请教螺栓预紧力

jdan2002

看了ansys帮助中的例子，计算螺栓预紧力需要添加如下两个命令即可：

psmesh,,example,,volu,1,0,z,0.5,,,,elems

sload,1,9,,force,100,1,2

但是在我的模型中，加入这两个语句，提示出错，预紧力单元没有添加上。

请大家帮忙指点一下，谢谢了！

ps:请问哪本书里有范例哦，之前看见用workbench计算的，我打算还是用命令流，请指点！

jg_meng

不知道什么错误提示，估计是实体编号不对
先看看【psmesh】【SLOAD】对应命令的帮助，使用GUI做一遍，再看看命令，就大概能明白了

586901

PSMESH,1,b1, ,VOLU,2,    0,Z,0.025,b1_2
PSMESH,2,b2, ,VOLU,67,   0,Z,0.025,b2_2

SLOAD,1,9,LOCK,DISP,0.75,1,2
SLOAD,2,9,LOCK,DISP,0.75,1,2

sload,1,9,lock,forc,f,1,2
sload,2,9,lock,forc,f,1,2
你可以参考下这个。

jdan2002

PSMESH,1,b1,,VOLU,34,0,Z,88,b1_2
PSMESH,2,b2,,VOLU,16,0,Z,88,b2_2
PSMESH,3,b3,,VOLU,5,0,Z,88,b3_2
PSMESH,4,b4,,VOLU,66,0,Z,88,b4_2

我添加这4个体积之后，出现了错误，见下图。
这4个体积实际上组成的一个圆柱体，在划分网格的时候被分割开了。请大家帮忙指点一下。
我只运行第一条语句，没有错误，运行第二条的时候就出错了。而且在模型上用cmplot看不到help例子中的被定义为prets179的单元位置，这是为何了？

jdan2002

/prep7
et,1,solid185
mp,ex,1,2.06e11  
mp,prxy,1,0.3
mp,ex,2,0.7e11   
mp,prxy,2,0.3
/pnum,kp,1
/pnum,line,1
/pnue,area,1

block,-7,7,-7,7,74,86.5
wpoff,0,0,70
wpoff,0,0,16.5
cyl4,0,0,4,360,0,0,8
vadd,1,2

wpoff,0,0,-2
cyl4,0,0,2,360,0,0,10
vsbv,3,1
wpoff,0,0,-14.5
cyl4,0,0,3,360,0,0,14.5
vsbv,2,1


allsel
vplot
wpoff,0,0,20
wprota,0,0,90
vsbw,all
vdele,1,,,1
kwpave,12
wprota,0,0,90
vsbw,all
kwpave,7
wprota,0,0,90
wprota,0,-45,0
vsbw,all

kwpave,6
wprota,0,90,0
vsbw,all
wprota,0,-45,0
kwpave,10
wprota,0,90,0
vsbw,all
wpave,0,0,0
wprota,0,-90,90
!加入螺母

cylind,4,5,90,93,-90,90
cylind,4.1,6,86.5,90,-90,90
vglue,2,3,8,1,4,6
wpoff,0,0,90
vsbw,all

accat,79,78
accat,69,68
accat,74,73
accat,83,82
wprota,0,0,90
wprota,0,45,0
kwpave,19
vsbw,11
vsbw,16
kwpave,13
wprota,0,-45,0
wprota,0,-90,0
vsbw,14
vsbw,12
kwpave,40
wprota,0,45,0
vsbw,14
vsbw,16
accat,60,98
accat,101,87
accat,119,115
accat,112,99
accat,98,97
accat,111,101
accat,118,115
accat,112,76

kwpave,30
wprota,0,-45,0
wprota,0,0,90
vsbw,5
vsbw,9
vsbw,10
vsbw,7
accat,21,12
accat,33,8
accat,54,19
accat,42,5
accat,127,23
accat,34,30
accat,135,55
accat,138,44


vsel,s,,,11!螺母
vsel,a,,,15!螺母
vsel,a,,,21!螺母
vsel,a,,,14!螺母
vsel,a,,,13!固定板
vsel,a,,,19!固定板
vsel,a,,,20!固定板
vsel,a,,,12!固定板
mat,1
vmesh,all
allsel

vsel,s,,,1,6,1
vsel,a,,,8,10,1
vsel,a,,,16
vsel,a,,,16,18,1
vsel,a,,,22,25,1
mat,2
vmesh,all
allsel
wpave,0,0,0
wprota,-90,0,90
wprota,0,0,90
wprota,180,0,0

!psmesh,,example,,volu,16,0,z,90,,,,elems
PSMESH,1,b1,,VOLU,3,0,Z,88,b1_2
!PSMESH,2,b2,,VOLU,2,0,Z,88,b2_2 !为何提示有错误
!PSMESH,3,b3,,VOLU,4,0,Z,88,b3_2  !为何提示有错误
!PSMESH,4,b4,,VOLU,1,0,Z,88,b4_2  !为何提示有错误

!CM,lines,LINE
!cmplot

!定义约束
finish
aplot
/solu
flst,2,12,5,orde,12
fitem,2,126
fitem,2,53
fitem,2,131
fitem,2,140
fitem,2,66
fitem,2,35
fitem,2,3
fitem,2,65
fitem,2,84
fitem,2,61
fitem,2,92
fitem,2,85
da,p51x,symm
flst,2,4,5,orde,4
fitem,2,21
fitem,2,33
fitem,2,54
fitem,2,42
!fitem,2,2
!fitem,2,5
da,p51x,all,0

finish
/solu
antype,0
nlgeom,1
nsubst,0
autots,0
time,1
!sload,1,9,,force,100,1,2
sload,1,9,lock,forc,100,1,2
!sload,2,9,lock,forc,100,1,2  !为何提示有错误
!sload,3,9,lock,forc,100,1,2  !为何提示有错误
!sload,4,9,lock,forc,100,1,2  !为何提示有错误
/statue,solu
solve
finish
/post1
/efacet,1
avprin,0
plnsol,s,eqv,0,1


我想定义4个prets179，为何出错了，提示已经存在预紧力单元，估计是体和体之间是相连的，如何解决，谢谢大家帮忙了！

zhangyp

错误说得很清楚，某些单元上的节点又被定义了，这主要是你体是相连的，实际螺栓可不是这样。
可将以下句
PSMESH,1,b1,,VOLU,3,0,Z,88,b1_2
!PSMESH,2,b2,,VOLU,2,0,Z,88,b2_2 !为何提示有错误
!PSMESH,3,b3,,VOLU,4,0,Z,88,b3_2  !为何提示有错误
!PSMESH,4,b4,,VOLU,1,0,Z,88,b4_2  !为何提示有错误
改为：
vsel,s,,,1,4
allsel,below,volume
PSMESH,1,b1,,all,,0,Z,88,,,,b1_2
再采用sload命令定义相同的预紧力即可

jdan2002

首先谢谢zhangyp的热心帮助，上面的问题解决了。

不过目前又遇到新的问题，之前的模型杆与固定板没有vglue，导致以前的分析结果出现杆与固定板分离。

下面是杆、固定板、螺母三者vglue，重新划分了网格。在定义约束时，按照ansys中help的例子，约束了节点20和节点22的自由度，可以得到结果。但是结果不对，因为固定板与杆的接触面上没有应力，这与实际不符。后来采用约束面的自由度，但是无法计算出结果。

请指教，谢谢！

/prep7
et,1,solid185
mp,ex,1,2.06e11  
mp,prxy,1,0.3
mp,ex,2,0.7e11   
mp,prxy,2,0.3
/pnum,kp,1
/pnum,line,1
/pnue,area,1

block,-7,7,-7,7,74,86.5
wpoff,0,0,70
wpoff,0,0,16.5
cyl4,0,0,4,360,0,0,8
vadd,1,2

wpoff,0,0,-2
cyl4,0,0,2,360,0,0,10
vsbv,3,1
wpoff,0,0,-14.5
cyl4,0,0,3,360,0,0,14.5
vsbv,2,1


allsel
vplot
wpoff,0,0,20
wprota,0,0,90
vsbw,all
vdele,1,,,1
kwpave,12
wprota,0,0,90
vsbw,all
kwpave,7
wprota,0,0,90
wprota,0,-45,0
vsbw,all

kwpave,6
wprota,0,90,0
vsbw,all
wprota,0,-45,0
kwpave,10
wprota,0,90,0
vsbw,all
wpave,0,0,0
wprota,0,-90,90
!加入螺母

cylind,4,5,90,93,-90,90
cylind,4.1,6,86.5,90,-90,90
!vglue,2,3,8,1,4,6
vglue,all
wpoff,0,0,90
vsbw,all

accat,79,78
accat,69,70
accat,74,75
accat,65,64
wprota,0,0,90
wprota,0,45,0
kwpave,19
vsbw,15
vsbw,16
kwpave,13
wprota,0,-45,0
wprota,0,-90,0
vsbw,10
vsbw,12
kwpave,40
wprota,0,45,0
vsbw,14
vsbw,15
accat,59,58
accat,107,92
accat,116,84
accat,121,119
accat,59,40
accat,107,61
accat,121,111
accat,124,116

kwpave,30
wprota,0,-45,0
wprota,0,0,90
vsbw,19
vsbw,18
vsbw,20
vsbw,17
adrag,145,148,152,142,,,209
vsba,22,29
vsba,23,96
vsba,24,145
vsba,25,146
accat,103,87
accat,88,98
accat,89,106
accat,86,95
accat,12,102
accat,99,8
accat,19,105
accat,5,94

accat,139,156
accat,154,104
accat,131,136
accat,150,147


accat,44,156
accat,154,55
accat,34,136
accat,150,23


vsel,s,,,9!螺母
vsel,a,,,13!螺母
vsel,a,,,16!螺母
vsel,a,,,12!螺母
vsel,a,,,11!固定板
vsel,a,,,10!固定板
vsel,a,,,14!固定板
vsel,a,,,21!固定板
mat,1
vmesh,all
allsel

vsel,s,,,1,8,1
vsel,a,,,15
vsel,a,,,17,20,1
vsel,a,,,22,24,1
vsel,a,,,26,29,1
mat,2
vmesh,all
allsel
wpave,0,0,0
wprota,-90,0,90
wprota,0,0,90
wprota,180,0,0

!psmesh,,example,,volu,16,0,z,90,,,,elems
!PSMESH,1,b1,,VOLU,3,0,Z,88,b1_2
!PSMESH,2,b2,,VOLU,2,0,Z,88,b2_2 !为何提示有错误
!PSMESH,3,b3,,VOLU,4,0,Z,88,b3_2  !为何提示有错误
!PSMESH,4,b4,,VOLU,1,0,Z,88,b4_2  !为何提示有错误
vsel,s,,,1,4
allsel,below,volume
PSMESH,1,b1,,all,,0,Z,88,,,,b1_2

!CM,lines,LINE
!cmplot

!定义约束
finish
aplot
/solu
flst,2,14,5,orde,14
fitem,2,130
fitem,2,97
fitem,2,148
fitem,2,141
fitem,2,151
fitem,2,157
fitem,2,90
fitem,2,91
fitem,2,15
fitem,2,3
fitem,2,81
fitem,2,82
fitem,2,39
fitem,2,52
da,p51x,symm
allsel

dk,20,ux
dk,22,ux
dk,20,uz
dk,20,uy
dk,22,uy

!flst,2,4,5,orde,4
!fitem,2,171
!fitem,2,170
!fitem,2,169
!fitem,2,168

!da,p51x,all,0

!flst,2,4,5,orde,4
!fitem,2,14
!fitem,2,18
!fitem,2,28
!fitem,2,32
!da,p51x,ux,0
!flst,2,4,5,orde,4
!fitem,2,14
!fitem,2,18
!fitem,2,28
!fitem,2,32
!da,p51x,uy,0

!finish
/solu

sload,1,9,,force,100,1,2
solve
finish
/post1
/efacet,1
avprin,0
plnsol,s,eqv,0,1

lliuzhicun2002

做接触绑定

jdan2002

是不是在固定板与螺母以及固定板与杆的接触面定义接触约束啊

但是ansys的help中没有定义接触也可以计算啊，请大家帮忙指点，谢谢了！

jdan2002

请大家帮忙看一看如何定义约束，是定义点的约束了，还是可以定义面的约束(见上面的命令流)？

djd852

收藏了，以后学习！

NWPYANG

正在学习使用这个，谢谢