''' ----------------------------------------------------------------------------- Two dimensional symmetric model of a double edged notch specimen (linear elastic material) modeled using plane strain elements (CPE8). ----------------------------------------------------------------------------- ''' from abaqus import * from abaqusConstants import * import part, material, section, assembly, step, interaction import regionToolset, displayGroupMdbToolset as dgm, mesh, load, job #---------------------------------------------------------------------------- # Create a model Mdb() modelName = '2DDoubleEdSymmCPE8' myModel = mdb.Model(name=modelName) # Create a new viewport in which to display the model # and the results of the analysis. myViewport = session.Viewport(name=modelName) myViewport.makeCurrent() myViewport.maximize() #--------------------------------------------------------------------------- # Create a part # Create a sketch for the base feature mySketch = myModel.Sketch(name='plateProfile',sheetSize=200.0) mySketch.sketchOptions.setValues(viewStyle=REGULAR) mySketch.setPrimaryObject(option=STANDALONE) mySketch.rectangle(point1=(0.0, 0.0), point2=(20.0, 50.0)) myPlate = myModel.Part(name='Plate', dimensionality=TWO_D_PLANAR, type=DEFORMABLE_BODY) myPlate.BaseShell(sketch=mySketch) mySketch.unsetPrimaryObject() del myModel.sketches['plateProfile'] myViewport.setValues(displayedObject=myPlate) # Partition the edge on the symmetry plane e1 = myPlate.edges.findAt((10,0,0)) (myPlate.PartitionEdgeByPoint(edge=e1, point=myPlate.InterestingPoint(edge=e1, rule=MIDDLE))) # Create a set referring to the whole part faces = myPlate.faces.findAt(((10,25,0),)) myPlate.Set(faces=faces, name='All') #--------------------------------------------------------------------------- # Assign material properties # Create linear elastic material myModel.Material(name='LinearElastic') myModel.materials['LinearElastic'].Elastic(table=((30000000.0, 0.3), )) myModel.HomogeneousSolidSection(name='SolidHomogeneous', material='LinearElastic', thickness=1.0) region = myPlate.sets['All'] # Assign the above section to the part myPlate.SectionAssignment(region=region, sectionName='SolidHomogeneous') #--------------------------------------------------------------------------- # Create an assembly myAssembly = myModel.rootAssembly myViewport.setValues(displayedObject=myAssembly) myAssembly.DatumCsysByDefault(CARTESIAN) myAssembly.Instance(name='myPlate-1', part=myPlate, dependent=OFF) myPlateInstance = myAssembly.instances['myPlate-1'] # Create a set for the top surface of the plate edges = myPlateInstance.edges side1Edge1 = myPlateInstance.edges.findAt((10,50,0)) side1Edge1 = edges[side1Edge1.index:(side1Edge1.index+1)] myAssembly.Surface(side1Edges=side1Edge1, name='topSurf') # Create circular partitions for sweep mesh around the crack tip face1 = myPlateInstance.faces.findAt((10,25,0),) t = myAssembly.MakeSketchTransform(sketchPlane=face1, sketchPlaneSide=SIDE1, origin=(10.0, 25.0, 0.0)) mySketch = myModel.Sketch(name='plateProfile', sheetSize=107.7, gridSpacing=2.69, transform=t) mySketch.setPrimaryObject(option=SUPERIMPOSE) myAssembly.projectReferencesOntoSketch(sketch=mySketch, filter=COPLANAR_EDGES) r, r1 = mySketch.referenceGeometry, mySketch.referenceVertices mySketch.sketchOptions.setValues(gridOrigin=(0.0,-25.0)) mySketch.ArcByCenterEnds(center=(0.0, -25.0), point1=(5.0,-25.0), point2=(-5.0,-25.0), direction=COUNTERCLOCKWISE) f1 = myPlateInstance.faces pickedFaces = f1[face1.index:(face1.index+1)] myAssembly.PartitionFaceBySketch(faces=pickedFaces, sketch=mySketch) mySketch.unsetPrimaryObject() del myModel.sketches['plateProfile'] # Create a set for the X edge of the plate edges = myPlateInstance.edges e1 = myPlateInstance.edges.findAt((2.5,0,0)) e2 = myPlateInstance.edges.findAt((7.5,0,0)) edge = edges[e1.index:(e1.index+1)] + edges[e2.index:(e2.index+1)] myAssembly.Set(edges=edge, name='xEdge') # Create a set for the Y edge of the plate edges = myPlateInstance.edges edge1 = myPlateInstance.edges.findAt((0,25,0)) edge1 = edges[edge1.index:(edge1.index+1)] myAssembly.Set(edges=edge1, name='yEdge') # Create a set for the crack tip verts1 = myPlateInstance.vertices ver1 = myPlateInstance.vertices.findAt((10,0,0)) ver1 = verts1[ver1.index:(ver1.index+1)] myAssembly.Set(vertices=ver1, name='crackTip') #--------------------------------------------------------------------------- # Create a step for applying a load myModel.StaticStep(name='ApplyLoad', previous='Initial', description='Apply a pressure load') #--------------------------------------------------------------------------- # Create interaction properties # Create the contour integral definition for the crack crackFront = crackTip = myAssembly.sets['crackTip'] verts = myPlateInstance.vertices v1 = myPlateInstance.vertices.findAt((10,0,0)) v2 = myPlateInstance.vertices.findAt((0,0,0)) myAssembly.engineeringFeatures.ContourIntegral(name='Crack', symmetric=ON, crackFront=crackFront, crackTip=crackTip, extensionDirectionMethod=Q_VECTORS, qVectors=((v1,v2),), midNodePosition=0.25, collapsedElementAtTip=SINGLE_NODE) #--------------------------------------------------------------------------- # Create loads and boundary conditions # Assign boundary conditions region = myAssembly.sets['xEdge'] myModel.DisplacementBC(name='yFixed', createStepName='Initial', region=region, u2=SET, distribution=UNIFORM, localCsys=None) region = myAssembly.sets['yEdge'] myModel.DisplacementBC(name='xFixed', createStepName='Initial', region=region, u1=SET, distribution=UNIFORM, localCsys=None) # Assign the loads region = myAssembly.surfaces['topSurf'] myModel.Pressure(name='topLoad', createStepName='ApplyLoad', region=region, distribution=UNIFORM, magnitude=-100.0) #--------------------------------------------------------------------------- # Create a mesh # Seed all the edges e1 = myPlateInstance.edges pickedEdges1 = myPlateInstance.edges.findAt((11,0,0),) pickedEdges2 = myPlateInstance.edges.findAt((9,0,0),) pickedEdges1 = e1[pickedEdges1.index:(pickedEdges1.index+1)] pickedEdges2 = e1[pickedEdges2.index:(pickedEdges2.index+1)] myAssembly.seedEdgeByBias(end1Edges=pickedEdges1, end2Edges=pickedEdges2, ratio=2.0, number=6, constraint=FIXED) pickedEdges = myPlateInstance.edges.findAt(((10,5,0),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=12, constraint=FIXED) pickedEdges = myPlateInstance.edges.findAt(((0,25,0),), ((20,25,0),)) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=15, constraint=FIXED) pickedEdges = myPlateInstance.edges.findAt(((10,50,0),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=5, constraint=FIXED) pickedEdges = myPlateInstance.edges.findAt(((17.5,0,0),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=4, constraint=FIXED) pickedEdges = myPlateInstance.edges.findAt(((2.5,0,0),),) myAssembly.seedEdgeByNumber(edges=pickedEdges, number=3, constraint=FIXED) # Assign meshing controls to the respective regions faces = myPlateInstance.faces f1 = myPlateInstance.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 = myPlateInstance.faces pickedRegions =(faces1, ) myAssembly.setElementType(regions=pickedRegions, elemTypes=(elemType1, elemType2)) partInstances =(myPlateInstance, ) myAssembly.generateMesh(regions=partInstances) #--------------------------------------------------------------------------- # Request history output for the crack myModel.historyOutputRequests.changeKey(fromName='H-Output-1', toName='JInt') myModel.historyOutputRequests['JInt'].setValues(contourIntegral='Crack', numberOfContours=7) #--------------------------------------------------------------------------- # Create the job myJob = mdb.Job(name=modelName, model=modelName, description='Contour integral analysis') mdb.saveAs(pathName=modelName) #---------------------------------------------------------------------------