014,FC*0.91
TBPT,,0.0016,FC*0.96
TBPT,,0.0018,FC*0.99
TBPT,,0.002,FC
TBPT,,0.0033,FC
blc4,,,2000,2000,100
lsel,s,length,,100
lesize,all,,,3
allsel,all
lsel,s,length,,2000
lesize,all,,,50
allsel,all
mat,100
vsweep,all
nsel,s,loc,x,0
nsel,a,loc,x,2000
d,all,all,0
nsel,s,loc,y,0
nsel,a,loc,y,2000
d,all,all,0
allsel,all
/solu
asel,s,loc,z,100
sfa,all,1,pres,0.5
allsel,all
cnvtol,f,,0.05
cnvtol,u,,0.05
cnvtol,m,-1
time,1
nsubst,1000,1000,1
autots,on
solve
/post1
set,last
plnsol,u,sum
在WB分析中,为了对比分析结果,网格划分以及单元的阶次尽量保持一致.
两者主要结果对比如下:
一、位移对比
WB位移最大值:6.0595mm,APDL位移最大值:6.01683mm
二、应力对比
可见两者都已达到屈服应力值
三、应变对比
弹性应变:
两者弹性应变均已达到最大值:0.001053
塑性应变:
两者最大值有一定差距,考虑是支座处应力集中造成的影响,选择跨中的点位进行对比,WB跨中点位的塑性应变为3.0052e-4,APDL跨中点位的塑性应变为2.99e-4,差距较小。
对比可见,采用上述思路可在WB中准确输入应力-应变曲线,有兴趣的同学可以尝试下!
暂无评论内容