百思

 找回密码
 注册
快捷导航
搜索
查看: 864|回复: 4

[求助] 请教关于梁的屈曲和极限承载力问题

[复制链接]

该用户从未签到

发表于 2007-12-19 10:49:24 | |阅读模式
各位高手: <br />
&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;大家好!我在利用ANSYS计算简支工子钢梁的屈曲遇到一些问题,请各位朋友提出您的宝贵意见,问题详见如下: <br />
&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;大家知道,特征值屈曲计算得到的极限荷载应该与弹性下的理论极限荷载值相同,当梁中央作用集中荷载P时,ANSYS计算得到的极限荷载和钢结构书中的理论值相同,但是梁上作用均布荷载q或梁两端同时作用弯矩M时,计算得到的ANSYS值与理论值差别很大。 <br />
&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;&nbsp;理论值是根据《钢结构》书上钢梁的整体稳定计算那一章的公式计算得来的&nbsp;&nbsp;<br />
&nbsp;&nbsp;&nbsp;&nbsp;AYSYS计算梁顶作用均布荷载是的特征值屈曲的命令流如下: <br />
&nbsp;&nbsp;&nbsp;&nbsp; <br />
&nbsp;&nbsp;/com,structural <br />
/units,si <br />
&nbsp;&nbsp;<br />
/prep7 <br />
!定义单元类型 <br />
et,1,solid45 <br />
&nbsp;&nbsp;<br />
!定义材料属性 <br />
mp,ex,1,2.1e11 <br />
mp,prxy,1,0.3 <br />
mp,dens,1,7800 <br />
&nbsp;&nbsp;<br />
*do,i,1,12 <br />
k,1+(i-1)*4,(i-1)*0.4,-0.18,0.01 <br />
k,2+(i-1)*4,(i-1)*0.4,0.18,0.01 <br />
k,3+(i-1)*4,(i-1)*0.4,0.18,-0.01 <br />
k,4+(i-1)*4,(i-1)*0.4,-0.18,-0.01 <br />
*enddo <br />
k,49,4.8,-0.18,0.01 <br />
k,50,4.8,0,0.01 <br />
k,51,4.8,0.18,0.01 <br />
k,52,4.8,-0.18,-0.01 <br />
k,53,4.8,0,-0.01 <br />
k,54,4.8,0.18,-0.01 <br />
&nbsp;&nbsp;<br />
k,55,0,0,-0.01 <br />
k,56,0,0,0.01 <br />
&nbsp;&nbsp;<br />
a,3,55,56,2 <br />
a,55,4,1,56 <br />
a,4,1,5,8 <br />
a,8,5,6,7 <br />
a,3,2,6,7 <br />
a,1,5,6,2,56 <br />
a,4,8,7,3,55 <br />
va,1,2,3,4,5,6,7 <br />
&nbsp;&nbsp;<br />
*do,i,2,11 <br />
v,1+(i-1)*4,2+(i-1)*4,3+(i-1)*4,4+(i-1)*4,1+i*4,2+i*4,3+i*4,4+i*4 <br />
*enddo <br />
a,46,45,49,50,51 <br />
a,45,49,52,48 <br />
a,49,52,53,50 <br />
a,50,53,54,51 <br />
a,46,51,54,47 <br />
a,48,52,53,54,47 <br />
va,57,58,59,60,61,62,63 <br />
&nbsp;&nbsp;<br />
*do,i,1,2 <br />
k,57+(i-1)*8,(i-1)*4.8,-0.2,0.1 <br />
k,58+(i-1)*8,(i-1)*4.8,-0.18,0.1 <br />
k,59+(i-1)*8,(i-1)*4.8,-0.18,-0.1 <br />
k,60+(i-1)*8,(i-1)*4.8,-0.2,-0.1 <br />
k,61+(i-1)*8,(i-1)*4.8,0.18,0.1 <br />
k,62+(i-1)*8,(i-1)*4.8,0.2,0.1 <br />
k,63+(i-1)*8,(i-1)*4.8,0.2,-0.1 <br />
k,64+(i-1)*8,(i-1)*4.8,0.18,-0.1 <br />
*enddo <br />
v,57,58,59,60,65,66,67,68 <br />
v,61,62,63,64,69,70,71,72 <br />
&nbsp;&nbsp;<br />
vglue,all <br />
&nbsp;&nbsp;<br />
!划分网格 <br />
type,1 <br />
mat,1 <br />
&nbsp;&nbsp;<br />
lesize,1,,,18,,,,,1 <br />
lesize,3,,,18,,,,,1 <br />
*do,i,1,10 <br />
lesize,20+(i-1)*8,,,20,,,,,1 <br />
*enddo <br />
*do,i,1,10 <br />
lesize,16+(i-1)*8,,,20,,,,,1 <br />
*enddo <br />
&nbsp;&nbsp;<br />
*do,i,1,10 <br />
lesize,18+(i-1)*8,,,20,,,,,1 <br />
*enddo <br />
*do,i,1,10 <br />
lesize,22+(i-1)*8,,,20,,,,,1 <br />
*enddo <br />
&nbsp;&nbsp;<br />
*do,i,1,9 <br />
lesize,17+(i-1)*8,,,18,,,,,1 <br />
*enddo <br />
*do,i,1,9 <br />
lesize,21+(i-1)*8,,,18,,,,,1 <br />
*enddo <br />
&nbsp;&nbsp;<br />
lesize,120,,,12,,,,,1 <br />
lesize,135,,,5,,,,,1 <br />
lesize,136,,,5,,,,,1 <br />
lesize,4,,,2,,,,,1 <br />
&nbsp;&nbsp;<br />
lesize,110,,,12,,,,,1 <br />
lesize,132,,,5,,,,,1 <br />
lesize,131,,,5,,,,,1 <br />
lesize,6,,,2,,,,,1 <br />
&nbsp;&nbsp;<br />
lesize,8,,,20,,,,,1 <br />
lesize,14,,,20,,,,,1 <br />
lesize,99,,,20,,,,,1 <br />
lesize,96,,,20,,,,,1 <br />
lesize,98,,,9,,,,,1 <br />
lesize,97,,,9,,,,,1 <br />
lesize,3,,,9,,,,,1 <br />
lesize,7,,,9,,,,,1 <br />
&nbsp;&nbsp;<br />
lesize,119,,,2,,,,,1 <br />
lesize,121,,,2,,,,,1 <br />
lesize,107,,,2,,,,,1 <br />
lesize,109,,,2,,,,,1 <br />
vsweep,all <br />
&nbsp;&nbsp;<br />
/solu <br />
antype,0 <br />
pstres,on <br />
dl,110,,all <br />
dl,118,,uy <br />
dl,118,,uz <br />
dl,121,,uz <br />
dl,119,,uz <br />
dl,124,,uz <br />
dl,128,,uz <br />
sfa,72,1,pres,-1&nbsp;&nbsp;<br />
solve <br />
finish <br />
&nbsp;&nbsp;<br />
/solu <br />
antype,buckle <br />
bucopt,lanb,1 <br />
mxpand,1 <br />
solve <br />
finish <br />
&nbsp;&nbsp;<br />
/solu <br />
expass,1 <br />
mxpand,1 <br />
outpr,all,all <br />
solve <br />
&nbsp;&nbsp;<br />
/post1 <br />
set,list <br />
set,first <br />
/eshape,1.0 <br />
plnsol,u,sum,2,1 <br />
exit,all <br />
&nbsp;&nbsp;<br />
我到底错在哪里,导致梁上作用均布荷载或纯弯情况下计算结构与理论不苻? <br />
还想问两个具体的问题: <br />
&nbsp;&nbsp;1、用ANSYS实体计算梁的屈曲,如果是简支,约束怎么加才比较准确? <br />
&nbsp;&nbsp;2、我看AYSYS 的一些资料,关于梁的特征值屈曲,都是集中荷载,是不是均布和加弯矩(纯弯情况)的屈曲计算方法不同? <br />
&nbsp;&nbsp;&nbsp;&nbsp;

该用户从未签到

发表于 2007-12-20 01:50:19 |
1。你看加载方式对不对?均布载是否实际加到结构上面去了!~ <br />
2。当结构约束跟理想不同的时候可以适当补充约束,加线约束与节点约束可以分别试试。 <br />
3。你这个是不考虑非线性的弹性屈服极限~!

该用户从未签到

发表于 2007-12-20 22:31:00 |
以下是我个人的观点: <br />
1、你研究的是简支工子钢梁的线性屈曲问题,选取的单元是不是可以采用梁单元,这样建模和计算可能回更快一些,我想结果可能也不会有很大的区别。 <br />
2、如果你要采用实体建模,由于截面不是变截面,采用先建立面,然后拉伸的方法可能也比你的这种方法快。 <br />
3、无论你采用那种单元,约束一定要明确。采用梁单元约束定义就简单多 了。采用实体单元其实也好定义。 <br />
下面我将附上我的命令流

该用户从未签到

发表于 2007-12-21 10:07:06 |
问题出在ANSYS在处理集中荷载时仅考虑stress stiffness,而在处理pressure load时,不仅考虑stress stiffness,而且考虑Pressure Load Stiffness。所以在施加集中荷载后的结果和施加均布荷载的结果有差别,差别在于Pressure Load Stiffness。 <br />
详见: <br />
Pressure Load Stiffness <br />
Quite often concentrated forces are treated numerically by equivalent pressure over a known area. This is especially common in the context of a linear static analysis. However, it is possible that different buckling loads may be predicted from seemingly equivalent pressure and force loads in a eigenvalue buckling analysis. The difference can be attributed to the fact that pressure is considered as a “follower” load. The force on the surface depends on the prescribed pressure magnitude and also on the surface orientation. Concentrated loads are not considered as follower loads. The follower effects is a preload stiffness and plays a significant role in nonlinear and eigenvalue buckling analysis. The follower effects manifest in the form of a “load stiffness matrix” in addition to the normal stress stiffening effects. As with any numerical analysis, it is recommended to use the type of loading which best models the in-service component. <br />
<br />
The effect of change of direction and/or area of an applied pressure is responsible for the pressure load stiffness matrix ([Spr]) (see section 6.5.2 of Bonet and Wood(236)). It is used either for a large deflection analysis (NLGEOM,ON), regardless of the request for stress stiffening (SSTIF command), for an eigenvalue buckling analysis, or for a dynamic analysis that has prestressing flagged (PSTRES,ON command).<br />
<br />
The need of [Spr] is most dramatically seen when modelling the collapse of a ring due to external pressure using eigenvalue buckling. The expected answer is:<br />
<br />
(3

该用户从未签到

发表于 2007-12-22 01:21:13 |
在你的结构使用均布荷载计算屈曲时,可能均布荷载值输入错误。你应该使用sfa,72,1,pres,-1/A,其中A为承受均布荷载的部件面积。 <br />
<br />
至于两端作用弯矩情况,不知你是如何作用的。 <br />
<br />
用ANSYS实体计算梁的屈曲,如果是简支,约束应该加在端面中轴的交点。
 
 
在线客服
在线反馈
工作时间:
8:00-24:00
 

QQ|小黑屋|Archiver|百思 ( 苏ICP备12027101号-1

©2014 百思(Baisi.net)

快速回复 返回顶部 返回列表