Abaqus输入文件INP解释 - 引自《ABAQUS工程实例详解》

 

**文件抬头说明
*Heading
** Job name: Job-1_Terminal Model name: Model-1
** Generated by: Abaqus/CAE 6.14-4
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**部件
** PARTS
**Terminal 部件的网格节点：编号和坐标，共计1991个节点
*Part, name=Terminal
*Node
      1,  -50.9272423,   8.98902893,          0.5
      2,  -51.2807961,    9.3425827,          0.5
      3,  -51.2807961,    9.3425827,           0.
            .....
   1989,  -49.3747673,   7.61297083, 0.0500000007
   1990,  -49.3247681,   7.61297083, 0.0500000007
   1991,  -49.2747688,   7.61297083, 0.0500000007
**Terminal部件的单元类型S4R、编号，以及由哪些节点组成，共计1800个单元
*Element, type=S4R
  1,   1,  17, 435,  52
  2,  17,  18, 436, 435
  3,  18,  19, 437, 436
        .....
1798, 1989, 1990,  397,  398
1799, 1990, 1991,  396,  397
1800, 1991,  395,   16,  396
**在选择几何赋予材料属性时，程序内部生成的节点集，具有全部节点1991个
*Nset, nset=_PickedSet2, internal, generate
    1,  1991,     1
**在选择几何赋予材料属性时，程序内部生成的单元集，具有全部单元1800个
*Elset, elset=_PickedSet2, internal, generate
    1,  1800,     1
**自定义的Set-1_Node节点集，仅有一个节点，节点编号为548
*Nset, nset=Set-1_Node
 548,
**界面属性名称Section：Section-shell
** Section: Section-shell
*Shell Section, elset=_PickedSet2, material=C7025-TM00
0.2, 5
*End Part
**以上为部件，以下为装配体
** ASSEMBLY 
*Assembly, name=Assembly
**转配实例
*Instance, name=Terminal-1, part=Terminal
*End Instance
**在选择固体边界几何面时，程序内部生成的装配实例节点集
*Nset, nset=_PickedSet4, internal, instance=Terminal-1
   13,   14,   15,   16,  338,  339,  340,  341,  342,  343,  344,  345,  346,  348,  349,  350
        .....
 1989, 1990, 1991
**在选择固体边界几何面时，程序内部生成的装配实例单元集（编号1401~1800）
*Elset, elset=_PickedSet4, internal, instance=Terminal-1, generate
 1401,  1800,     1
*End Assembly
**定义材料
** MATERIALS
** 
*Material, name=C7025-TM00
*Elastic
133500., 0.3
*Plastic
545.,  0.
703., 0.1
** ----------------------------------------------------------------
** 定义分析步
** STEP: Step-1_Displacement
** 
*Step, name=Step-1_Displacement, nlgeom=YES
*Static
0.1, 1., 1e-05, 0.1
** 定义边界条件
** BOUNDARY CONDITIONS
** 
** Name: BC-1_Encastre Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PickedSet4, ENCASTRE
** Name: BC-2_Set-Displacement Type: Displacement/Rotation
*Boundary
Terminal-1.Set-1_Node, 2, 2, -0.5
** 定义输出需求
** OUTPUT REQUESTS
** 定义重启文件保存频率，针对Standard分析时，默认为0
*Restart, write, frequency=0
** 厚度场输出自定义
** FIELD OUTPUT: F-Output-Thinckness
** 
*Output, field
*Element Output, directions=YES
STH, 
** 系统默认场输出定义
** FIELD OUTPUT: F-Output-1
** 
*Output, field, variable=PRESELECT
** 力、位移历史输出自定义
** HISTORY OUTPUT: H-Output-Set-Node
** 
*Output, history
*Node Output, nset=Terminal-1.Set-1_Node
RF2, U2
** 系统默认历史输出定义
** HISTORY OUTPUT: H-Output-1
** 
*Output, history, variable=PRESELECT
*End Step