【Abaqus】*Solid Section定义复合材料

*SOLID SECTION

介绍

*solid section 用来定义单元的材料属性,材料方向等信息:

  1. solid (continuum) elements
  2. infinite elements
  3. acoustic finite and infinite elements
  4. particle elements
  5. truss elements.

Type : Model data;Level : Part,Part instance;Abaqus/CAE : Property module

  • example:

img

** Section: Section-1
*Solid Section, elset=Set-3, composite, orientation=Ori-1, layup=lam
0.5, 1, Gr/Epoxy, 0., p1
0.05, 1, pvdf2, 0., pv1
0.5, 1, Gr/Epoxy, 90., p2
0.5, 1, Gr/Epoxy, 90., p3
0.5, 1, Gr/Epoxy, 90., p4
0.05, 1, pvdf2, 90., pv2
0.5, 1, Gr/Epoxy, 0., p5

data lines

format 1

define homogeneous solid elements, infinite elements, acoustic elements, particle, or truss elements

First (and only) line:

  1. Enter any attribute values required. The default for the first attribute is 1.0.

format 2

define a composite solid

First line:

  1. layer thickness(可以是单元相对厚度). 各层的thickness在求解时会自动调整,使所有layer thickness 之和==堆叠方向上的单元长度。
  2. Number of integration points , layer厚度上的积分点个数,必须是奇数,默认值1.0
  3. layer material name, 各层的材料名称.
  4. layer orientation, 各层的材料方向 , 可以是orien angle,也可以引用一个orientation, 或者一个orien distribution
  5. ply name,指定ply的名称,如果没有指定,则会自动生成ply名称.

重复first line, 直到所有层都定义完毕.如果SYMMETRIC参数出现,则只需要定义从底层到中面的层ply.

参数说明

必要的参数

  • elset : string, 单元集的名称.e.g. elset=Set-3
  • composite : none, 该参数只能用于只有位移自由度的三维brick solid elements type。如果单元属于多层材料，则必须包含此参数。这个参数只对Abaqus/Standard analyses有效
  • material : string, 材料名称.e.g. material=cfrp

The composute 和material参数不能同时出现，如果单元是均质材料就使用material，是多层材料就使用composite。

  • ref node : 该参数仅适用于广义平面应变单元和声学无限单元;对于所有其他元素类型，它将被忽略。将此参数设置为参考节点的节点号或包含参考节点的节点集的名称。如果选择了节点集的名称，则该节点集必须只包含一个节点。e.g. ref node=node_set-1 or ref node=Node-1

可选的参数

  • CONTROLS

这个参数用来指定SECTION SONTROLS.具体参见帮助文档

The SECTION CONTROLS option can be used to select the hourglass control and order of accuracy of the formulation for two- and three-dimensional solid elements and to select the kinematic formulation for 8-node brick elements.

  • LAYUP

这个参数需要和composite参数一起使用,Set this parameter equal to the name of a composite layup

  • ORDER

此参数只能用于Abaqus/Explicit中的声学无限单元。定义用于解析声场在无限方向上的变化的九阶多项式的个数,默认ORDER=10

  • STACK DIRECTION

此参数仅适用于Abaqus/Standard分析。只用于composite element.定义堆叠方向,默认STACK DIRECTION=3

  • SYMMETRIC

需要和composite参数一起使用,如果设置为SYMMETRIC,则只需要定义从底层到中面的层ply.

This parameter cannot be used if spatially varying orientation angles are defined on any composite layer using distributions

定义各向异性材料必须的参数

对于isotropic ,是可选的

  • orientation : string, 材料方向,这个参数用来定义单元局部材料坐标..e.g. orientation=Ori-1

For a composite solid ,orientation 选项+ orientation angle 一起定义了laminate 中ply的材料方向

此外,也可以直接在data line中引用orientation 来定义layer 方向.此时orientation参数指定的材料方向将被忽略,其他layer如果没指定angle,或引用orienation,则会使用orientaion参数作为该layer的方向.即默认为0度

*Orientation, name=Ori-1
          1.,           0.,           0.,           0.,           1.,           0.
1, 0.
*Orientation, name=Ori-2
          0., 0.161320529915925, 0.986902065368011,           0., 0.986902065368011, -0.161320529915925
1, 0.
** Section: Section-1
*Solid Section, elset=Set-3, composite, orientation=Ori-1, layup=lam
0.5, 1, Gr/Epoxy, Ori-2, p1
0.05, 1, pvdf2, 0., pv1
0.5, 1, Gr/Epoxy, 90., p2
0.5, 1, Gr/Epoxy, 90., p3
0.5, 1, Gr/Epoxy, 90., p4
0.05, 1, pvdf2, 90., pv2
0.5, 1, Gr/Epoxy, 0., p5

在dat文件中会warning:

 ***WARNING: A SECTION ORIENTATION AND LAYER ORIENTATION HAS BEEN SPECIFIED. 
             THE SECTION ORIENTATION WILL BE IGNORED.
 LINE IMAGE: 0.5, 1, GR/EPOXY, ASSEMBLY_PART-1-1_ORI-2, P1
展开查看inp 
*Heading
** Job name: Job-1 Model name: Model-1
** Generated by: Abaqus/CAE 2020
*Preprint, echo=NO, model=NO, history=NO, contact=NO
**
** PARTS
**
*Part, name=Part-1
*Node
      1,          10.,  0.425000012,    2.5999999
      2,          10.,  -4.57499981,    2.5999999
      3,          10.,  0.425000012,           0.
      4,          10.,  -4.57499981,           0.
      5,          7.5,  0.425000012,    2.5999999
      6,          7.5,  -4.57499981,    2.5999999
      7,          7.5,  0.425000012,           0.
      8,          7.5,  -4.57499981,           0.
      9,           5.,  0.425000012,    2.5999999
     10,           5.,  -4.57499981,    2.5999999
     11,           5.,  0.425000012,           0.
     12,           5.,  -4.57499981,           0.
     13,          2.5,  0.425000012,    2.5999999
     14,          2.5,  -4.57499981,    2.5999999
     15,          2.5,  0.425000012,           0.
     16,          2.5,  -4.57499981,           0.
     17,           0.,  0.425000012,    2.5999999
     18,           0.,  -4.57499981,    2.5999999
     19,           0.,  0.425000012,           0.
     20,           0.,  -4.57499981,           0.
*Element, type=CSS8
1,  7,  8,  4,  3,  5,  6,  2,  1
2, 11, 12,  8,  7,  9, 10,  6,  5
3, 15, 16, 12, 11, 13, 14, 10,  9
4, 19, 20, 16, 15, 17, 18, 14, 13
*Nset, nset="Edge Seeds-1", generate
  1,  20,   1
*Elset, elset="Edge Seeds-1", generate
 1,  4,  1
*Nset, nset=Set-3, generate
  1,  20,   1
*Elset, elset=Set-3, generate
 1,  4,  1
*Orientation, name=Ori-1
          1.,           0.,           0.,           0.,           1.,           0.
1, 0.
*Orientation, name=Ori-2
          0., 0.161320529915925, 0.986902065368011,           0., 0.986902065368011, -0.161320529915925
1, 0.
** Section: Section-1
*Solid Section, elset=Set-3, composite, orientation=Ori-1, layup=lam
0.5, 1, Gr/Epoxy, Ori-2, p1
0.05, 1, pvdf2, 0., pv1
0.5, 1, Gr/Epoxy, 90., p2
0.5, 1, Gr/Epoxy, 90., p3
0.5, 1, Gr/Epoxy, 90., p4
0.05, 1, pvdf2, 90., pv2
0.5, 1, Gr/Epoxy, 0., p5
*End Part
**  
**
** ASSEMBLY
**
*Assembly, name=Assembly
**  
*Instance, name=Part-1-1, part=Part-1
*End Instance
**  
*Nset, nset=Set-2, instance=Part-1-1
  3,  4,  7,  8, 11, 12, 15, 16, 19, 20
*Elset, elset=Set-2, instance=Part-1-1, generate
 1,  4,  1
*Nset, nset=Set-fix, instance=Part-1-1, generate
 17,  20,   1
*Elset, elset=Set-fix, instance=Part-1-1
 4,
*End Assembly
** 
** MATERIALS
** 
** si-mm,Gr/Epoxy
*Material, name=Gr/Epoxy
*Density
 1.578e-09,
*Elastic, type=ENGINEERING CONSTANTS
132400.,10800.,10800.,  0.24,  0.24,  0.49, 5600., 5600.
 3600.,
** si-mm
*Material, name=pvdf2
*Density
 1.8e-09,
*Dielectric
 228.568,
*Elastic
10000., 0.3
*Piezoelectric, type=E
0.,       0.,       0.,       0.,       0.,       0.,       0.,       0.
       0.,       0.,       0.,       0., -1.8e-11,       0.,    3e-11,       0.
       0.,       0.
** 
** BOUNDARY CONDITIONS
** 
** Name: BC-2 Type: Electric potential
*Boundary
Set-2, 9, 9
** ----------------------------------------------------------------
** 
** STEP: Step-1
** 
*Step, name=Step-1, nlgeom=NO, perturbation
*Frequency, eigensolver=Lanczos, sim, acoustic coupling=on, normalization=mass
15, , , , , 
** 
** BOUNDARY CONDITIONS
** 
** Name: BC-1 Type: Displacement/Rotation
*Boundary
Set-fix, 1, 1
Set-fix, 2, 2
Set-fix, 3, 3
Set-fix, 4, 4
Set-fix, 5, 5
Set-fix, 6, 6
** 
** OUTPUT REQUESTS
** 
*Restart, write, frequency=0
** 
** FIELD OUTPUT: F-Output-1
** 
*Output, field
*Node Output
EPOT, U
*Element Output, directions=YES
1, 2, 3, 4, 5, 6, 7
E, ELEDEN, ELEN, ENER, EVOL, S
*End Step
posted @ 2024-08-19 11:07  FE-有限元鹰  阅读(139)  评论(0)  编辑  收藏  举报