请帮我看看桩土接触不收敛的原因!!!有命令流

xuebaoak47

我做的问题是，一根单桩的桩土接触模拟分析，目的是研究这种桩型的力学特征，土体一共有5层，桩长15m，做了5个接触对，每层土做一个，考虑重力的影响，取了四分之一的模型建模！！！

但是我在计算求解的时候总是不收敛，而且有提示说有多少个小的矩阵方程求解失败！！

我马上就毕业了，很着急，希望各位朋友能帮我分析一下到底是哪里出的问题！！！！

AaronSpark

运行了10分钟你的命令流，没有出现错误或者什么提示，后来关闭了

什么是小的矩阵方程？是不是出现小主元？关于小主元问题我专篇帖子你看看

问题的前面讨论有很多
   小弟在静态、瞬态分析中，经常遇到
   There are n small equation solver pivot terms 小主元错误
小主元错误系数矩阵欠秩，系数矩阵欠秩意味着结构约束不足，源于矩阵奇异导致，一般是约束出了问题，出现了整体的刚体位移。刚度矩阵为半正定。
   出现小主元
   说明结构的切线刚度矩阵|Kt|=0
   如果出现的小主元不多，说明可能是达到某个临界点，以后还可以继续求下去，
   分支点稳定里经常有这种情况，比如受压薄板，固接扁拱
   如果出现的小主元很多了，而且越来越多，就说明这个结构要坏了，比如出现大面积的塑性区
   形成多个塑性铰等
   （参考sunny兄的解释）
     Small Pivot Terms

The term 'pivot' refers to the first non-zero term in the matrix when one is performing Gaussian elimination to upper-triangularize the matrix before finding the displacement vector by back-substitution. These concepts are most applicable to use of the frontal solver. Typically, the matrix being solved is the stiffness matrix. Consider, for example, a simple 1-d element with two nodes, x1 and x2. If the model is unconstrained, ANSYS will attempt to write two equations: k(x1-x2) = 0
k(x2-x1) = 0 ANSYS tries to solve for these two equations and two unknowns by subtracting one equation from the other. However, you can quickly see that this technique won't work because the two equations are not independent, meaning that for any value of x1=x2, the equations are satisfied. In matrix manipulation space, ANSYS ends up with the following: | k -k | x1 = | 0 |
| -k k | x2 = | 0 | Using Gaussian elimination: | k -k | x1 = | 0 |
| 0 0 | x2 = | 0 | The second '0' that I've underlined is the 'pivot'. The zero pivot here means that you have made ANSYS write more equations than can be solve deterministically. The mathematical term for this is that the matrix failed to be "positive definite." The practical upshot is that zero pivots always are caused by unconstrained problems. The "small pivot" problem comes from the fact that computers don't give zero when doing subtraction using real variables. Instead, you get values like 1e-20, or even -1e-20. Hence, poorly constrained problems will tend to lead to exceedingly small pivots, near the roundoff level for the machine. To the best of my knowledge, there is no significance to whether these small pivots are negative or positive, although ANSYS will sometimes tell you that you have a "negative pivot," rather than a "small pivot." They both indicate the same problem. Lastly, when you have a big stiffness difference between adjacent elements, poor constraint can result from asking ANSYS to do Gaussian elimination that causes it to calculated small differences between large numbers. In this case, you start to lose accuracy as the pivot gets to be very close to the roundoff error of the computer. This is why ANSYS will also complain about stiffness matrix ratios that exceed 1e8. What do you do to figure out what is going on? One answer is to do a modal analysis and see what part goes flying off at near zero frequency. I try to think about where the offending dof is in the model and try to visualize that part of the model moving as a rigid body. In your case, however, I believe the problem is poor element choice. Someone may correct me on this, but I believe that the SOLID72's are your problem. If you read the fine manual regarding this element, you will note the following little gotcha: "Do not apply nodal forces or nodal moments, due to theoretical limitations of this element." You see, SOLID72 rotational degrees of freedom are not "real," as has been discussed on this list in relation to its full-blown cousin SOLID73. They are a poor- mans approximation to the SOLID92 element, and have been proposed to be eliminated because they set just the type of trap that you are apparently falling into. The conventional techniques for reacting beam and shell moments in solids include: - bury the beam/shell one row deep into the solid
- make a tee out of the beam/shell and overlay on the solid face
- write constraint equations General purpose SOLID92's are then your best bet, in conjunction with these techniques.


  该类问题的解决方法：
       1。检查边界约束
       2、模型是否存在较大刚度突变
       3、材料属性、约束情况、荷载等改变是否合理
       4、更换相近单元试试
       5、最好不要采用稀疏求解器

   但是对于小主元对问题求解结果的精度影响，一直没有人作讨论，在作高层钢结构弹塑性时程分析时，这个问题好像难以避免，特别是结构进入塑性后，对于这类结果的取舍有待进一步讨论。
   小弟这里抛块砖，备了个筐，各位大侠，有玉的都砸过来。

来自傲雪

yangdong28

2楼的很有理论水平，就我个人的一点点经验说说：
我在算固接实体拱时用了solid65单元，出现过上面的问题，我的办法是：
1。检查模型，GLUE和合并压缩结点单元号，解决可能在切割分块后单元的连接问题，同时检查约束；
2。先把网格划的粗些，节省计算时间，看看还出现“There are n small equation solver pivot terms ”；
3。调整收敛容差，把它变得宽松些；
4。还有就是把荷载水平降低些，按2楼的说法可能会避免出现塑性；
5。如果可以调整得收敛，再逐步细化单元、加大荷载、把容差收紧。
试试或许有用,不知大家在实际操作时的办法，交流一下吧！