基于Python的Abaqus二次开发实例讲解

基于Python的Abaqus二次开发实例讲解（asian58 2013.6.26）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=14300W0=1650H0=800#创建零件P01_12 L1=H0+200 W1=200 T1=12s = 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=12p = 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.datumsp.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'] Array f = p.facespickedFaces02 = 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_08T3=12T4=8p = mdb.models['Model-1'].parts['Part-1']d = p.datumst = 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.constraintss.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.datumsp.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.facespickedFaces03 = 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.facespickedFaces04 = 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_08T5=8p = mdb.models['Model-1'].parts['Part-1']d = p.datumst = 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.constraintss.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.datumsp.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.facespickedFaces05 = 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_08L6=W0+W1n=L0//2520+1T6=8p = mdb.models['Model-1'].parts['Part-1']f, d = p.faces, p.datumst = 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.constraintss.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): Array 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.datumsp.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.facesfor i in range(0,n): Array 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_12W7=200L7=W0+W1T7=12T8=12p = mdb.models['Model-1'].parts['Part-1']f, e = p.faces, p.edgest = 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.constraintss.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.edgesp.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.facesfor 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))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.facesfor 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=100r0=100p = mdb.models['Model-1'].parts['Part-1']f1, e1 = p.faces, p.edgest = 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.constraintss.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.datumsp.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_1p = 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.datumst = 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.constraintss.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.edgesp.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): Array 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 assemblya = mdb.models['Model-1'].rootAssemblya.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 stepmdb.models['Model-1'].StaticStep(name='Step-1', previous='Initial')#定义底面与梁的tiedimport interactiona = mdb.models['Model-1'].rootAssemblyregion1=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 regionToolseta = mdb.models['Model-1'].rootAssemblyd, r = a.datums, a.referencePoints#定义参考点a.ReferencePoint(point=(0.0, H0/2, 500+2520/2))rp1 = r.keys()[-1]refPoints1=(r1[rp1], )region1=regionToolset.Region(referencePoints=refPoints1)s1 = a.instances['Part-1-1'].facesregion2 = 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 loada = mdb.models['Model-1'].rootAssemblyd, r = a.datums, a.referencePointsregion = 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'].rootAssemblyregion = 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.referencePointsrefPoints1=(r1[rp1], )region = regionToolset.Region(referencePoints=refPoints1)mdb.models['Model-1'].ConcentratedForce(name='force', createStepName='Step-1',海外最大专业学习论坛-- mechbbs论坛网址：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 meshp = 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 jobmdb.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 visualizationo3 = 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')第11 页共11 页。