问几个LS_DYNA的警告和错误?

Learning_DYNA

仿真一导弹在推力作用下运动，舱段和舱段材料不同。我的模型是平面的，第一次把舱段之间的公共部分共用同一条直线，接触为单面自动，计算没出现问题。但我第二次修改了模型，即公用部分没有用同一条直线，而是用了两条，接触仍为单面自动，但出现了两类错误和警告，如下：
1。 *** Warning Initialization - node will not be moved
   Penetrating node near or at shell mid-surface
   single surface interface # =        1
   penetrating node #         =     1119
   segment #                  =     1175
   penetration                =  0.3363647E+00
   s,t                        =  -0.1000000E+01 -0.1000000E+01
   penetrated segment nodes:
      1332     1333     1334     1331
2。 *** Warning Initialization
   single surface interface # =        1
   penetrating node #         =     7722
   segment #                  =     3643
   penetration                = -0.1319314E+00
   s,t                        =   0.7333374E+00 -0.1000000E+01
   penetrated segment nodes:
      3451     4136     4149     3454
   original coordinates of slave node=    7722
               x-coordinate          = 0.211000004E+02
               y-coordinate          = 0.374076660E+03
               z-coordinate          = 0.000000000E+00
   modified coordinates of slave node=    7722
               x-coordinate          = 0.212319317E+02
               y-coordinate          = 0.374076660E+03
               z-coordinate          = 0.000000000E+00
3。 *** Error negative volume in 2D solid element #    8208 cycle  207893

*** Error negative volume in 2D solid element #    8379 cycle  207893

*** Error negative volume in 2D solid element #    8381 cycle  207893
请问这是什么原因，是接触有问题吗，应用什么类型的接触？还用有什么方面的书籍讲解这些错误和警告的，请推荐，ansys的帮助中好像没有压？

AaronSpark

Warning Initialization
初始化时发现有穿透的情况，你试着把接触实体的初始距离稍稍拉开一点再进行计算。

negative volume
负体积过多造成的，这个原因很多
1.看看材料设置是否有问题
2.变形过大，改变步长看看
3.网格质量太差，重新划分网格

下面再转一篇相关文章

AaronSpark

Negative Volumes in Foams (or other soft materials)
  
In materials that undergo extremely large
deformations, such as soft foams, an element may become so distorted
that the volume of the element is calculated as negative.  This may
occur without the material reaching a failure criterion.  There is
an inherent limit to how much deformation a Lagrangian mesh can
accommodate without some sort of mesh smoothing or remeshing taking
place.  A negative volume calculation in LS-DYNA will cause the
calculation to terminate unless ERODE in *control_timestep is set to 1
in which case the  offending element is deleted and the calculation  
continues.  

Some approaches that can help to overcome negative volumes include the following.
-  Simply stiffen up the material stress-strain curve at large strains.  This  
   approach can be quite effective.  
  
-  Sometimes tailoring the initial mesh to accomodate
   a particular deformation field will prevent formation of negative
   volumes.  Again, negative volumes are generally only an issue for very
   severe deformation problems and typically occur only in soft materials
   like foam.
-  Reduce the timestep scale factor.  The default of 0.9 may not be sufficient to  
   prevent numerical instabilities.
-  Avoid fully-integrated solids (formulations 2 and 3) which tend to be less stable  
   in situations involving large deformation or distortion.  
   Use the default element formulation (1 point solid) with type 5 or 6 hourglass  
   control.  Perhaps as an even better alternatative, model the foam with tetrahedral  
   elements using solid element formulation 10.
-  Increase the DAMP parameter (foam model 57) to the maximum recommended value of 0.5.

-  Use optional card B of *contact to turn shooting node logic off for contacts involving foam.
  
-  Use *contact_interior.  This approach is generally not very effective.
***********************************************************        `
    Version 970 will have improved contact_interior as
    implemented by Dave Benson
***********************************************************

Learning_DYNA

非常感谢楼上的,再问一下,两舱段连接部分直线有重合,是不是就算是初始穿透?应如何该,稍微拉开一点不让重合吗?那与实际情况符合吗?