【求助】请教如何将总刚度矩阵导出？

大头

在ansys5.7或者6.1下有没有相关的命令，将总刚度矩阵和外载荷以文件形式导出？

cswbww

不知道楼上的兄弟是什么意思，如果有可能能不能将详细做法告知。
  
在国外论坛，也有人这么问。我大概归纳了一下。
1。对ansys的文件扩展名有所了解，什么是.emat,.tri等等。
2。用psolve命令
     elform可以形成.emat（单元矩阵）
     elprep形成.erot
     triang形成.tri（刚度矩阵）
3。运用binlib将.tri的二进制文件转化为可以用.txt，详情参照
     http://www.cesup.ufrgs.br/ansys/prog_55/g-int/INS2.htm
  
或者你用别的软件，文献说用matlab可以做到；还有用c++和fortran的。可以直接从.full文件里面读出刚度矩阵和质量矩阵，具体做了才知道，我没有compaq visual fortran：（

cswbww

我找到了二楼兄弟说的substructure的意思了，不过是在一个大学的网页里，原文如下：
  
You can list all components of the global stiffness matrix in ANSYS by converting your model into a "super element". To do this:
1. Build your model normally. You do not need to apply any boundary conditions.
2. In the solution processor choose the Analysis Type to be substructuring (Solu -> New Analysis -> Substructuring).  
3. Select Solu -> Analysis Options and give your substructure a name (defaults to the jobname) and select the Matrix to be generated to be the Stiffness Matrix. Click OK.
4. Next you need to define the master DOF. Master DOFs are all DOFs that will be considered when assembling the global stiffness matrix. Since you want all components of the matrix just define all DOFs to be master DOF: Solu -> Master DOFs -> Define -> Pick All -> All DOF -> OK.  
4. Solve the Problem: Solu -> Solve LS. ANSYS will compute the solution and write the global stiffness matrix into a new file called "name.sub" (name being whatever name you defined in step 3). Do not delete this file. You will need it to later if you want to relist the global stiffness matrix.
5. Click: UM -> List -> Other -> Superelement Data. Set name to the name of your *.sub file, the name you defined in step 3, and set KOPT = Full Contents, then click OK.
6. ANSYS will list all the superelement data. The beginning is just a bunch of header information you do not have to worry about. Scroll down to: GLOBAL DOF SET NODES, LABELS = . Next ANSYS lists the order of the DOF vector for your global stiffness matrix. For example:
  
GLOBAL DOF SET NODES, LABELS =
1 UX 1 UY 2 UX 2 UY 3 UX
3 UY 4 UX 4 UY  
  
This means that in the subsequent matrix the 1st row and 1st column are associated with the DOF UX at node 1, 2nd is UY1, 3rd UX2, etc. Then follows the listing of the stiffness matrix, e.g.:
  
ROW 1 MATRIX 1
103846.15 37500.000 -63461.538 -2884.6154 -51923.077
-37500.000 11538.462 2884.6154  
  
ROW 2 MATRIX 1
37500.000 103846.15 2884.6154 11538.462 -37500.000
-51923.077 -2884.6154 -63461.538  
  
etc.
  
Here, ROW 1 lists the elements of the first row of the stiffness matrix, i.e., K11=103846.15, K12=37500.00, K13=-62461.538, etc

edodo

唉！！！
大家好好看看我们这个版的置顶!!
以后不许再出现这类问！
以后建议大家都看看精华区

cat_Tom

edodo 说得不对!
我非常感谢此贴!
精华版的我看了,但除了给了我一个看不懂的程序外,一无所获.况且无compaq fortran 6.5,无法利用.
而cswbww的回答使我知道程序的来龙去脉,就可自己编程序了.
建议斑竹将此贴并入精华版相应贴中并随时更新!