知识点|Abaqus里应用Python的一些技巧

2017-04-21 by:CAE仿真在线来源:互联网

例如:cell4 = mdb.models['block'].parts['crankcase'].cells[4],要把part模块中编号为4的体赋值给cell4,就需通过路径mdb→models→part→cells(4号体属性),其中'block'、'crankcase'、分别是model和part的名字。

在草图Sketch中画线:
s = mdb.models[' block '].ConstrainedSketch(name='grid',
sheetSize=3.0)
s.Line(point1=(-1.275, 0.0), point2=(-1.125, 0.0))
s.Line(point1=(1.125, 0.0), point2=(1.275, 0.0))
执行任何一条命令都必须按照结构树的格式进行操作。我们所看到的python脚本繁杂的语句就是这样形成的。这样大量的命令不能在短时间内掌握,我们只需要根据自己的需要边建立模型边学习就可以了。
a = mdb.models['Model-1'].rootAssembly
s = a.instances['Mount-1'].edges
side1Edges = s.findAt(((0.0475, 0.0, 0.0), ))
以上三行与下面的句子是等同的,即把findat找到的edges赋值给side1Edges。分开来写简单明了,大大缩短了语句的长度。
side1Edges = mdb.models['Model-1'].rootAssembly. instances['Mount-1'].edges. findAt(((0.0475, 0.0, 0.0), ))
a.Surface(side1Edges=side1Edges, name='Bottom'),这行语句设置side1Edges所对应的edge为名称'Bottom'的surface的set。
#===========================================================
3.模型参数分析技巧
Python脚本建模的好处就是可以进行参数分析,即改变我们要分析模型的几何尺寸、材料属性等可变参数,对数值模型进行求解计算,从而对所分析的对象有更全面的了解。
1.对自己要进行参数分析的参数赋值:如几何尺寸或材料属性等a1=20,b1=30,c1=40,命名要符合python规则。
2.cae与Python混合建模,不会的命令就利用cae自动生成,用Python reader记录命令然后进行修改,可以弥补不熟悉Python的缺点;
3.逐句修改Python脚本,可以去掉一些不必要的语句并在cae中逐句进行验证。
#===========================================================
4. 几个命令的体会
4.1 Set ( )
Set命令在python建模时要经常用到,对实体、surface、element等分组,方便加载、施加约束和单元生死等控制
4.2 Findat ( )
对cell、edge、face、vertice进行查找,括号中参数为实体坐标
p = mdb.models['Model-1'].parts['Mount']
f = p.faces
faces = f.findAt(((0.042303, 0.006937, 0.0), ))
pickedRegions =(faces, )
p.setElementType(regions=pickedRegions,
elemTypes=(elemType1, elemType2))
4.3 Len ( )
利用len命令可以实现对单元选取
p = mdb.models['precast culvert'].parts['soil']
e = p.elements
len(e)
n1=len(e)
elements = e[1:n1] #单元数存放在e [ ]的一维数组里
p.Set(elements=elements, name='Set-3')
对单元进行编组set,可以进行生死单元的控制,我摸索了好久才想到这个办法,目前只在二维模型应用过,三维也应该没问题。Abaqus没有办法对单元编号进行编号控制,也没有像ansys那样有效的选择命令,怎样选择abaqus的单元就是很头疼的问题,我要做路堤的分层回填模拟,手动选取单元根本就没有可能。Abaqus的编号其实是有规则的,后划分的单元编号最小,先划分的单元编号最大;这样我们就可以每次划分单元后都采用len命令计算一次单元数量,并用参数记录下来,这样我们就能计算出每部分单元的数量以及他的起始和终止编号。根据elements = e[1:n1]、p.Set(elements=elements, name='Set-3')语句就可以把每部分单元设置成set,以后操作就很方便了。
#===========================================================
5. 一个Abaqus/Python例子
下面是一个Getting Started with Abaqus: Interactive Edition中的一个橡胶避震垫例子:☺号后语句表示我的注释,注释上面的句子。我也不懂的就没有注释,先熟悉一下Python的样子。在学习的时候可以copy(Crtol + V)到cae下面的命令行中一句句的执行,并在cae视窗中查看命令执行情况,领会命令使用方法。
# Script for rubber mount example
☺“#”开头表示这一行为注释行,同ansys的“!”号
from abaqus import *
from abaqusConstants import *
☺引入abaqus中的一些模块,这些模块是abaqus已事先存储在文件中,要引入才这些模块能运行相应的命令
session.viewports['Viewport: 1'].makeCurrent()
session.viewports['Viewport: 1'].maximize()
session.journalOptions.setValues(replayGeometry=COORDINATE,
recoverGeometry=COORDINATE)
☺对cae视窗的操作命令;maximize()的括号好像是默认为当前值
from caeModules import *
from driverUtils import executeOnCaeStartup
executeOnCaeStartup()
Mdb()
#--------------------------------------------------------------------------------------------------
## Sketch profile of the mount
☺进入草图模块
s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__', sheetSize=0.3)
☺建立一个sketch草图,草图的尺寸为0.3个单位;这个句子算是一个标准的Python语句,具体后面解释
g, v, d, c = s.geometry, s.vertices, s.dimensions, s.constraints
s.sketchOptions.setValues(decimalPlaces=3, viewStyle=AXISYM)
s.setPrimaryObject(option=STANDALONE)
☺设置草图为轴对称模式
s.ConstructionLine(point1=(0.0, -100.0), point2=(0.0, 100.0))
s.FixedConstraint(entity=g[2])
☺建立辅助线及约束
mdb.models['Model-1'].sketches['__profile__'].sketchOptions.setValues(gridFrequency=4)
☺sketch参数修改
s.rectangle(point1=(0.01, 0.0), point2=(0.025, 0.01))
☺画矩形
s.DistanceDimension(entity1=g[2], entity2=v[0],textPoint=(0.00998260825872421, -0.00830297358334064), value=0.01)
s.VerticalDimension(vertex1=v[0],vertex2=v[1],textPoint=(0.0,0.00851448811590672), value=0.03)
s.ObliqueDimension(vertex1=v[0],vertex2=v[3],textPoint=(0.025699570775032, -0.00830297358334064), value=0.05)
☺标注图形尺寸,还可以修改图形尺寸,如拉伸、压缩等
s.CircleByCenterPerimeter(center=(0.085,0.025),point1=(0.06, 0.00740899052470922))
☺画圆
s.CoincidentConstraint(entity1=v[5], entity2=g[5])
s.DistanceDimension(entity1=g[2], entity2=v[4],textPoint=(0.0811913833022118, -0.023865295574069), value=0.1)
s.VerticalDimension(vertex1=v[2], vertex2=v[4],textPoint=(0.115524396300316, 0.0262394621968269), value=0.0)
s.ObliqueDimension(vertex1=v[5], vertex2=v[3],textPoint=(0.0519323498010635, 0.0), value=0.005)
☺修改圆尺寸、移动位置―――没搞清楚修改尺寸命令有什么实际意义,直接定义好尺寸不就结了?
s.autoTrimCurve(curve1=g[7],point1=(0.124150268733501,-0.00965208746492863))
☺裁剪命令,其中g[7]是圆的线编号,g=s.geometry
s.autoTrimCurve(curve1=g[5],point1=(0.0601795427501202,0.020298857241869))
s.autoTrimCurve(curve1=g[4],point1=(0.0557677671313286,0.030869778245687))
☺裁剪命令
s.RadialDimension(curve=g[8],textPoint=(0.0725325122475624,0.0207393132150173),radius=0.047169905660283)
d[6].setValues(reference=ON)
☺标注命令,标注界面很漂亮
session.viewports['Viewport: 1'].view.fitView()
☺cae图形缩放的合适大小
p = mdb.models['Model-1'].Part(name='Mount', dimensionality=AXISYMMETRIC, type=DEFORMABLE_BODY)
p = mdb.models['Model-1'].parts['Mount']
☺命名model
p.BaseShell(sketch=s)
s.unsetPrimaryObject()
session.viewports['Viewport: 1'].setValues(displayedObject=p)
del mdb.models['Model-1'].sketches['__profile__']
☺显示model
#--------------------------------------------------------------------------------------------------
## Create material 'Rubber'
☺创建材料模型
mdb.models['Model-1'].Material('Rubber')
mdb.models['Model-1'].materials['Rubber'].Hyperelastic(type=POLYNOMIAL, table=())
mdb.models['Model-1'].materials['Rubber'].hyperelastic.UniaxialTestData(table=(( 0.054E6, 0.0380), (0.152E6, 0.1338), (0.254E6, 0.2210), (0.362E6, 0.3450), (0.459E6, 0.4600), (0.583E6, 0.6242), (0.656E6, 0.8510), (0.730E6, 1.4268)))
mdb.models['Model-1'].materials['Rubber'].hyperelastic.BiaxialTestData(table=((0.089E6, 0.0200), (0.255E6, 0.1400), (0.503E6, 0.4200), (0.958E6, 1.4900), (1.703E6, 2.7500), (2.413E6, 3.4500)))
mdb.models['Model-1'].materials['Rubber'].hyperelastic.PlanarTestData(table=((0.055E6, 0.0690), (0.324E6, 0.2828), (0.758E6, 1.3862), (1.269E6, 3.0345), (1.779E6, 4.0621)))
##
## Create material 'Steel'
##
mdb.models['Model-1'].Material('Steel')
mdb.models['Model-1'].materials['Steel'].Elastic(table=((200.E9, 0.3), ))
##
## Create solid sections for the rubber and steel
##
mdb.models['Model-1'].HomogeneousSolidSection(name='RubberSection',
material='Rubber', thickness=1.0)
mdb.models['Model-1'].HomogeneousSolidSection(name='SteelSection',
material='Steel', thickness=1.0)
#-------------------------------------------------------------------
## Partition the part into two regions (rubber and steel regions)
☺切割体形成两个部分,从而可以赋予不同材料属性
f, e, d = p.faces, p.edges, p.datums
t =p.MakeSketchTransform(sketchPlane=f.findAt(coordinates=(0.043333,
0.001667,0.0),normal=(0.0,0.0,1.0)),sketchPlaneSide=SIDE1,
origin=(0.033052,0.014514, 0.0))
s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',
sheetSize=0.134, gridSpacing=0.003, transform=t)
g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints
s.sketchOptions.setValues(decimalPlaces=3)
s.setPrimaryObject(option=SUPERIMPOSE)
p.projectReferencesOntoSketch(sketch=s, filter=COPLANAR_EDGES)
☺进入草图,并设置草图属性(图纸大小、网格间距等)
s.Line(point1=(0.026948, -0.009514), point2=(-0.03, -0.009514))
s.HorizontalConstraint(entity=g.findAt((-0.001526, -0.009514)))
s.PerpendicularConstraint(entity1=g.findAt((0.026948, -0.012014)),
entity2=g.findAt((-0.001526, -0.009514)))
☺作辅助线,findat(查找)命令很有用,可以用来选择实体
pickedFaces = f.findAt(((0.043333, 0.001667, 0.0), ))
p.PartitionFaceBySketch(faces=pickedFaces, sketch=s)
☺用辅助线分割体
s.unsetPrimaryObject()
☺显示分割后体
del mdb.models['Model-1'].sketches['__profile__']
#--------------------------------------------------------------------------------------------------
## Assign rubber section
☺实体指定不同的材料属性
p = mdb.models['Model-1'].parts['Mount']
f = p.faces
faces = f.findAt(((0.042303, 0.006937, 0.0), ))
region = regionToolset.Region(faces=faces)
p.SectionAssignment(region=region, sectionName='RubberSection', offset=0.0)
##
## Assign steel section
##
faces = f.findAt(((0.043333, 0.003333, 0.0), ))
region = regionToolset.Region(faces=faces)
p.SectionAssignment(region=region, sectionName='SteelSection', offset=0.0)
a = mdb.models['Model-1'].rootAssembly
session.viewports['Viewport: 1'].setValues(displayedObject=a)
##
## Set coordinate system (done by default)
##
a.DatumCsysByDefault(CARTESIAN)
##
## Instance the mount
##
p = mdb.models['Model-1'].parts['Mount']
a.Instance(name='Mount-1', part=p, dependent=ON)
##
## Create geometry set 'Middle'
##
e = a.instances['Mount-1'].edges
edges = e.findAt(((0.020708, 0.03, 0.0), ))
a.Set(edges=edges, name='Middle')
☺通过findat命令定义了一个edges组“Middle”
## Create geometry set 'Out'
##
v = a.instances['Mount-1'].vertices
verts = v.findAt(((0.01, 0.0, 0.0), ))
a.Set(vertices=verts, name='Out')
☺通过findat命令定义了一个vertices组“Out”
## Create surface 'Bottom'
##
s = a.instances['Mount-1'].edges
side1Edges = s.findAt(((0.0475, 0.0, 0.0), ))
a.Surface(side1Edges=side1Edges, name='Bottom')
☺通过findat命令定义了一个edges组“Bottom”
#--------------------------------------------------------------------------------------------------
## Create a static general step
☺进入step模块
mdb.models['Model-1'].StaticStep(name='Compress mount', previous='Initial',
description='Apply axial pressure load to mount', timePeriod=1,
adiabatic=OFF, maxNumInc=100, stabilization=None,
timeIncrementationMethod=AUTOMATIC,
initialInc=0.01, minInc=1e-05, maxInc=1, matrixSolver=SOLVER_DEFAULT,
amplitude=RAMP, extrapolation=LINEAR, fullyPlastic="", nlgeom=ON)
☺step中的一些设置,与cae操作框相对应
session.viewports['Viewport: 1'].assemblyDisplay.setValues(
step='Compress mount')
☺cae中显示step模块 Compress mount
##
## Modify output requests
##
mdb.models['Model-1'].fieldOutputRequests['F-Output-1'].setValues(
variables=('S', 'PE', 'PEEQ', 'PEMAG', 'NE', 'LE', 'U', 'RF',
'CF', 'CSTRESS', 'CDISP'))
☺对结果数据输出的一些定义
regionDef=a.sets['Out']
mdb.models['Model-1'].HistoryOutputRequest(name='H-Output-1',
createStepName='Compress mount', variables=('U1', 'U2', 'U3'),
region=regionDef)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(loads=ON, bcs=ON,
predefinedFields=ON)
#--------------------------------------------------------------------------------------------------
## Apply pressure load
☺进入load模块
region = a.surfaces['Bottom']
mdb.models['Model-1'].Pressure(name='Pressure',
createStepName='Compress mount', region=region, magnitude=500000.0)
☺通过bottom的set对底边进行加载
## Apply symmetry bc to set "Middle'
##
region = a.sets['Middle']
mdb.models['Model-1'].DisplacementBC(name='Symmetry',
createStepName='Compress mount', region=region, u2=0.0)
☺对顶面进行约束
## Suppress visibility of datum geometry
##
session.viewports['Viewport: 1'].assemblyDisplay.geometryOptions.setValues(
geometryEdgesInShaded=OFF, datumPoints=OFF, datumAxes=OFF, datumPlanes=OFF,datumCoordSystems=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=ON, loads=OFF,
bcs=OFF, predefinedFields=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=ON)
p = mdb.models['Model-1'].parts['Mount']
session.viewports['Viewport: 1'].setValues(displayedObject=p)
☺mesh模块的一些显示设置
#--------------------------------------------------------------------------------------------------
## Assign edge seeds
☺进入mesh模块
p = mdb.models['Model-1'].parts['Mount']
e = p.edges
pickedEdges = e.findAt(((0.0225, 0.005, 0.0), ), ((0.0475, 0.0, 0.0), ),
((0.020708, 0.03, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=30)
pickedEdges = e.findAt(((0.053289, 0.023434, 0.0), ), ((0.01, 0.01125, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=14)
pickedEdges = e.findAt(((0.01, 0.00125, 0.0), ), ((0.06, 0.00375, 0.0), ))
p.seedEdgeByNumber(edges=pickedEdges, number=1)
☺选择边,设置种子数
## Use structured meshing
##
f = p.faces
pickedRegions = f
p.setMeshControls(regions=pickedRegions, technique=STRUCTURED)
☺ STRUCTURED划分网格
## Assign element type to the rubber
##
elemType1 = mesh.ElemType(elemCode=CAX4H, elemLibrary=STANDARD)
elemType2 = mesh.ElemType(elemCode=CAX3, elemLibrary=STANDARD)
faces = f.findAt(((0.042303, 0.006937, 0.0), ))
pickedRegions =(faces, )
p.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2))
## Assign element type to the steel
##
elemType1 = mesh.ElemType(elemCode=CAX4I, elemLibrary=STANDARD)
elemType2 = mesh.ElemType(elemCode=CAX3, elemLibrary=STANDARD)
faces = f.findAt(((0.043333, 0.003333, 0.0), ))
pickedRegions =(faces, )
p.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2))
☺ 单元类型设置及不同材料面指定
## Generate mesh
##
p.generateMesh()
☺ 划分当前网格
session.viewports['Viewport: 1'].assemblyDisplay.setValues(mesh=OFF)
session.viewports['Viewport: 1'].assemblyDisplay.meshOptions.setValues(
meshTechnique=OFF)
#--------------------------------------------------------------------------------------------------
## Create job
☺ 创建job设置
mdb.Job(name='Mount', model='Model-1',
description='Axisymmetric mount analysis under axial loading',
modelPrint=ON)
a = mdb.models['Model-1'].rootAssembly
a.regenerate()
##
## Save model database
##
mdb.saveAs('Mount')
#--------------------------------------------------------------------------------------------------
小结:
1.Abaqus的python看似繁琐,但有着其固定、严谨的结构并不难理解
2.pthon的顺序与cae的模块操作顺序基本一致
3.这个例子的python脚本基本与cae自动生成的python脚本基本相同,完全可以通过交互式修改cae生成的python.rpy文件来建立自己的python脚本,免去了许多学习abaqus python命令格式的痛苦。