基于Python的Abaqus二次开发实例讲解

铺就函授 2018年4月27日 1444浏览 8收藏

专题技术邻> CAE仿真> 结构仿真

基于Python的Abaqus的二次开发便捷之处在于：

1、所有的代码均可以先在Abaqus\CAE中操作一遍后再通过rp文件读取，然后再在此基础上进行相应的修改；

2、Python是一种解释性语言，读起来非常清晰，因此在修改程序的过程中，不存在程序难以理解的问题；

3、Python是一种通用性的、功能非常强大的面向对象编程语言，有许多成熟的类似于Matlab函数的程序在网络上流传，为后期进一步的数据处理提供了方便。

为了更加方便地完成Abaqus的二次开发，需进行一些相关约定：

1、所有参数化直接通过点的坐标值进行，直接对几何尺寸的参数化反而更加繁琐；

2、程序参数化已不允许在模型中添加太多的Tie，因此不同零部件的绑定直接通过共节点来进行，这就要求建模方法与常规的建模方法有所区别。思路如下：

将一个整机拆成几个大的Part来建立，一个Part中包含许多零件，这样在划分网格式时就可以自动实现共节点的绑定。不同的零件可通过建立不同的Set来进行区分，不同Part的绑定可以通过Tie来实现。将一个复杂的结构拆成几个恰当的Part来建立，一方面可以将复杂的模型简单化，使建立复杂模型成为可能；另一方面，不同的Part可单独调用，从而又可实现程序的模块化，增加程序的适应范围，延长程序的使用寿命，也方便后期程序的维护和修改。

3、通过py文件建立起的模型要进行参数优化，已不适合采用Isight中Abaqus模块，需要用到Isight的Simcode模块。

下面详细解释一个臂架的py文件。

#此程序用来绘制臂架前段

#导入相关模块

# -*- coding: mbcs -*-

from abaqus import *

from abaqusConstants import *

#定义整个臂架的长、宽、高

L0=14300

W0=1650

H0=800

#创建零件P01_12

L1=H0+200

W1=200

T1=12

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=2000.0)

g, v, d, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=STANDALONE)

s.rectangle(point1=(W0/2, L1/2), point2=(W0/2+W1, -L1/2))

s.rectangle(point1=(-W0/2, L1/2), point2=(-W0/2-W1, -L1/2))

p = mdb.models['Model-1'].Part(name='Part-1', dimensionality=THREE_D,

type=DEFORMABLE_BODY)

p = mdb.models['Model-1'].parts['Part-1']

p.BaseShell(sketch=s)

session.viewports['Viewport: 1'].setValues(displayedObject=p)

del mdb.models['Model-1'].sketches['__profile__']

#定义零件的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

pickedFaces01 = f.findAt(((W0/2, L1/2, 0),),((-W0/2, L1/2, 0),), )

p.assignThickness(faces=pickedFaces01, thickness=T1)

p.Set(faces=pickedFaces01, name='P01_12')

#创建辅助平面和辅助坐标系

p = mdb.models['Model-1'].parts['Part-1']

p.DatumCsysByThreePoints(name='Datum csys-1', coordSysType=CARTESIAN, origin=(

0.0, 0.0, 0.0), line1=(1.0, 0.0, 0.0), line2=(0.0, 1.0, 0.0))

p = mdb.models['Model-1'].parts['Part-1']

p.DatumPlaneByPrincipalPlane(principalPlane=XYPLANE, offset=L0)

#创建零件P02_12

L2=L1

W2=W1

T2=12

p = mdb.models['Model-1'].parts['Part-1']

d = p.datums

#将草图原点参数化

t = p.MakeSketchTransform(sketchPlane=d[5], sketchUpEdge=d[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, origin=(0.0, 0.0, L0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=29006.85, gridSpacing=725.17, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

s.rectangle(point1=(W0/2, L2/2), point2=(W0/2+W2, -L2/2))

s.rectangle(point1=(-W0/2, L2/2), point2=(-W0/2-W2, -L2/2))

p = mdb.models['Model-1'].parts['Part-1']

d2 = p.datums

p.Shell(sketchPlane=d2[5], sketchUpEdge=d2[4].axis2, sketchPlaneSide=SIDE1,

sketchOrientation=RIGHT, sketch=s)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#定义零件的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

pickedFaces02 = f.findAt(((W0/2, L1/2, L0),),((-W0/2, L1/2, L0),), )

p.assignThickness(faces=pickedFaces02, thickness=T2)

p.Set(faces=pickedFaces02, name='P02_12')

#创建零件P03_12和零件P04_08

T3=12

T4=8

p = mdb.models['Model-1'].parts['Part-1']

d = p.datums

t = p.MakeSketchTransform(sketchPlane=d[5], sketchUpEdge=d[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, origin=(0.0, 0.0, L0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=29006.85, gridSpacing=725.17, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

#创建草图

p = mdb.models['Model-1'].parts['Part-1']

s.Line(point1=(-W0/2-W1, H0/2), point2=(-W0/2, H0/2))

s.Line(point1=(W0/2, H0/2), point2=(W0/2+W1, H0/2))

s.Line(point1=(-W0/2-W1, -H0/2), point2=(-W0/2, -H0/2))

s.Line(point1=(W0/2, -H0/2), point2=(W0/2+W1, -H0/2))

p = mdb.models['Model-1'].parts['Part-1']

d2 = p.datums

p.ShellExtrude(sketchPlane=d2[5], sketchUpEdge=d2[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, sketch=s, depth=L0,

flipExtrudeDirection=ON)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#定义零件P03_12的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

pickedFaces03 = f.findAt(((-W0/2, H0/2, L0/2),),((W0/2, H0/2, L0/2),),)

p.assignThickness(faces=pickedFaces03, thickness=T3)

p.Set(faces=pickedFaces03, name='P03_12')

#定义零件P04_12的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

pickedFaces04 = f.findAt(((-W0/2, -H0/2, L0/2),),((W0/2, -H0/2, L0/2),),)

p.assignThickness(faces=pickedFaces04, thickness=T4)

p.Set(faces=pickedFaces04, name='P04_12')

#创建零件P05_08

T5=8

p = mdb.models['Model-1'].parts['Part-1']

d = p.datums

t = p.MakeSketchTransform(sketchPlane=d[5], sketchUpEdge=d[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, origin=(0.0, 0.0, L0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=29006.85, gridSpacing=725.17, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

s.Line(point1=(-W0/2-W1/2, H0/2), point2=(-W0/2-W1/2, -H0/2))

s.Line(point1=(W0/2+W1/2, H0/2), point2=(W0/2+W1/2, -H0/2))

p = mdb.models['Model-1'].parts['Part-1']

d2 = p.datums

p.ShellExtrude(sketchPlane=d2[5], sketchUpEdge=d2[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, sketch=s, depth=L0,

flipExtrudeDirection=ON)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#定义零件P05_8的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

pickedFaces05 = f.findAt(((-W0/2-W1/2, 0, L0/2),),((W0/2+W1/2, 0, L0/2),),)

p.assignThickness(faces=pickedFaces05, thickness=T5)

p.Set(faces=pickedFaces05, name='P05_08')

#创建零件P06_08

L6=W0+W1

n=L0//2520+1

T6=8

p = mdb.models['Model-1'].parts['Part-1']

f, d = p.faces, p.datums

t = p.MakeSketchTransform(sketchPlane=f[0], sketchUpEdge=d[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, origin=(W0/2+W1/2, -H0/2,

0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=28684, gridSpacing=717, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

#循环命令绘制平行隔板

for i in range(0,n):

s.Line(point1=(-500-(i*2520), H0), point2=(-500-(i*2520), 0.0))

p = mdb.models['Model-1'].parts['Part-1']

f1, d2 = p.faces, p.datums

p.ShellExtrude(sketchPlane=f1[0], sketchUpEdge=d2[4].axis2,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, sketch=s, depth=L6,

flipExtrudeDirection=ON)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#定义零件P06_08的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

for i in range(0,n):

pickedFaces = f.findAt(((0, H0/4, 500+i*2520),))

p.assignThickness(faces=pickedFaces, thickness=T6)

p.Set(faces=pickedFaces, name='P06_08_'+str(1+i))

#创建零件P07_12,P08_12

W7=200

L7=W0+W1

T7=12

T8=12

p = mdb.models['Model-1'].parts['Part-1']

f, e = p.faces, p.edges

t = p.MakeSketchTransform(

sketchPlane=f.findAt(coordinates=(W0/2+W1/2, 0.0, 100.0)),

sketchUpEdge=e.findAt(coordinates=(W0/2+W1/2, 0.0, 0.0)),

sketchOrientation=RIGHT,sketchPlaneSide=SIDE1,

origin=(W0/2+W1/2, -H0/2, 0.0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=53678, gridSpacing=1341, transform=t)

g, v, d, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

#循环命令绘制平行隔板

for i in range(0,n):

s.Line(point1=(400+i*2520, -H0), point2=(600+i*2520, -H0))

s.Line(point1=(400+i*2520, 0), point2=(600+i*2520, 0))

p = mdb.models['Model-1'].parts['Part-1']

f1, e1 = p.faces, p.edges

p.ShellExtrude(

sketchPlane=f.findAt(coordinates=(W0/2+W1/2, 0.0, 100.0)),

sketchUpEdge=e.findAt(coordinates=(W0/2+W1/2, 0.0, 0.0)),

sketchPlaneSide=SIDE1,

sketchOrientation=RIGHT, sketch=s, depth=W0+W1, flipExtrudeDirection=ON,

keepInternalBoundaries=ON)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#定义零件P07_12的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

for i in range(0,n):

pickedFaces07 = f.findAt(((0, H0/2, 400+i*2520),),((0, H0/2, 600+i*2520),),)

p.assignThickness(faces=pickedFaces07, thickness=T7)

p.Set(faces=pickedFaces07, name='P07_12_'+str(1+i))

#定义耦合set

fp=[]

for i in range(0,2):

fp.append(f.findAt(((0, H0/2, 400+i*2520),),((0, H0/2, 600+i*2520),),))

p.Set(faces=fp, name='P07_fp')

#定义零件P08_12的厚度

p = mdb.models['Model-1'].parts['Part-1']

f = p.faces

for i in range(0,n):

pickedFaces08 = f.findAt(((0, -H0/2, 400+i*2520),),((0, -H0/2, 600+i*2520),),)

p.assignThickness(faces=pickedFaces08, thickness=T7)

p.Set(faces=pickedFaces08, name='P08_12_'+str(1+i))

#为中间隔板创建空腔

#定义相关参数边界距离、圆角

d0=100

r0=100

p = mdb.models['Model-1'].parts['Part-1']

f1, e1 = p.faces, p.edges

t = p.MakeSketchTransform(

f.findAt(coordinates=(0, 0.0, 500.0)),

sketchUpEdge=e.findAt(coordinates=(W0/2+W1/2, 0.0, 500.0)),

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT,

origin=(0.0, 0.0, 500.0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=5910.0, gridSpacing=147.0, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

p.projectReferencesOntoSketch(sketch=s, filter=COPLANAR_EDGES)

#创建矩形

s.rectangle(point1=(-W0/2-W1/2+d0, H0/2-d0), point2=(W0/2+W1/2-d0, -H0/2+d0))

#创建圆角

s.FilletByRadius(radius=r0, curve1=g[29], nearPoint1=(-W0/2-W1/2+d0,

H0/2-d0), curve2=g[26], nearPoint2=(-W0/2-W1/2+d0, H0/2-d0))

s.FilletByRadius(radius=r0, curve1=g[26], nearPoint1=(-W0/2-W1/2+d0,

-H0/2+d0), curve2=g[27], nearPoint2=(-W0/2-W1/2+d0, -H0/2+d0))

s.FilletByRadius(radius=r0, curve1=g[27], nearPoint1=(W0/2+W1/2-d0,

-H0/2+d0), curve2=g[28], nearPoint2=(W0/2+W1/2-d0, -H0/2+d0))

s.FilletByRadius(radius=r0, curve1=g[28], nearPoint1=(W0/2+W1/2-d0,

H0/2-d0), curve2=g[29], nearPoint2=(W0/2+W1/2-d0, H0/2-d0))

p = mdb.models['Model-1'].parts['Part-1']

f1, d2 = p.faces, p.datums

p.CutExtrude(

f.findAt(coordinates=(0, 0.0, 500.0)),

sketchUpEdge=e.findAt(coordinates=(W0/2+W1/2, 0.0, 500.0)),

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, sketch=s, depth=L0,

flipExtrudeDirection=OFF)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

#开始建立梁Beam_1

p = mdb.models['Model-1'].parts['Part-1']

f, d = p.faces, p.datums

#绘制参考面

p.DatumPlaneByOffset(plane=f.findAt(coordinates=

(W0/2, -H0/2, 100.0)),flip=SIDE2, offset=8.0)

dp1 = d.keys()[-1]

p = mdb.models['Model-1'].parts['Part-1']

d = p.datums

t = p.MakeSketchTransform(sketchPlane=d[dp1], sketchUpEdge=d[4].axis1,

sketchPlaneSide=SIDE1, sketchOrientation=RIGHT, origin=(0.0, 0.0,

0.0))

s = mdb.models['Model-1'].ConstrainedSketch(name='__profile__',

sheetSize=31857.0, gridSpacing=796.0, transform=t)

g, v, d1, c = s.geometry, s.vertices, s.dimensions, s.constraints

s.setPrimaryObject(option=SUPERIMPOSE)

p = mdb.models['Model-1'].parts['Part-1']

#计算中间加强梁的数量

if n%2==1:

n1=n//2

n2=n//2

else:

n1=n//2

n2=n//2-1

for i in range(0,n1):

s.Line(point1=(-500-i*2520*2, W0/2+W1/2), point2=(-500-2520-i*2520*2,-W0/2-W1/2 ))

for i in range(0,n2):

s.Line(point1=(-500-2520-i*2520*2,-W0/2-W1/2), point2=(-500-2*2520-i*2520*2,W0/2+W1/2 ))

#在基准平面dp1上面绘制梁

p = mdb.models['Model-1'].parts['Part-1']

d2 = p.datums

e = p.edges

p.Wire(sketchPlane=d2[dp1], sketchUpEdge=d2[4].axis1, sketchPlaneSide=SIDE1,

sketchOrientation=RIGHT, sketch=s)

s.unsetPrimaryObject()

del mdb.models['Model-1'].sketches['__profile__']

edges1=[]

for i in range(0,n-1):

edges1.append(e.findAt(((0, -H0/2-8, 500+2520/2+i*2520),),))

p.Set(edges=edges1, name='Beam_1')

###########################

#开始定义有限元分析的相关参数

#定义材料

mdb.models['Model-1'].Material(name='steel')

mdb.models['Model-1'].materials['steel'].Elastic(table=((210000.0, 0.3), ))

mdb.models['Model-1'].materials['steel'].Density(table=((7.8e-06, ), ))

#定义壳单元属性

mdb.models['Model-1'].HomogeneousShellSection(name='shell', preIntegrate=OFF,

material='steel', thicknessType=UNIFORM, thickness=10.0, thicknessField='',

idealization=NO_IDEALIZATION, poissonDefinition=DEFAULT,

thicknessModulus=None, temperature=GRADIENT, useDensity=OFF,

integrationRule=SIMPSON, numIntPts=5)

#赋所有壳单元属性

p = mdb.models['Model-1'].parts['Part-1']

for i in range(1,5):

region1 = p.sets['P0'+str(i)+'_12']

p.SectionAssignment(region=region1, sectionName='shell', offset=0.0,

offsetType=FROM_GEOMETRY, offsetField='',

thicknessAssignment=FROM_GEOMETRY)

region2 = p.sets['P05_08']

p.SectionAssignment(region=region2, sectionName='shell', offset=0.0,

offsetType=FROM_GEOMETRY, offsetField='',

thicknessAssignment=FROM_GEOMETRY)

for i in range(1,n+1):

region3 = p.sets['P06_08_'+str(i)]

p.SectionAssignment(region=region3, sectionName='shell', offset=0.0,

offsetType=FROM_GEOMETRY, offsetField='',

thicknessAssignment=FROM_GEOMETRY)

for i in range(1,n+1):

region4 = p.sets['P07_12_'+str(i)]

p.SectionAssignment(region=region4, sectionName='shell', offset=0.0,

offsetType=FROM_GEOMETRY, offsetField='',

thicknessAssignment=FROM_GEOMETRY)

for i in range(1,n+1):

region5 = p.sets['P08_12_'+str(i)]

p.SectionAssignment(region=region5, sectionName='shell', offset=0.0,

offsetType=FROM_GEOMETRY, offsetField='',

thicknessAssignment=FROM_GEOMETRY)

#定义梁单元属性

mdb.models['Model-1'].LProfile(name='L_65', a=65.0, b=65.0, t1=7.0, t2=7.0)

mdb.models['Model-1'].BeamSection(name='B_65', integration=DURING_ANALYSIS,

poissonRatio=0.0, profile='L_65', material='steel', temperatureVar=LINEAR,

consistentMassMatrix=False)

#赋所有梁单元属性

p = mdb.models['Model-1'].parts['Part-1']

region = p.sets['Beam_1']

p.SectionAssignment(region=region, sectionName='B_65', offset=0.0,

offsetType=MIDDLE_SURFACE, offsetField='',

thicknessAssignment=FROM_SECTION)

p.assignBeamSectionOrientation(region=region, method=N1_COSINES, n1=(0.0, 0.0,

-1.0))

#定义装配体

import assembly

a = mdb.models['Model-1'].rootAssembly

a.DatumCsysByDefault(CARTESIAN)

p = mdb.models['Model-1'].parts['Part-1']

a.Instance(name='Part-1-1', part=p, dependent=ON)

#定义分析步

import step

mdb.models['Model-1'].StaticStep(name='Step-1', previous='Initial')

#定义底面与梁的tied

import interaction

a = mdb.models['Model-1'].rootAssembly

region1=a.instances['Part-1-1'].sets['P04_12']

region2=a.instances['Part-1-1'].sets['Beam_1']

mdb.models['Model-1'].Tie(name='Constraint-1', master=region1, slave=region2,

positionToleranceMethod=COMPUTED, adjust=OFF, tieRotations=ON, thickness=ON)

#开始定义耦合

#导入相关模块

import regionToolset

a = mdb.models['Model-1'].rootAssembly

d, r = a.datums, a.referencePoints

#定义参考点

a.ReferencePoint(point=(0.0, H0/2, 500+2520/2))

r1 = a.referencePoints

rp1 = r.keys()[-1]

refPoints1=(r1[rp1], )

region1=regionToolset.Region(referencePoints=refPoints1)

s1 = a.instances['Part-1-1'].faces

region2 = a.instances['Part-1-1'].sets['P07_fp']

mdb.models['Model-1'].Coupling(name='Constraint-2', controlPoint=region1,

surface=region2, influenceRadius=WHOLE_SURFACE, couplingType=DISTRIBUTING,

localCsys=None, u1=ON, u2=ON, u3=ON, ur1=ON, ur2=ON, ur3=ON)

########################

#定义边界条件

import load

a = mdb.models['Model-1'].rootAssembly

d, r = a.datums, a.referencePoints

region = a.instances['Part-1-1'].sets['P02_12']

mdb.models['Model-1'].DisplacementBC(name='SPC', createStepName='Initial',

region=region, u1=SET, u2=SET, u3=SET, ur1=SET, ur2=SET, ur3=SET,

amplitude=UNSET, distributionType=UNIFORM, fieldName='', localCsys=None)

a = mdb.models['Model-1'].rootAssembly

region = a.instances['Part-1-1'].sets['P08_12_'+str(n-1)]

mdb.models['Model-1'].DisplacementBC(name='SPC2', createStepName='Initial',

region=region, u1=SET, u2=SET, u3=SET, ur1=SET, ur2=SET, ur3=SET,

amplitude=UNSET, distributionType=UNIFORM, fieldName='', localCsys=None)

r1 = a.referencePoints

refPoints1=(r1[rp1], )

region = regionToolset.Region(referencePoints=refPoints1)

mdb.models['Model-1'].ConcentratedForce(name='force', createStepName='Step-1',

region=region, cf2=-10000.0, distributionType=UNIFORM, field='',

localCsys=None)

mdb.models['Model-1'].Gravity(name='G', createStepName='Step-1', comp2=-9.8,

distributionType=UNIFORM, field='')

################

#划分网格

import mesh

p = mdb.models['Model-1'].parts['Part-1']

p.seedPart(size=20.0, deviationFactor=0.1, minSizeFactor=0.1)

p.generateMesh()

a = mdb.models['Model-1'].rootAssembly

##############

#创建作业并提交分析

import job

mdb.Job(name='006', model='Model-1', description='', type=ANALYSIS,

atTime=None, waitMinutes=0, waitHours=0, queue=None, memory=90,

memoryUnits=PERCENTAGE, getMemoryFromAnalysis=True,

explicitPrecision=SINGLE, nodalOutputPrecision=SINGLE, echoPrint=OFF,

modelPrint=OFF, contactPrint=OFF, historyPrint=OFF, userSubroutine='',

scratch='', multiprocessingMode=DEFAULT, numCpus=4, numDomains=4)

mdb.jobs['006'].submit(consistencyChecking=ON)

mdb.jobs['006'].waitForCompletion()

##############

#进入后处理模块

import visualization

o3 = session.openOdb(name='F:/ABAQUS/006.odb')

session.viewports['Viewport: 1'].setValues(displayedObject=o3)

session.viewports['Viewport: 1'].odbDisplay.display.setValues(plotState=(

CONTOURS_ON_DEF, ))

session.viewports['Viewport: 1'].view.setValues(session.views['Iso'])

mdb.saveAs(pathName='F:/ABAQUS/006.cae')

ABAQUS结构CAE显式动力学及仿真

基于Python的Abaqus二次开发实例讲解的评论3条

发布

啦咯啦咯啦咯啦咯啦咯 2021年5月30日

0 0

请问楼主知道比如定义一个变量 a=3以后再定义 b=2×a+4会报错(错误原因是 b没有被定义) 的原因吗😅

回复
中沫工师-小周 2020年10月12日

0 0

很不错

回复

基于Python的Abaqus二次开发实例讲解的相关视频课程

基于Python的Abaqus二次开发实例讲解的相关案例教程

Abaqus里应用Python的一些技巧附Python语言在Abaqus中的应用文档下载 2022-05-06

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 '].Co

星辰技文|一步步教你如何使用35行代码生成ABAQUS二维随机颗粒模型 2023-07-13

前面推荐了一些ABAQUS二次开发小工具，不知道大家是否已经安装使用。后面以一些小案例带大家熟悉ABAQUS前后处理相关的Python库，以及使用技巧。星哥开发的插件大多集中在非均质相关断裂问题，相信关注公众号的很多朋友也都是做这方面，那么我们从最初始的非均质几何模型的案例出发，来演示一个随机颗粒模型的代码编写的全过程，效果如下所示：在这个案例中，最大的帮手是PythonReader,它能让

Python二次开发——findAt方法的正确食用方法 2021-11-29

在讲解 findAt（）方法之前，先让我们简单回顾一下Abaqus中需要指定区域（region）的情况吧~ Load命令：使用region参数指定施加荷载的区域 Mesh命令：使用region参数指定单元类型、网格种子的定义区域 Set命令：使用region参数定义节点集、单元集当我们在CAE中建立模型后，软件会自动为他们进行编号，如节点编号、单元编号、各条边等，如果我们在编写脚本的时候选用模

abaqus Python 简单梁的例子 2021-12-17

from abaqus import * from abaqusConstants import * backwardCompatibility.setValues(includeDeprecated=True,reportDeprecated=False) # Create a model. myModel = mdb.Model(name='Beam') # Create a new view

走进abaqus gui开发(4)--新建插件程序 2022-06-05

前言 Python具有以下特点。Python语言是一种动态解释型编程语言,其功能强大,简单易学,支持面向对象编程(（object-oriented programming)，虽然由于其动态性致使程序解释执行速度比编译语言慢,但是随着Python语言的不断优化以及计算机硬件的迅猛发展，Python语言将会受到越来越多用户的关注。Python具有开源、自由等特征。它的简洁性和易用性使程序的开发过程变得

铺就函授

关注

影响力

粉丝

NaN

内容

获赞

项目客服

培训客服

铺就函授

关注

3 3 8