ANSYS中upcoord与upgeom的用法 - 小众知识

ANSYS中upcoord与upgeom的用法

2013年01月27日 14:18:05 苏内容
  标签: ANSYS
阅读:226
ANSYS中upcoord与upgeom的用法(gch原创).
Ansys中upcoord与upgeom都是更新节点位移的命令。下面将针对二者的用法进行讲解。
一、UPCOORD与UPGEOM命令简介
UPCOORD:
帮助文件中是这么介绍的:UPCOORD
UPCOORD, FACTOR, Key
Modifies the coordinates of the active set of nodes, based on the current displacements.
FACTOR
Scale factor for displacements being added to nodal coordinates. If FACTOR = 1.0, the full displacement value will be added to each node, 0.5, half the displacement value will be added, etc. If FACTOR = -1, the full displacement value will be subtracted from each node, etc.
Key
Key for zeroing displacements in the database:
OFF — Do not zero the displacements (default).
ON — Zero the displacements.
FACTOR代表要使用上步结果位移的倍数,现有坐标=等于建模时的坐标+FACTOR*上一步计算的位移
Key代表是否将位移设置为0
UPGEOM:
帮助文件:UPGEOM
UPGEOM:
UPGEOM, FACTOR, LSTEP, SBSTEP, Fname, Ext, --
Adds displacements from a previous analysis and updates the geometry of the finite element model to the deformed configuration.
FACTOR
Multiplier for displacements being added to coordinates. The value 1.0 will add the full value of the displacements to the geometry of the finite element model. Defaults to 1.0.
LSTEP
Load step number of data to be imported. Defaults to the last load step.
SBSTEP
Substep number of data to be imported. Defaults to the last substep.
Fname
File name and directory path (248 characters maximum, including the characters needed for the directory path). An unspecified directory path defaults to the working directory; in this case, you can use all 248 characters for the file name.
The field must be input (no default).
Ext
Filename extension (eight-character maximum).
The extension must be an RST extension.
-- Unused field.
UPGEOM命令是根据文件中的结果进行读取的,可以应用某一步或者某一子步的结果。
二者异同:
UPCOORD, FACTOR, Key-命令是仅仅更新了结构的有限元模型而并不更新其计算结果文件,发出该命令后进行下一步有限元求解时ANSYS将重新计算其刚度矩阵后求解。
UPGEOM, FACTOR, LSTEP, SBSTEP, Fname, Ext, -- — 将分析所得的位移加到有限元模型的节点上,并更新有限元模型的几何形状。
upcoord根据当前DB数据库数据更改节点坐标
upgeom根据RST结果数据文件更改节点坐标
二、部分问题。
1、首先了解UPCOORD中Key的作用,下面以一个例子说明问题。
例1
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,11,FY,-1            ! Unit load at free end
SOLVE
upcoord,0.1,on    
F,11,FY,-1
Solve
当Key为on时,得到以下位移数据。
建模时的节点坐标
NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     10.0000000000     0.00000000000  
       3    0.00000000000     20.0000000000     0.00000000000  
       4    0.00000000000     30.0000000000     0.00000000000  
       5    0.00000000000     40.0000000000     0.00000000000  
       6    0.00000000000     50.0000000000     0.00000000000  
       7    0.00000000000     60.0000000000     0.00000000000  
       8    0.00000000000     70.0000000000     0.00000000000  
       9    0.00000000000     80.0000000000     0.00000000000  
      10    0.00000000000     90.0000000000     0.00000000000  
      11    0.00000000000     100.000000000     0.00000000000  
计算得到的节点位移
NODE    UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
Upcoord之后的节点坐标
  NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     9.99999986667     0.00000000000  
       3    0.00000000000     19.9999997333     0.00000000000  
       4    0.00000000000     29.9999996000     0.00000000000  
       5    0.00000000000     39.9999994667     0.00000000000  
       6    0.00000000000     49.9999993333     0.00000000000  
       7    0.00000000000     59.9999992000     0.00000000000  
       8    0.00000000000     69.9999990667     0.00000000000  
       9    0.00000000000     79.9999989333     0.00000000000  
      10    0.00000000000     89.9999988000     0.00000000000  
      11    0.00000000000     99.9999986667     0.00000000000  
再次加同样的荷载计算后的结果
NODE    UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
如果再次Upcoord之后的节点坐标
  NODE      X             Y              Z
      1    0.00000000000     0.00000000000     0.00000000000  
      2    0.00000000000     9.99999973333     0.00000000000  
      3    0.00000000000     19.9999994667     0.00000000000  
      4    0.00000000000     29.9999992000     0.00000000000  
      5    0.00000000000     39.9999989333     0.00000000000  
      6    0.00000000000     49.9999986667     0.00000000000  
      7    0.00000000000     59.9999984000     0.00000000000  
      8    0.00000000000     69.9999981333     0.00000000000  
      9    0.00000000000     79.9999978667     0.00000000000  
     10    0.00000000000     89.9999976000     0.00000000000  
     11    0.00000000000     99.9999973333     0.00000000000  
当Key为off时,得到以下位移数据。
建模时的节点坐标
NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     10.0000000000     0.00000000000  
       3    0.00000000000     20.0000000000     0.00000000000  
       4    0.00000000000     30.0000000000     0.00000000000  
       5    0.00000000000     40.0000000000     0.00000000000  
       6    0.00000000000     50.0000000000     0.00000000000  
       7    0.00000000000     60.0000000000     0.00000000000  
       8    0.00000000000     70.0000000000     0.00000000000  
       9    0.00000000000     80.0000000000     0.00000000000  
      10    0.00000000000     90.0000000000     0.00000000000  
      11    0.00000000000     100.000000000     0.00000000000  
计算得到的节点位移
NODE    UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
Upcoord之后的节点坐标
  NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     9.99999986667     0.00000000000  
       3    0.00000000000     19.9999997333     0.00000000000  
       4    0.00000000000     29.9999996000     0.00000000000  
       5    0.00000000000     39.9999994667     0.00000000000  
       6    0.00000000000     49.9999993333     0.00000000000  
       7    0.00000000000     59.9999992000     0.00000000000  
       8    0.00000000000     69.9999990667     0.00000000000  
       9    0.00000000000     79.9999989333     0.00000000000  
      10    0.00000000000     89.9999988000     0.00000000000  
      11    0.00000000000     99.9999986667     0.00000000000  
再次加同样的荷载计算后的结果
   NODE     UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
如果再次Upcoord之后的节点坐标
  NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     9.99999973333     0.00000000000  
       3    0.00000000000     19.9999994667     0.00000000000  
       4    0.00000000000     29.9999992000     0.00000000000  
       5    0.00000000000     39.9999989333     0.00000000000  
       6    0.00000000000     49.9999986667     0.00000000000  
       7    0.00000000000     59.9999984000     0.00000000000  
       8    0.00000000000     69.9999981333     0.00000000000  
       9    0.00000000000     79.9999978667     0.00000000000  
      10    0.00000000000     89.9999976000     0.00000000000  
      11    0.00000000000     99.9999973333     0.00000000000  
在没有第二次之前,当使用upcoord,0.1,on之后,查看位移结果得到
  NODE    UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000    0.0000    0.0000    0.0000  
      3  0.0000    0.0000    0.0000    0.0000  
      4  0.0000    0.0000    0.0000    0.0000  
      5  0.0000    0.0000    0.0000    0.0000  
      6  0.0000    0.0000    0.0000    0.0000  
      7  0.0000    0.0000    0.0000    0.0000  
      8  0.0000    0.0000    0.0000    0.0000  
      9  0.0000    0.0000    0.0000    0.0000  
     10  0.0000    0.0000    0.0000    0.0000  
     11  0.0000    0.0000    0.0000    0.0000  
可见位移清零了。
相反,在没有第二次之前,当使用upcoord,0.1,off之后,查看位移结果得到
   NODE     UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
可见仍然是保持着计算的结果。
虽然on和off之后,没再计算之前,二者位移结果不一样,但是其他结果是一样的。
如果取节点位移改变后的节点坐标重新建模进行计算,得到结果
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
可以发现与上述结果是一样的。位移还没变呢?可以通过提取刚度矩阵的方法去看,当荷载加大倍数前后提取整体刚度矩阵,
例2
无UPCOORD命令流
fini
/cle
/PREP7
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/solu
antype,7 !substructuring分析类型
seopt,matname,2   !设置文件名称和刚度矩阵类型(刚度,质量,阻尼等)
nsel,all   !选择所有节点
m,all,all    !定义所有节点自由度为主自由度
solve   !求解
selist,matname,3    !列出整体刚度矩阵
得到结果:
   1874.9880      0.0000000    -9374.9400    -1874.9880     0.0000000    -9374.9400  
   0.0000000      750000.00     0.0000000      0.0000000    -750000.00    0.0000000  
  -9374.9400     0.0000000      62499.600     9374.9400      0.0000000    31249.800  
  -1874.9880     0.0000000      9374.9400     1874.9880      0.0000000    9374.9400  
   0.0000000     -750000.00     0.0000000      0.0000000     750000.00     0.0000000  
  -9374.9400     0.0000000      31249.800     9374.9400      0.0000000    62499.600
例3
UPCOORD命令流
fini
/cle
/PREP7
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,2,FY,-100000          ! Unit load at free end
SOLVE
save
finish
/prep7
upcoord,0.1,on
finish
/solu
antype,7 !substructuring分析类型
seopt,matname,2   !设置文件名称和刚度矩阵类型(刚度,质量,阻尼等)
nsel,all   !选择所有节点
m,all,all    !定义所有节点自由度为主自由度
solve   !求解
selist,matname,3    !列出整体刚度矩阵
得到刚度矩阵:
   1882.5080      0.0000000     9399.9899   
   0.0000000      751001.34     0.0000000   
   9399.9899      0.0000000     62583.044  
由于6*6的刚度(无upgeom)矩阵中包含了非位移刚度,beam3是二维梁单元。去掉与4,5,6自由度有关的也可以得到一个3*3(upgeom)的矩阵。而且经过查看,6*6的刚度矩阵(无upgeom)节点顺序是1至2,而3*3的矩阵(upgeom)是2至1,导致了矩阵13和31项(矩阵中的9374.9402)符号相反。调整至节点顺序1至2可得
无upcoord
1874.9880     0.0000000     -9374.9400
0.0000000     750000.00      0.0000000
-9374.9400     0.0000000      62499.600
Upcoord之后
   1882.5080      0.0000000     9399.9899   
   0.0000000      751001.34     0.0000000   
   9399.9899      0.0000000     62583.044  
经过对比发现,刚度矩阵是变化的。命令流如下:
/solu
antype,7 !substructuring分析类型
seopt,matname,2   !设置文件名称和刚度矩阵类型(刚度,质量,阻尼等)
nsel,all   !选择所有节点
m,all,all    !定义所有节点自由度为主自由度
solve   !求解
selist,matname,3    !列出整体刚度矩阵
!以上程序用于整体矩阵的提取,下面是关于单元质量和刚度矩阵的提取:
/OUTPUT,cp,out,, ! 将输出信息送到cp.out文件
/debug,-1,,,1 ! 指定输出单元矩阵
/SOLU
SOLVE
finish
2、UPGEOM与upcoord出现不同结果
使用如下命令
例4
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,11,FY,-1          ! Unit load at free end
SOLVE
save
/prep7
upgeom,1,,,file,rst
/SOLU
Solve
第一次solve之后,得到位移结果
   NODE     UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
在第二次solve之前,upgeom之后,得到节点坐标如下
  NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     9.99999986667     0.00000000000  
       3    0.00000000000     19.9999997333     0.00000000000  
       4    0.00000000000     29.9999996000     0.00000000000  
       5    0.00000000000     39.9999994667     0.00000000000  
       6    0.00000000000     49.9999993333     0.00000000000  
       7    0.00000000000     59.9999992000     0.00000000000  
       8    0.00000000000     69.9999990667     0.00000000000  
       9    0.00000000000     79.9999989333     0.00000000000  
      10    0.00000000000     89.9999988000     0.00000000000  
     11    0.00000000000     99.9999986667     0.00000000000可
第二次solve之后得到位移结果
   NODE     UX       UY        UZ        USUM  
      1  0.0000    0.0000    0.0000    0.0000  
      2  0.0000   -0.13333E-05  0.0000    0.13333E-05
      3  0.0000   -0.26667E-05  0.0000    0.26667E-05
      4  0.0000   -0.40000E-05  0.0000    0.40000E-05
      5  0.0000   -0.53333E-05  0.0000    0.53333E-05
      6  0.0000   -0.66667E-05  0.0000    0.66667E-05
      7  0.0000   -0.80000E-05  0.0000    0.80000E-05
      8  0.0000   -0.93333E-05  0.0000    0.93333E-05
      9  0.0000   -0.10667E-04  0.0000    0.10667E-04
     10  0.0000   -0.12000E-04  0.0000    0.12000E-04
     11  0.0000   -0.13333E-04  0.0000    0.13333E-04
再次upgeom之后查看节点坐标
  NODE      X             Y              Z
       1    0.00000000000     0.00000000000     0.00000000000  
       2    0.00000000000     9.99999973333     0.00000000000  
       3    0.00000000000     19.9999994667     0.00000000000  
       4    0.00000000000     29.9999992000     0.00000000000  
       5    0.00000000000     39.9999989333     0.00000000000  
       6    0.00000000000     49.9999986667     0.00000000000  
       7    0.00000000000     59.9999984000     0.00000000000  
       8    0.00000000000     69.9999981333     0.00000000000  
       9    0.00000000000     79.9999978667     0.00000000000  
      10    0.00000000000     89.9999976000     0.00000000000  
      11    0.00000000000     99.9999973333     0.00000000000  
可见二者得到的结果完全一致。
下面建立一个简单的模型输出总纲矩阵进行对比。命令流如下
例5
fini
/cle
/PREP7
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/solu
antype,7 !substructuring分析类型
seopt,matname,2   !设置文件名称和刚度矩阵类型(刚度,质量,阻尼等)
nsel,all   !选择所有节点
m,all,all    !定义所有节点自由度为主自由度
solve   !求解
selist,matname,3    !列出整体刚度矩阵
得到结果:
   1874.9880      0.0000000    -9374.9400    -1874.9880     0.0000000    -9374.9400  
   0.0000000      750000.00     0.0000000      0.0000000    -750000.00    0.0000000  
  -9374.9400     0.0000000      62499.600     9374.9400      0.0000000    31249.800  
  -1874.9880     0.0000000      9374.9400     1874.9880      0.0000000    9374.9400  
   0.0000000     -750000.00     0.0000000      0.0000000     750000.00     0.0000000  
  -9374.9400     0.0000000      31249.800     9374.9400      0.0000000    62499.600
使用UPGEOM之后,命令流如下:
例6
fini
/cle
/PREP7
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,2,FY,-100000          ! Unit load at free end
SOLVE
save
finish
/prep7
upgeom,0.1,,,file,rst
finish
/solu
antype,7 !substructuring分析类型
seopt,matname,2   !设置文件名称和刚度矩阵类型(刚度,质量,阻尼等)
nsel,all   !选择所有节点
m,all,all    !定义所有节点自由度为主自由度
solve   !求解
selist,matname,3    !列出整体刚度矩阵
得到矩阵为3*3的,只有线位移,没有角位移。
   1882.5080      0.0000000     9399.9899   
   0.0000000      751001.34     0.0000000   
   9399.9899      0.0000000     62583.044   
由于6*6的刚度(无upgeom)矩阵中包含了非位移刚度,beam3是二维梁单元。去掉与4,5,6自由度有关的也可以得到一个3*3(upgeom)的矩阵。而且经过查看,6*6的刚度矩阵(无upgeom)节点顺序是1至2,而3*3的矩阵(upgeom)是2至1,导致了矩阵13和31项(矩阵中的9374.9402)符号相反。调整至节点顺序1至2可得
无upgeom
1874.9880     0.0000000     -9374.9400
0.0000000     750000.00      0.0000000
-9374.9400     0.0000000      62499.600
Upgeom之后
1882.5080     0.0000000      9399.9899  
0.0000000     751001.34      0.0000000  
9399.9899     0.0000000      62583.044  
可见Upgeom改变了结构刚度,而且改变的刚度是一样的。 计不计算预应力效应的结果是一样的。
对于一根梁单元,Upgeom之后位移有了改变
例7
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,2,FY,-1e6          ! Unit load at free end
SOLVE
save
finish
/prep7
upgeom,0.1,,,file,rst
finish
/SOLU
Solve
第1个solve之后得到的节点的位移为
   NODE     UY  
      1  0.0000  
     2  -1.3333  
第2个solve之后得到的节点的位移为
   NODE     UY  
      1  0.0000  
     2  -1.3156
可见,刚度矩阵得到了改变。
对于upcoord命令,
例8
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,2,,10
E,1,2
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,2,FY,-1e6          ! Unit load at free end
SOLVE
save
finish
/prep7
upcoord,0.1,off
finish
/SOLU
Solve
得到节点位移结果
   NODE     UY  
      1  0.0000  
     2  -1.3156
而且无论Key是on或者off,都得到一样的结果,说明upcoord和upgeom都能改变结构刚度矩阵。但是为什么上次多根梁单元的结果判定不一致呢。做尝试时有一个发现。就是upcoord与upgeom在那个模块操作的问题,是/prep7,/solu,/post1,在/prep7,/post1都能得到刚度矩阵的改变,而/solu则不行。
(1)/prep7 upcoord,0.1,on
例9
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,11,FY,-1e6            ! Unit load at free end
SOLVE
/prep7
upcoord,0.1,on
/solu
F,11,FY,-1e6
solve
节点位移:
   NODE     UY  
      1  0.0000  
     2  -1.3156  
     3  -2.6311  
     4  -3.9467  
     5  -5.2622  
     6  -6.5778  
     7  -7.8933  
     8  -9.2089  
     9  -10.524  
     10  -11.840  
     11  -13.156
(2)/prep7 upcoord,0.1,off
例10
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,11,FY,-1e6            ! Unit load at free end
SOLVE
/prep7
upcoord,0.1,off
/solu
F,11,FY,-1e6
solve
节点位移:
   NODE     UY  
     1   0.0000  
     2  -1.3156  
     3  -2.6311  
     4  -3.9467  
     5  -5.2622  
     6  -6.5778  
     7  -7.8933  
     8  -9.2089  
     9  -10.524  
    10  -11.840  
    11  -13.156
(3)/prep7  upgeom,0.1,,,file,rst
例11
fini
/cle
/PREP7
/TITLE, BUCKLING OF A BAR WITH HINGED SOLVES
ET,1,BEAM3
R,1,.25,52083E-7,.5
MP,EX,1,30E6
mp,prxy,1,0.3
N,1
N,11,,100
FILL
E,1,2
EGEN,10,1,1
FINISH
/SOLU
ANTYPE,STATIC          ! Static analysis
PSTRES,ON            ! Calculate prestress effects
D,1,ALL
F,11,FY,-1          ! Unit load at free end
SOLVE
save
finish
/prep7
upgeom,0.1,,,file,rst
finish
/SOLU
Solve
节点位移结果
   NODE     UY  
      1  0.0000  
     2  -1.3156  
     3  -2.6311  
     4  -3.9467  
     5  -5.2622  
     6  -6.5778  
     7  -7.8933  
     8  -9.2089  
     9  -10.524  
     10  -11.840  
     11  -13.156
与为改变坐标之前的结果相比较
   NODE     UY  
      1  0.0000  
     2  -1.3333  
     3  -2.6667  
     4  -4.0000  
     5  -5.3333  
     6  -6.6667  
     7  -8.0000  
     8  -9.3333  
     9  -10.667  
     10  -12.000  
     11  -13.333  
显然有了改变。再次证明了upcoord和upgeom都有改变结构刚度矩阵的效果。而且在upgeom之后,没有solve之前查看不到上次计算的应力结果,只有位移结果了。
总结
经过以上验证,得出如下结论:
(1)upcoord和upgeom都有改变结构刚度矩阵的效果,其实也不难想象,ansys既然有这么个功能,节点坐标变了,刚度矩阵应随着改变。但是软件归软件,并不是什么情况下都能正确执行命令。同样是upcoord和upgeom命令,但是在不同的处理器当中却呈现出不同的效果,只有不在/solu 中使用这两个命令再能达到更新刚度矩阵的效果。所以操作对了并不等于结果对了,所谓尽信书不如无书,多怀疑多讨论还是有利于判断结果的。
(2)upcoord和upgeom只是改变节点坐标,并没有预应力的效果。
(3)upcoord中Key的on和off只影响上一步solve之后的位移结果,并不改变其他结果。Off之后的唯一结果与upcoord之前的solve结果的位移是一致的。而on(清零)之后,位移结果清零了,而其他结果一直存在。
(4)upgeom之后,第二次solve之前查看不到上次solve的应力结果,只有位移结果。
(5)upcoord和upgeom均可以应用到非线性屈曲当中去,增加初始缺陷。
以上结果纯属个人意见,欢迎各位批评指正。
扩展阅读
© CopyRight 2010-2021, PREDREAM.ORG, Inc.All Rights Reserved. 京ICP备13045924号-1