""" Abaqus Example Manaual script to create the model and the and optimization attributes for the shape optimization of a connecting rod.The script is run using File -> Run Script in Abaqus/CAE. In order to successfully run conrod_shape_optimization.py the user must have conRod.inp in the working directory. """ from abaqus import * from abaqusConstants import * import regionToolset #Define the current viewport # curViewportName=session.currentViewportName curViewport=session.viewports[curViewportName] #Import of the model input file # try: mdb.ModelFromInputFile(name='connecting_rod', inputFileName='connecting_rod.inp') except: msg = "The input file (conRod.inp) was not found in the working directiory." raise ValueError, msg #model, part, assembly and part instance assignment # model=mdb.models['connecting_rod'] assembly = model.rootAssembly part1 = model.parts['PART-1'] instance=assembly.instances['PART-1-1'] #Use of the element set 'SOLID_ELEMENTS' with all the elements in the model # partElements = part1.elements #Creation of an elastic material # model.Material(name='Elastic_Mat') model.materials['Elastic_Mat'].Density(table=((7.81e-09, ), )) model.materials['Elastic_Mat'].Elastic(table=((210000.0, 0.3), )) #Creation of a homogeneous solid section # model.HomogeneousSolidSection(name='Section-1_Solid', material='Elastic_Mat', thickness=None) #Creation of the solid section assignment # solidElementRegion = part1.sets['SOLID_ELEMENTS'] part1.SectionAssignment(region=solidElementRegion, sectionName='Section-1_Solid', offset=0.0, offsetType=MIDDLE_SURFACE, offsetField='', thicknessAssignment=FROM_SECTION) #Part and assembly regeneration # part1.regenerate() assembly.regenerate() #Creation of a set 'ControlPt1' using the center node at the small end. # assembNodes = instance.nodes #Creation of constraints (kinematic couplings) at the small end and big end. # region1=assembly.sets['CONTROLPT1'] region2=assembly.surfaces['SURF_1_SMALL_END'] model.Coupling(name='Constraint-1', controlPoint=region1, surface=region2, influenceRadius=WHOLE_SURFACE, couplingType=KINEMATIC, localCsys=None, u1=ON, u2=ON, u3=ON, ur1=ON, ur2=ON, ur3=ON) #Creation of constraints (kinematic couplings) at the big end. # region1=assembly.sets['CONTROLPT2'] region2=assembly.surfaces['SURF_2_BIG_END'] model.Coupling(name='Constraint-2', controlPoint=region1, surface=region2, influenceRadius=WHOLE_SURFACE, couplingType=KINEMATIC, localCsys=None, u1=ON, u2=ON, u3=ON, ur1=ON, ur2=ON, ur3=ON) #Creation of Loads: 'Load-1' is created at the center node of the small end #'Load-2' is created at the center node of the big end. # region = assembly.sets['CONTROLPT1'] model.ConcentratedForce(name='Load-1', createStepName='Step-1', region=region, cf3=25000.0, distributionType=UNIFORM, field='', localCsys=None) #region = assembly.sets['CONTROLPT1'] model.ConcentratedForce(name='Load-3', createStepName='Step-2', region=region, cf3=-2000.0, distributionType=UNIFORM, field='', localCsys=None) region = assembly.sets['CONTROLPT2'] model.ConcentratedForce(name='Load-2', createStepName='Step-2', region=region, cf2=1750.0, distributionType=UNIFORM, field='', localCsys=None) #Creation of Displacement/Rotation Boundary conditions. # #For Step-1 # nodes1 = assembNodes.getSequenceFromMask(mask=('[#0:631 #3000000 ]', ), ) region = regionToolset.Region(nodes=nodes1) model.DisplacementBC(name='BC-1', createStepName='Step-1', region=region, u1=0.0, u2=0.0, u3=UNSET, ur1=UNSET, ur2=0.0, ur3=0.0, amplitude=UNSET, fixed=OFF, distributionType=UNIFORM, fieldName='', localCsys=None) nodes1 = assembNodes.getSequenceFromMask(mask=('[#0:631 #1000000 ]', ), ) region = regionToolset.Region(nodes=nodes1) model.DisplacementBC(name='BC-2',createStepName='Step-1', region=region, u1=UNSET, u2=UNSET, u3=0.0, ur1=UNSET, ur2=UNSET, ur3=UNSET, amplitude=UNSET, fixed=OFF, distributionType=UNIFORM, fieldName='', localCsys=None) #For Step-2 # model.loads['Load-1'].deactivate('Step-2') model.boundaryConditions['BC-1'].deactivate('Step-2') model.boundaryConditions['BC-2'].deactivate('Step-2') nodes1 = assembNodes.getSequenceFromMask(mask=('[#0:631 #3000000 ]', ), ) region = regionToolset.Region(nodes=nodes1) model.DisplacementBC(name='BC-3', createStepName='Step-2', region=region, u1=0.0, u2=UNSET, u3=UNSET, ur1=UNSET, ur2=0.0, ur3=0.0, amplitude=UNSET, fixed=OFF, distributionType=UNIFORM, fieldName='', localCsys=None) nodes1 = assembNodes.getSequenceFromMask(mask=('[#0:631 #2000000 ]', ), ) region = regionToolset.Region(nodes=nodes1) model.DisplacementBC(name='BC-4', createStepName='Step-2', region=region, u1=UNSET, u2=0.0, u3=UNSET, ur1=UNSET, ur2=UNSET, ur3=UNSET, amplitude=UNSET, fixed=OFF, distributionType=UNIFORM, fieldName='', localCsys=None) nodes1 = assembNodes.getSequenceFromMask(mask=('[#0:631 #1000000 ]', ), ) region = regionToolset.Region(nodes=nodes1) model.DisplacementBC(name='BC-5',createStepName='Step-2', region=region, u1=UNSET, u2=UNSET, u3=0.0, ur1=0.004, ur2=UNSET, ur3=UNSET, amplitude=UNSET, fixed=OFF, distributionType=UNIFORM, fieldName='', localCsys=None) #An elset selected asa region for Mesh Smoothing in Edit Optimization Task dialog # regionElset=assembly.sets['MESH_SMOOTH_ELEMENTS'] #A node set selected as design area region for the shape optimization region. # designNodesRegion=assembly.sets['DESIGN_NODES'] #Creation of a shape optimization task # model.ShapeTask(name='conrodShapeOptimizaton', region=designNodesRegion, freezeBoundaryConditionRegions=ON, frozenBoundaryConditionRegion=MODEL, smoothingRegion=regionElset) #Mises stress is selected as a design response for the design area nodes, which will be used #in the objective function. # shapeOptimizationTask=model.optimizationTasks['conrodShapeOptimizaton'] shapeOptimizationTask.SingleTermDesignResponse( name='misesStress1', region=designNodesRegion, identifier='SIG_MISES', drivingRegion=None, operation=MAXIMUM, shellLayer=MAXIMUM, stepOperation=MAXIMUM, stepOptions=(('Step-1', '', ALL, ALL), )) shapeOptimizationTask.SingleTermDesignResponse( name='misesStress2', region=designNodesRegion, identifier='SIG_MISES', drivingRegion=None, operation=MAXIMUM, shellLayer=MAXIMUM, stepOperation=MAXIMUM, stepOptions=(('Step-2', '', ALL, ALL), )) #Use of an element set 'ALL_SOLID_ELEMENTS' to be used as a region for the #Volume design response. # volConstRegion= assembly.sets['ALL_SOLID_ELEMENTS'] #Creation of the volume design response using the all solid elements (volConstRegion) # shapeOptimizationTask.SingleTermDesignResponse( name='volume', region=volConstRegion, identifier='VOLUME', drivingRegion=None, operation=SUM, stepOptions=()) #Creation of the optimization constraint using Volume desgin response. # shapeOptimizationTask.OptimizationConstraint( name='volume', designResponse='volume', restrictionMethod=RELATIVE_EQUAL, restrictionValue=1.0) #Vector definition to be used in the Demolding restriction. # negDemoldVector=((0.0, 0.0, 0.0), (-1.0, 0.0, 0.0)) #A region used for Demolding restriction, 'demoldControlNeg' # negDemoldRegion = assembly.sets['SURF_DEMOLD_NEG'] #Creation of Demold Control, Geometric Restriction using negDemoldRegion # shapeOptimizationTask.ShapeDemoldControl( name='demoldControlNeg', masterPointDetermination=MAXIMUM, region=negDemoldRegion, collisionCheckRegion=negDemoldRegion, masterPoint=None, csys=None, pullDirection=negDemoldVector, tolerance1=0.01, tolerance2=0.01, tolerance3=0.01, drawAngle=0.0, undercutTolerance=0.0, presumeFeasibleRegionAtStart=True) #Vector definition to be used in the Demolding restriction. # posDemoldVector=((0.0, 0.0, 0.0), (1.0, 0.0, 0.0)) #A region used for Demolding restriction, 'demoldControlPos' # posDemoldRegion = assembly.sets['SURF_DEMOLD_POS'] #Creation of Demold Control, Geometric Restriction using posDemoldRegion # shapeOptimizationTask.ShapeDemoldControl( name='demoldControlPos', masterPointDetermination=MAXIMUM, region=posDemoldRegion, collisionCheckRegion=posDemoldRegion, masterPoint=None, csys=None, pullDirection=posDemoldVector, tolerance1=0.01, tolerance2=0.01, tolerance3=0.01, drawAngle=0.0, undercutTolerance=0.0, presumeFeasibleRegionAtStart=True) #Creation of the Objective Function to minimize the maximum desgin response (Mises Stress) # shapeOptimizationTask.ObjectiveFunction( name='minimizeMaxStress', target=MINIMIZE_MAXIMUM, objectives=((OFF, 'misesStress1', 1.0, DEFAULT, ''), (OFF, 'misesStress2', 1.0, DEFAULT, ''))) #Creation of the Shape Optimization process of the model, conrodShapeOpt2. # mdb.OptimizationProcess(name='Shape-Opt-Process-1', model='connecting_rod', task='conrodShapeOptimizaton', description='Connecting rod shape optimization process', prototypeJob='Shape-Opt-Process-1-Job', maxDesignCycle=15, odbMergeFrequency=2, dataSaveFrequency=OPT_DATASAVE_FIRST_AND_LAST_CYCLE) #Creation of the job of the Shape Optimization process,'Shape-Opt-Process-1' # mdb.optimizationProcesses['Shape-Opt-Process-1'].Job( name='Shape-Opt-Process-1-Job', model='connecting_rod', atTime=None, waitMinutes=0, waitHours=0, queue=None, memory=50, memoryUnits=PERCENTAGE, getMemoryFromAnalysis=True, explicitPrecision=SINGLE, nodalOutputPrecision=SINGLE, multiprocessingMode=DEFAULT, numCpus=1) #Display the model assembly # curViewport.setValues(displayedObject=assembly)