Abaqus 隱式分析轉顯示分析
導入模板
導入模型一般模板如下，其中update=NO表示import后的模型采用原始構型，yes表示采用新的基准。
只有在考慮集合非線性的情況下才能update=yes
若采用NO則位移在導入前后保持連續，且材料狀態可以導入。
若采用YES則單元屬性及節點坐標均可更改，但材料狀態不會導入。
隱式轉顯式（由實例進行裝配）
- 顯式部分
*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
- 顯式部分
*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
隱式轉顯式（直接導入裝配件）
- 隱式部分
*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
- 顯式部分
*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
導入限制
節點導入與節點定義
- 新的節點定義需要基於變形后的節點，無論update=yes or no
- 只有導入的單元
- 若update=no則，所導入的單元、節點均可以改變坐標
集合導入
材料信息導入
update=no，state=yes的情況下，才可以導入材料狀態。只有如下所示的情況才能導入材料狀態，其他情況僅能導入應力。
- 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.
初始條件導入
允許導入的初始條件包括以下部分：
| 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 |
溫度應力無法導入，此時預應力需要通過用戶材料子程序的方式施加。
邊界條件
導入前后的邊界條件需要保持一致，例：導入前施加位移為0.1，則導入后施加的位移要從0.1開始
import材料子程序
前后兩步中sdv變量要一一對應，才能正確傳遞數值。
需要注意的是：后一步的sdv個數會自動選為前一步已經使用的sdv的個數，而不是定義的*Depvar的個數。
import單元子程序
uel與vuel無法互通，可分別計算，但是sdv無法傳遞