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 UMAT and VUMAT, 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。

import单元子程序

uel与vuel无法互通，可分别计算，但是sdv无法传递