''' ----------------------------------------------------------------------------- Two dimensional submodel of a single edged notch specimen (linear elastic material) modeled using plane strain elements (CPE8). 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: 2DSingleEdSymmGlCPE8_model.py and 2DSingleEdSymmGlCPE8_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 = '2DSingleEdSymmGlCPE8' openMdb(globalModelName) subModelName = '2DSingleEdSymmSubCPE8' 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='Single edged notch specimen submodel', globalJob='2DSingleEdSymmGlCPE8.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.ArcByCenterEnds(center=(10.0,0.0), point1=(15.0,0.0), point2=(5.0,0.0), direction=COUNTERCLOCKWISE) mySubSketch.Line(point1=(5.0,0.0), point2=(15.0,0.0)) 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 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) # Delete all the sets/BCs/Loads/step/crack properties # created for the global model del myAssembly.sets['crackTip'] del myAssembly.sets['fixedEdge'] del myAssembly.sets['fixedPt'] del myAssembly.surfaces['loadSurf'] del mySubModel.steps['LoadPlate'] del myAssembly.engineeringFeatures.cracks['Crack'] del mySubModel.boundaryConditions['FixedInX'] del mySubModel.boundaryConditions['FixedInY'] # 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((12.5,0,0)) e1 = edges[e1.index:(e1.index+1)] myAssembly.Set(edges=e1, name='subXEdge') # Create a set for the sub modeling boundary e1 = mySubPlateInstance.edges.findAt((10,5,0)) 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((15,0,0)) 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) # 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 edges = mySubPlateInstance.edges pickedEdges1 = mySubPlateInstance.edges.findAt((11,0,0)) pickedEdges2 = mySubPlateInstance.edges.findAt((9,0,0)) pickedEdges1 = edges[pickedEdges1.index:(pickedEdges1.index+1)] pickedEdges2 = edges[pickedEdges2.index:(pickedEdges2.index+1)] myAssembly.seedEdgeByBias(end1Edges=pickedEdges1, end2Edges=pickedEdges2, ratio=3.0, number=6, constraint=FIXED) pickedEdges = mySubPlateInstance.edges.findAt((10,5,0)) pickedEdges = edges[pickedEdges.index:(pickedEdges.index+1)] myAssembly.seedEdgeByNumber(edges=pickedEdges, number=12, constraint=FIXED) # Assign meshing controls to the respective regions faces = mySubPlateInstance.faces f1 = mySubPlateInstance.faces.findAt((10,2.5,0)) pickedRegions = faces[f1.index:(f1.index+1)] myAssembly.setMeshControls(regions=pickedRegions, elemShape=QUAD_DOMINATED, technique=SWEEP) elemType1 = mesh.ElemType(elemCode=CPE8, 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=5) mySubModel.HistoryOutputRequest(name='StressInt', createStepName='subApplyLoad', contourIntegral='subCrack', numberOfContours=5, contourType=K_FACTORS) mySubModel.HistoryOutputRequest(name='Tstr', createStepName='subApplyLoad', contourIntegral='subCrack', numberOfContours=5, contourType=T_STRESS) #--------------------------------------------------------------------------- # Create the job myJob = mdb.Job(name=subModelName, model=subModelName, description='Contour integral analysis') mdb.saveAs(pathName=subModelName) #---------------------------------------------------------------------------