Abaqus 隐式分析转显示分析
导入模板
导入模型一般模板如下，其中update=NO表示import后的模型采用原始构型，yes表示采用新的基准。
只有在考虑集合非线性的情况下才能update=yes
若采用NO则位移在导入前后保持连续，且材料状态可以导入。
若采用YES则单元属性及节点坐标均可更改，但材料状态不会导入。
隐式转显式（由实例进行装配）
- 显式部分
*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, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *STATIC … *RESTART, WRITE, FREQUENCY=n *END STEP
- 显式部分
*HEADING Part definitions (optional) *ASSEMBLY, NAME=Assembly-1 *INSTANCE, INSTANCE=i1, LIBRARY=oldjob-name Additional set and surface definitions (optional) *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO *END INSTANCE Additional part instance definitions (optional) Assembly level set and surface definitions *END ASSEMBLY ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to redefine linear elasticity *PLASTIC Data lines to redefine Mises plasticity … *BOUNDARY Data lines to redefine boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP
隐式转显式（直接导入装配件）
- 隐式部分
*HEADING … *MATERIAL, NAME=mat1 *ELASTIC Data lines to define linear elasticity *PLASTIC Data lines to define Mises plasticity *DENSITY Data line to define the density of the material … *BOUNDARY Data lines to define boundary conditions *STEP *STATIC … *RESTART, WRITE, FREQUENCY=n *END STEP
- 显式部分
*HEADING *IMPORT, STEP=step, INCREMENT=increment, STATE=YES, UPDATE=NO Data lines to specify element sets to be imported *IMPORT ELSET Data lines to specify element set definitions to be imported *IMPORT NSET Data lines to specify node set definitions to be imported ** *** Optionally redefine the material block ** *MATERIAL, NAME=mat1 *ELASTIC Data lines to redefine linear elasticity *PLASTIC Data lines to redefine Mises plasticity … *BOUNDARY Data lines to redefine boundary conditions *STEP *DYNAMIC, EXPLICIT … *END STEP
导入限制
节点导入与节点定义
- 新的节点定义需要基于变形后的节点，无论update=yes or no
- 只有导入的单元
- 若update=no则，所导入的单元、节点均可以改变坐标
集合导入
材料信息导入
update=no，state=yes的情况下，才可以导入材料状态。只有如下所示的情况才能导入材料状态，其他情况仅能导入应力。
- linear elasticity,
- Mises plasticity (including the kinematic hardening models),
- extended Drucker-Prager plasticity,
- crushable foam plasticity,
- Mohr-Coulomb plasticity,
- critical state (clay) plasticity,
- cast iron plasticity,
- concrete damaged plasticity,
- hyperelasticity (including Mullins effect),
- hyperfoam,
- viscoelasticity,
- traction-separation response with damage for cohesive elements,
- damage for ductile metals,
- damage for fiber-reinforced composites,
- connector behavior,
- materials defined in user subroutines
UMATandVUMAT, and - materials defined using the parallel rheological framework for nonlinear viscoelastic-elastoplastic behavior.
初始条件导入
允许导入的初始条件包括以下部分：
| Initial condition | Material state imported |
|---|---|
| Hardening | No |
| Relative density | No |
| Rotational velocity | Yes or No |
| Solution-dependent state variables | No |
| Stress | No |
| Velocity | Yes or No |
| Void ratio | No |
温度应力无法导入，此时预应力需要通过用户材料子程序的方式施加。
边界条件
导入前后的边界条件需要保持一致，例：导入前施加位移为0.1，则导入后施加的位移要从0.1开始
import材料子程序
前后两步中sdv变量要一一对应，才能正确传递数值。
需要注意的是：后一步的sdv个数会自动选为前一步已经使用的sdv的个数，而不是定义的*Depvar的个数。