学习script 第一例

wrj001

# -*- coding: mbcs -*-
此行为注释行，# 开始from part import *
from material import *
from section import *
from assembly import *
from step import *
from interaction import *
from load import *
from mesh import *
from optimization import *
from job import *
from sketch import *
from visualization import *
from connectorBehavior import *
引入Abaqus使用的模块/用不到的可不引入
mdb.models['Model-1'].ConstrainedSketch(name='__profile__', sheetSize=20.0)
mdb.models['Model-1'].sketches['__profile__'].rectangle(point1=(-5.0, -1.0),
    point2=(5.0, 5.0))
mdb.models['Model-1'].Part(dimensionality=TWO_D_PLANAR, name='Part-1', type=
    DEFORMABLE_BODY)
mdb.models['Model-1'].parts['Part-1'].BaseShell(sketch=
    mdb.models['Model-1'].sketches['__profile__'])
del mdb.models['Model-1'].sketches['__profile__']
mdb 变量为 model database,  使用此变量可生成模型;
ConstrainedSketch() 方法生成模型；
使用ConstrainedSketch() 中的 rectangle()方法在sketch面上生成rectangle，参数为两个对角点坐标，也可不使用point1,point2:rectangle((-5.0, -1.0),  (5.0, 5.0));
..............
这些行生成草图与零件 sketch and part
mdb.models['Model-1'].Material(name='STEEL')
mdb.models['Model-1'].materials['STEEL'].Elastic(table=((200000.0, 0.3), ))
mdb.models['Model-1'].HomogeneousSolidSection(material='STEEL', name=
    'Section-1', thickness=None)
mdb.models['Model-1'].parts['Part-1'].SectionAssignment(offset=0.0,
    offsetField='', offsetType=MIDDLE_SURFACE, region=Region(
    faces=mdb.models['Model-1'].parts['Part-1'].faces.findAt(((-1.666667, 1.0,
    0.0), (0.0, 0.0, 1.0)), )), sectionName='Section-1', thicknessAssignment=
    FROM_SECTION)
材料，截面与截面赋予
mdb.models['Model-1'].rootAssembly.DatumCsysByDefault(CARTESIAN)
mdb.models['Model-1'].rootAssembly.Instance(dependent=ON, name='Part-1-1',
    part=mdb.models['Model-1'].parts['Part-1'])
组装
mdb.models['Model-1'].StaticStep(initialInc=0.1, name='Step-1', nlgeom=ON,
    previous='Initial')
生成一个step
mdb.models['Model-1'].rootAssembly.Set(edges=
    mdb.models['Model-1'].rootAssembly.instances['Part-1-1'].edges.findAt(((
    -5.0, 0.5, 0.0), )), name='WEST')
mdb.models['Model-1'].rootAssembly.Surface(name='NORTH', side1Edges=
    mdb.models['Model-1'].rootAssembly.instances['Part-1-1'].edges.findAt(((
    -2.5, 5.0, 0.0), )))
定义边界
mdb.models['Model-1'].DisplacementBC(amplitude=UNSET, createStepName='Step-1',
    distributionType=UNIFORM, fieldName='', fixed=OFF, localCsys=None, name=
    'BC-1', region=mdb.models['Model-1'].rootAssembly.sets['WEST'], u1=0.0, u2=
    0.0, ur3=0.0)
mdb.models['Model-1'].Pressure(amplitude=UNSET, createStepName='Step-1',
    distributionType=UNIFORM, field='', magnitude=-10.0, name='Load-1', region=
    mdb.models['Model-1'].rootAssembly.surfaces['NORTH'])
定义边界条件
mdb.models['Model-1'].parts['Part-1'].setMeshControls(elemShape=QUAD,
    minTransition=OFF, regions=
    mdb.models['Model-1'].parts['Part-1'].faces.findAt(((-1.666667, 1.0, 0.0),
    )), technique=STRUCTURED)
mdb.models['Model-1'].parts['Part-1'].setElementType(elemTypes=(ElemType(
    elemCode=CPS8, elemLibrary=STANDARD), ElemType(elemCode=CPS6M,
    elemLibrary=STANDARD)), regions=(
    mdb.models['Model-1'].parts['Part-1'].faces.findAt(((-1.666667, 1.0, 0.0),
    )), ))
mdb.models['Model-1'].parts['Part-1'].seedPart(deviationFactor=0.1,
    minSizeFactor=0.1, size=0.125)
mdb.models['Model-1'].parts['Part-1'].generateMesh()
设置网格，划分/网格尺寸
mdb.models['Model-1'].rootAssembly.regenerate()
mdb.Job(atTime=None, contactPrint=OFF, description='', echoPrint=OFF,
    explicitPrecision=SINGLE, getMemoryFromAnalysis=True, historyPrint=OFF,
    memory=90, memoryUnits=PERCENTAGE, model='Model-1', modelPrint=OFF,
    multiprocessingMode=DEFAULT, name='EXAMPLE', nodalOutputPrecision=SINGLE,
    numCpus=1, numGPUs=0, queue=None, scratch='', type=ANALYSIS,
    userSubroutine='', waitHours=0, waitMinutes=0)
mdb.jobs['EXAMPLE'].submit(consistencyChecking=OFF)
生成JOB
一个长方形，左边约束，上边施加均布拉载荷。在Abaqus里建模，提交后，保存Cae，在工作目录下生成jnl文件。将后缀改为py，删除后面的计算部分即可。