ANSYS/LSDYNA负体积 速度过大

Question

#学渣求助帖#我的Ansys/LS-DYNA的求解过程又出了问题。私人电脑算报错的原因是节点速度过大（node has out-of-range velocities）工作站报错的原因是单元里面有负体积（negative volumn）。私人电脑4核的预计完成时间（estimated clock time）只有13h，用工作站8核的预计完成时间是1100h。现在已经排查了以下原因：1、结构网格疏密问题2、材料参数问题3、timestep大小问题4、接触用的是通用接触5、固体结构用的是constant stress solid element,炸药和空气用的1point ALE multi-material element大牛们有没有觉得哪里出了问题...

Answer 1

用得什么材料模型？我之前也出现过。
以下是官方的说法，材料属性和网格划分都会导致负体积的出现。希望能帮助到你。
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 and DTMIN in *control_termination is set to any nonzero value in which case the offending element is deleted and the calculation continues (in most cases). Even with ERODE and DTMIN set as described, a negative volume may cause an error termination (see erode/negvol.k). 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. (The fully integrated element is less robust than a 1-point element when deformation is large because a negative Jacobian can occur at one of the integration points while the element as a whole maintains a positive volume. The calculation with fully integrated element will therefore terminate with a negative Jacobian much sooner than will a 1-point element. (lpb))
- Use the default element formulation (1 point solid) with type 4 or 5 hourglass control (will stiffen response). Preferred hourglass formulations for foams are:type 6 with coef. = 1.0 if low velocity impact types 2 or 3 if high velcocityimpact
- Model the foam with tetrahedral elements using solid element formulation 10 (see ~pdf/dubois-foam-tets.pdf).
- 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.
A part set defines the parts to be treated by contact_interior. Attribute 4 (DA4 = 5th field of Card 1) of the part set defines the TYPE of contact_interior used. The default TYPE is 1 which is recommended for uniform compression. In version 970, solid formulation 1 elements
can be assigned TYPE=2 which treats combined modes of shear and compression. - If mat_126 is used, try ELFORM = 0.
- Try EFG formulation (*section_solid_EFG). Use only where deformations are severe as this formulation is very expensive. Use only with hex elements. ***********************************************************
LS-DYNA FAQ 中英文版-Negative Volume 负体积 2007年09月13日 星期四 下午 10:26 泡沫材料的负体积(或其它软的材料)
对于承受很大变形的材料，比如说泡沫，一个单元可能变得非常扭曲以至于单元的体积计算得到一个负值。这可能发生在材料还没有达到失效标准前。对一个拉格朗日(Lagrangian)网格在没有采取网格光滑(mesh smoothing)或者重划分(remeshing)时能适应多大变形有个内在的限制。LS-DYNA中计算得到负体积(negative volume)会导致计算终止，除非在*control_timestep卡里面设置ERODE选项为1，而且在* control_termination里设置DTMIN项为任何非零的值，在这种情况下，出现负体积的单元会被删掉而且计算继续进行(大多数情况)。有时即使ERODE和DTMIN换上面说的设置了，负体积可能还是会导致因错误终止。
有助于克服负体积的一些方法如下：
* 简单的把材料应力－应变曲线在大应变时硬化。这种方法会非常有效。
* 有时候修改初始网格来适应特定的变形场将阻止负体积的形成。此外，负体积通常只对非常严重的变形情况是个问题，而且特别是仅发生在像泡沫这样的软的材料上面。 * 减小时间步缩放系数(timestep scale factor)。缺省的0.9可能不足以防止数值不稳定。
* 避免用全积分的体单元(单元类型2和3)，它们在包含大变形和扭曲的仿真中往往不是很稳定。全积分单元在大变形的时候鲁棒性不如单点积分单元，因为单元的一个积分点可能出现负的Jacobian而整个单元还维持正的体积。在计算中用全积分单元因计算出现负的Jacobian而终止会比单元积分单元来得快。
* 用缺省的单元方程(单点积分体单元)和类型4或者5的沙漏(hourglass)控制(将会刚化响应)。对泡沫材料首先的沙漏方程是：如果低速冲击type 6，系数1.0; 高速冲击type 2或者3。
* 对泡沫用四面体(tetrahedral)单元来建模，使用类型10体单元。 * 增加DAMP参数(foam model 57)到最大的推荐值0.5。
* 对包含泡沫的接触，用*contact选项卡B来关掉shooting node logic。
* 使用*contact_interior卡
用part set来定义需要用contact_interior来处理的parts，在set_part卡1的第5项DA4来定义contact_interior类型。缺省类型是1，推荐用于单一的压缩。在版本970里，类型1的体单元可以设置type=2，这样可以处理压缩和减切混合的模式。 * 如果用mat_126，尝试ELFORM=0
* 尝试用EFG方程(*section_solid_EFG)。因为这个方程非常费时，所以只用在变形严重的地方，而且只用于六面体单元。追问

你好，我用的是*MAT_PLASTIC_KINEMATIC材料模型。

其实我现在是在复现别人的工作，所以材料参数什么的都是从别人已经算出来的k文件里面直接拷过来，但是不懂为什么还是会出现这样的问题。

Answer 2

在复现的过程中，相关求解设置也是一样的吗？可能实际操作的时候，求解时间步长不一样。