''' ----------------------------------------------------------------------------- Two dimensional submodel symmetric double edged notch specimen (elastic plastic material) modeled using hybrid reduced integration plane stress elements (CPE8RH). First the global model job is completed. The *.odb file from the global model is used to drive this submodel. Global model scripts to be run: 2DDoubleEdPlasGlCPE8RH_model.py and 2DDoubleEdPlasGlCPE8RH_job.py ----------------------------------------------------------------------------- ''' from abaqus import * import testUtils testUtils.setBackwardCompatibility() from abaqusConstants import * import part, material, section, assembly, step, interaction import regionToolset, displayGroupMdbToolset as dgm, mesh, load, job #---------------------------------------------------------------------------- # Copy the global model into a new model Mdb() globalModelName = '2DDoubleEdPlasGlCPE8RH' openMdb(globalModelName) subModelName = '2DDoubleEdPlasSubCPE8RH' mySubModel = mdb.Model(name=subModelName) mySubModel = (mdb.Model(name=subModelName, objectToCopy=mdb.models[globalModelName])) # Create a new viewport in which to display the model # and the results of the analysis. myAssembly = mySubModel.rootAssembly myViewport = session.viewports['Viewport: 1'] myViewport.setValues(displayedObject=myAssembly) myViewport.makeCurrent() myViewport.maximize() #--------------------------------------------------------------------------- # Edit the model attributes to refer to the global model ODB file # to drive the sub model. mySubModel.setValues(description='Double edged notch specimen submodel', globalJob='2DDoubleEdPlasGlCPE8RH.odb') #--------------------------------------------------------------------------- # Create the sub model section of the global model # Create a sketch for the base feature myPlate = mySubModel.parts['Plate'] myViewport.setValues(displayedObject=myPlate) mySubSketch = mySubModel.Sketch(name='plateProfile',sheetSize=200.0) mySubSketch.sketchOptions.setValues(viewStyle=REGULAR) mySubSketch.setPrimaryObject(option=STANDALONE) mySubSketch.rectangle(point1=(0.0,0.0), point2=(20.0,10.0)) mySubPlate = mySubModel.Part(name='subPlate', dimensionality=TWO_D_PLANAR, type=DEFORMABLE_BODY) mySubPlate.BaseShell(sketch=mySubSketch) mySubSketch.unsetPrimaryObject() del mySubModel.sketches['plateProfile'] myViewport.setValues(displayedObject=mySubPlate) # Create a set referring to the whole part faces = mySubPlate.faces.findAt(((10,2.5,0),)) mySubPlate.Set(faces=faces, name='subAll') #--------------------------------------------------------------------------- # Assign material properties del mySubModel.materials['ElasticMaterial'] mySubModel.Material(name='A1') mySubModel.materials['A1'].Elastic(table=((30000000.0, 0.3), )) mySubModel.materials['A1'].Plastic(table=((40000.0,0.0), (60000.0,0.0085))) mySubModel.sections['SolidHomogeneous'].setValues(material='A1', thickness=1.0) region = mySubPlate.sets['subAll'] mySubPlate.SectionAssignment(region=region, sectionName='SolidHomogeneous') #--------------------------------------------------------------------------- # Create an assembly # Place the plate created above at the same position as in the # global model. Then the instance of the full plate is deleted. myViewport.setValues(displayedObject=myAssembly) myAssembly.Instance(name='subPlate-1', part=mySubPlate, dependent=OFF) mySubPlateInstance = myAssembly.instances['subPlate-1'] del myAssembly.features['myPlate-1'] # Partition the edge at t=0.5 pickedEdges = mySubPlateInstance.edges.findAt((9,0,0)) myAssembly.PartitionEdgeByParam(edges=pickedEdges, parameter=0.5) # Partition the instance for sweep meshing face1 = mySubPlateInstance.faces.findAt((10,5,0)) t = myAssembly.MakeSketchTransform(sketchPlane=face1, sketchPlaneSide=SIDE1, origin=(10.0, 5.0, 0.0)) mySketch = mySubModel.Sketch(name='partitionProfile', sheetSize=44.72, gridSpacing=1.11, transform=t) mySketch.setPrimaryObject(option=SUPERIMPOSE) myAssembly.projectReferencesOntoSketch(sketch=mySketch, filter=COPLANAR_EDGES) r1 = mySketch.referenceVertices mySketch.sketchOptions.setValues(gridOrigin=(0.0,-5.0)) mySketch.ArcByCenterEnds(center=(0.0,-5.0), point1=(5.0,-5.0), point2=(-5.0,-5.0), direction=COUNTERCLOCKWISE) mySketch.Line(point1=(0.0,-5.0), point2=(10.0,5.0)) mySketch.Line(point1=(0.0,-5.0), point2=(-10.0,5.0)) mySketch.constraintReferences(vertex1=r1.findAt((0.0,-5.0),1)) faces = mySubPlateInstance.faces pickedFaces = faces[face1.index:(face1.index+1)] myAssembly.PartitionFaceBySketch(faces=pickedFaces, sketch=mySketch) mySketch.unsetPrimaryObject() del mySubModel.sketches['partitionProfile'] # Delete all the sets/BCs/Loads/step/crack properties # created for the global model del mySubModel.steps['ApplyLoad'] #del myAssembly.sets['Monitor'] del myAssembly.sets['crackTip'] del myAssembly.sets['xEdge'] del myAssembly.sets['yEdge'] del myAssembly.surfaces['topSurf'] del myAssembly.engineeringFeatures.cracks['Crack'] del mySubModel.boundaryConditions['xFixed'] del mySubModel.boundaryConditions['yFixed'] # Create a set for the crack tip verts = mySubPlateInstance.vertices v1 = mySubPlateInstance.vertices.findAt((10,0,0)) verts1 = verts[v1.index:(v1.index+1)] myAssembly.Set(vertices=verts1, name='subCrackTip') # Create a set for the X edge of the plate edges = mySubPlateInstance.edges e1 = mySubPlateInstance.edges.findAt(((2.5,0,0),), ((7.5,0.,0.),),) myAssembly.Set(edges=e1, name='subXEdge') # Create a set for the Y edge of the plate edges = mySubPlateInstance.edges e1 = mySubPlateInstance.edges.findAt(((0,5,0),),) myAssembly.Set(edges=e1, name='subYEdge') # Create a set for the sub modeling boundary e1 = mySubPlateInstance.edges.findAt((10,10,0)) e1 = edges[e1.index:(e1.index+1)] myAssembly.Set(edges=e1, name='drivenBoundary') #--------------------------------------------------------------------------- # Create a step mySubModel.StaticStep(name='subApplyLoad', previous='Initial', description='Drive the submodel') #--------------------------------------------------------------------------- # Create interaction properties # Create the contour integral definition for the crack crackFront = crackTip = myAssembly.sets['subCrackTip'] verts = mySubPlateInstance.vertices v1 = mySubPlateInstance.vertices.findAt((10,0,0)) v2 = mySubPlateInstance.vertices.findAt((0,0,0)) myAssembly.engineeringFeatures.ContourIntegral(name='subCrack', symmetric=ON, crackFront=crackFront, crackTip=crackTip, extensionDirectionMethod=Q_VECTORS, qVectors=((v1,v2),), midNodePosition=0.25, collapsedElementAtTip=SINGLE_NODE) #--------------------------------------------------------------------------- # Create loads and boundary conditions # Create a boundary condition for X edge to be fixed in Y region = myAssembly.sets['subXEdge'] mySubModel.DisplacementBC(name='subYFixed', createStepName='Initial', region=region, u2=SET, distributionType=UNIFORM, localCsys=None) region = myAssembly.sets['subYEdge'] mySubModel.DisplacementBC(name='subXFixed', createStepName='Initial', region=region, u1=SET, distributionType=UNIFORM, localCsys=None) # Create the sub modeling boundary condition region = myAssembly.sets['drivenBoundary'] mySubModel.SubmodelBC(name='subBC', createStepName='subApplyLoad', region=region, globalStep='1', globalIncrement=0, timeScale=OFF, dof=(1, 2), globalDrivingRegion='', absoluteExteriorTolerance=0.0, exteriorTolerance=0.05) #--------------------------------------------------------------------------- # Create a mesh # Seed all the edges pickedEdges1 = mySubPlateInstance.edges.findAt(((10.789162,0.,0.),),) pickedEdges2 = mySubPlateInstance.edges.findAt(((10.526264,0.526264,0.),),) myAssembly.seedEdgeByBias(end1Edges=pickedEdges1, end2Edges=pickedEdges2, ratio=3.0, number=6, constraint=FIXED) pickedEdges2 = mySubPlateInstance.edges.findAt(((9.194185,0.,0.),),) pickedEdges1 = mySubPlateInstance.edges.findAt(((9.473736,0.526264,0.),),) myAssembly.seedEdgeByBias(end1Edges=pickedEdges1, end2Edges=pickedEdges2, ratio=3.0, number=6, constraint=FIXED) pickedEdges = mySubPlateInstance.edges.findAt(((3.617743,0.,0.),), ((5.23299,4.76701,0.),), ((14.237743,4.237743,0.),), ((15.741623,0.,0.),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=2, constraint=FIXED) pickedEdges = mySubPlateInstance.edges.findAt(((5.380602,1.913417,0.),), ((0.,5.,0.),), ((20.,5.,0.),), ((14.619398,1.913417,0.),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=3, constraint=FIXED) pickedEdges = mySubPlateInstance.edges.findAt(((10.,5.,0.),), ((10.,10.,0.),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=6, constraint=FIXED) # Assign meshing controls to the respective regions pickedRegions = mySubPlateInstance.faces.findAt(((8.649209,0.450264,0.),), ((10.,0.900527,0.),), ((11.350791,0.450263,0.),),) myAssembly.setMeshControls(regions=pickedRegions, elemShape=QUAD_DOMINATED, technique=SWEEP) pickedRegions = mySubPlateInstance.faces.findAt(((9.805735,5.959446,0.),), ((16.54391,1.931576,0.),), ((4.425367,2.383505,0.),),) myAssembly.setMeshControls(regions=pickedRegions, elemShape=QUAD, technique=STRUCTURED) elemType1 = mesh.ElemType(elemCode=CPE8RH, elemLibrary=STANDARD) elemType2 = mesh.ElemType(elemCode=CPE6M, elemLibrary=STANDARD) faces1 = mySubPlateInstance.faces pickedRegions =(faces1, ) myAssembly.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2)) partInstances =(mySubPlateInstance, ) myAssembly.generateMesh(regions=partInstances) #--------------------------------------------------------------------------- # Request history output for the crack mySubModel.historyOutputRequests.changeKey(fromName='H-Output-1', toName='JInt') mySubModel.historyOutputRequests['JInt'].setValues(contourIntegral='subCrack', numberOfContours=6) #--------------------------------------------------------------------------- # Create the job myJob = mdb.Job(name=subModelName, model=subModelName, description='Contour integral analysis') mdb.saveAs(pathName=subModelName) #---------------------------------------------------------------------------