输入文件模板
以下模板包括基本的Abaqus选项和创建破碎分析所需的所有可用的CZone for Abaqus选项。模板中有两个块，每个块都以材料定义开始。第一个区块是用于蔡武伤害初始化。第二块是用于Hashin伤害初始化。模板的其余部分继续引用蔡武模型的所有材料。模板使用Abaqus/CAE中使用的部件和实例输入文件格式;但是，CZone for Abaqus不要求您使用这种格式。
*HEADING
…
*PART, NAME=Part-1
Node, element, section, set, and surface definitions
*END PART
*ASSEMBLY, NAME=Assembly-1
*INSTANCE, NAME=i1, PART=Part-1
<positioning data>
Additional set and surface definitions (optional)
*END INSTANCE
Assembly level set and surface definitions
…
*END ASSEMBLY
**
**Material with Tsai-Wu damage
**
*MATERIAL, NAME=material1
*PARAMETER
Independent parameter definitions for plane stress orthotropic elasticity
*ELASTIC, TYPE=LAMINA
Data lines to define the material constants
Data lines to define the material constants with damage evolution
*DEPVAR, DELETE=1
Data lines to define the 3 dependent variables (status, Tsai-Wu, and stiffness degradation)
*USER DEFINED FIELD, CZONE, PROPERTIES=16
Data lines to define Tsai-Wu failure stresses and the original material stiffness and absorbed energy
*CRUSH STRESS
Data lines to define the crush stress as a function of orientation
*CRUSH STRESS VELOCITY FACTOR
Data line to define the stress scaling factor as a function of relative velocity (optional)
**
**End Tsai-Wu material definition
**
**
**Material with Hashin damage
**
*MATERIAL, NAME=material2
*PARAMETER
Independent parameter definitions for plane stress orthotropic elasticity
*ELASTIC, TYPE=LAMINA
Data lines to define the material constants
*DAMAGE INITIATION, CRITERION=HASHIN
Data lines to define the Hashin failure criterion
*DAMAGE EVOLUTION
Data lines to define the evolution of damage leading to eventual failure
*CRUSH STRESS
Data lines to define the crush stress as a function of orientation
*CRUSH STRESS VELOCITY FACTOR
Data line to define the stress scaling factor as a function of relative velocity (optional)
**
**End Hashin material definition
**
*SURFACE INTERACTION, NAME=Int-1
*FRICTION
Specify the friction coefficient
*INITIAL CONDITIONS, TYPE=VELOCITY
Nodeset1, dof, initial_velocity
**
*STEP, NAME=Step-1
*DYNAMIC, Explicit
, time
**
**Optional boundary condition for use with *CRUSH STRESS VELOCITY FACTOR
**
*BOUNDARY, TYPE=VELOCITY
Data line to define stress scaling factor and relative velocity
*CONTACT
*CONTACT INCLUSIONS, ALL EXTERIOR
*CONTACT PROPERTY ASSIGNMENT
, , Int-1
**
**Output requests
**
*RESTART, WRITE, NUMBER INTERVAL=integer, TIME MARKS=NO
*OUTPUT, FIELD, VARIABLE=PRESELECT
...
Specify desired element, contact, and history output requests
*END STEP
温馨提示：
此文档为达索官方英文文档翻译，尽管我们已经尽力确保准确性，但在翻译过程中可能会有一些错误或细微差别。如果想要了解官方原版，可联系客服进行索取。
