有关零能模式的问题

kevinansys

这几天在做一个跌落分析,大概是这样的,四个保护钩,然后是10根钢坯从40mm的高度落下，分析出能够承受这冲击载荷的钩子的几何尺寸来．一开始好好的，但我修改了钩子的几何尺寸后，我发现计算中有零能模式出现，后来我对网格加以改进，还有采用了全积分单元，都不行，还是网格变形奇异．由于接触情况比较复杂，我用的是single auto gel，有关的接触常数我也采用默认的，材料模型用的是*mat_plastic_kinematic．
我现在还是怀疑是网格粗细差别太大造成的，可是数次改进了网格还是不行，希望大家集思广义，帮忙看看．
按理说用了全积分单元之后，就不应该会出现零能模式了，真是搞不懂！

kevinansys

这是出现了ZERO-ENERGY MODE后的变形图：

kevinansys

这是一段原先没有出现ZERO-ENERGY MODE的动画：

okan

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.

kevinansys

你给出的办法跟LSTC的理论手册上给出的有关ZERO-ENERGY MODE的解决方法有出入啊,人家说用FULLY-INTEGRATED FORMULATION就可以避免ZERO-ENERGY MODE了,或者是改变BULK VISCOSITY ,OR HOURGLASS COEFFICIENT.
我的分析在前阶段是成功的,并没有出现ZERO-ENERGY MODE;只是我出了另一个方案之后,计算就出现单元的不规则变形了,并且我设置的计算时间是比较短的,大概就是钢坯刚碰撞钩子的时刻,我就不明白为什么前面好好的,到后来计算新的钩子方案时就出现ZERO-ENERGY MODE了呢?

kevinansys

我的问题已经解决了，我调整了一下TSSFAC的值，计算后就没有出现网格的ZIGZAG变形了。在这，我真是要感谢楼上的两位啊，给了我启发。
我觉得问题出在结构上，由于我改变钩子的几何形状，那么整体结构的固有频率也改变了，我看了下LSTC的THEORY MANUAL，里面说LS-DYNA计算得到的TIME STEP SIZE是受结构的固有频率限制的。在我的计算模型中，LS-DYNA计算得到的TIME STEP SIZE导致了数值计算的不稳定，通过降低TSSFAC的数值就可以解决这个问题了。

orwellzeng

采用精确积分就可以了.