Fracture Analysis: Semi-Elliptical Crack

This example creates a Fracture Analysis that uses a Semi-Elliptical Crack. A semi-elliptical crack is inserted at the tubular joint of the structure, the crack mesh is generated for defined Semi-Elliptical Crack, and then fracture parameters are computed and post-processed.

This example begins in the Mechanical application. It requires you to download the following Ansys DesignModeler and python files.

Semi-Elliptical_Crack_Example_003.agdb
Semi-Elliptical_Crack_Example_003.py

These files are available here.

Procedure

Open Mechanical directly without importing a geometry or specifying an analysis type. This can be done through Start Menu.
From the Analysis drop-down menu of the Insert group on the Home tab, insert a Static Structural system into the tree.
Select the Geometry object and select the Attach Geometry option from the Geometry group on the Geometry Context tab. Navigate to the proper folder location and select Semi-Elliptical_Crack_Example_003.agdb.
Select the Automation tab and select the Scripting option to open the Mechanical Scripting pane.
Select the Open Script option ( ) from the Editor toolbar. Navigate to the proper folder location and select Semi-Elliptical_Crack_Example_003.py.
Select the Run Script option ( ) from the Editor toolbar.

Scripts Illustrated

In this example, the python file automatically performs the following actions:

# Scenario 1 Store main Tree Object items
MODEL = Model
GEOMETRY = Model.Geometry
SOLID2 = [x for x in ExtAPI.DataModel.Tree.AllObjects if x.Name == 'Solid2'][0]

COORDINATE_SYSTEMS = Model.CoordinateSystems
GLOBAL_COORDINATE_SYSTEM = [i for i in COORDINATE_SYSTEMS.GetChildren[Ansys.ACT.Automation.Mechanical.CoordinateSystem](True) if i.Name == 'Global Coordinate System'][0]

MESH = Model.Mesh

NAMED_SELECTIONS = ExtAPI.DataModel.Project.Model.NamedSelections
NS_PIPE_BODY = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Pipe_Body'][0]
NS_FILET_FACE = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Filet_Face'][0]
NS_VERTEX_FILET = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Vertex_Filet'][0]
NS_PRESSURE_FACE = [i for i in NAMED_SELECTIONS.GetChildren[Ansys.ACT.Automation.Mechanical.NamedSelection](True) if i.Name == 'Pressure_Face'][0]

STATIC_STRUCTURAL = ExtAPI.DataModel.AnalysisByName("Static Structural")
ANALYSIS_SETTINGS = STATIC_STRUCTURAL.AnalysisSettings
SOLUTION= STATIC_STRUCTURAL.Solution

# Scenario 2 Set Display Unit
ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMM

# Scenario 3 Add local Coordinate System for defining Semi-Elliptical Crack
COORDINATE_SYSTEMS.Activate()
COORDINATE_SYSTEM = COORDINATE_SYSTEMS.AddCoordinateSystem()
SEL=ExtAPI.SelectionManager.AddSelection(NS_VERTEX_FILET)
SEL2=ExtAPI.SelectionManager.CurrentSelection
COORDINATE_SYSTEM.OriginLocation = SEL2
ExtAPI.SelectionManager.ClearSelection()

COORDINATE_SYSTEM.AddTransformation(TransformationType.Rotation, CoordinateSystemAxisType.PositiveZAxis)
COORDINATE_SYSTEM.SetTransformationValue(1, 22.2922)
COORDINATE_SYSTEM.AddTransformation(TransformationType.Rotation, CoordinateSystemAxisType.PositiveYAxis)
COORDINATE_SYSTEM.SetTransformationValue(2, 180)

# Scenario 4 Define Mesh controls and generate base mesh
MESH.Activate()
MESH.SpanAngleCenter = 2 # For setting it to Fine option

METHOD_MESH = MESH.AddAutomaticMethod()
METHOD_MESH.Location = NS_PIPE_BODY
METHOD_MESH.Method=MethodType.AllTriAllTet

SIZING_MESH = MESH.AddSizing()
SIZING_MESH.Location = NS_FILET_FACE
SIZING_MESH.ElementSize = Quantity('5 [mm]')

MESH.Activate()
MESH.GenerateMesh()

# Scenario 5 Add Semi-Elliptical Crack object and Generate Crack Mesh
MODEL.Activate()
FRACTURE = MODEL.AddFracture()

SEMI_ELLIPTICAL_CRACK = FRACTURE.AddSemiEllipticalCrack()
SEL=ExtAPI.SelectionManager.AddSelection(NS_PIPE_BODY)
SEL2=ExtAPI.SelectionManager.CurrentSelection
SEMI_ELLIPTICAL_CRACK.Location=SEL2
ExtAPI.SelectionManager.ClearSelection()

SEMI_ELLIPTICAL_CRACK.CoordinateSystem=COORDINATE_SYSTEM
SEMI_ELLIPTICAL_CRACK.MajorRadius = Quantity("18.4 [mm]")
SEMI_ELLIPTICAL_CRACK.MinorRadius = Quantity("9.5 [mm]")
SEMI_ELLIPTICAL_CRACK.LargestContourRadius= Quantity("2 [mm]")
SEMI_ELLIPTICAL_CRACK.CrackFrontDivisions = 35
SEMI_ELLIPTICAL_CRACK.CircumferentialDivisions = 18

SEMI_ELLIPTICAL_CRACK.CrackFacesNodes = True
SEMI_ELLIPTICAL_CRACK.ContactPairsNodes= True
FRACTURE.GenerateAllCrackMesh()

# Scenario 6 Define Analysis Settings for Fracture calculations
ANALYSIS_SETTINGS.Activate()
ANALYSIS_SETTINGS.WeakSprings=WeakSpringsType.ProgramControlled
ANALYSIS_SETTINGS.SIFS = True
ANALYSIS_SETTINGS.JIntegral = True
ANALYSIS_SETTINGS.MaterialForce = True
ANALYSIS_SETTINGS.TStress = True

# Scenario 7 Define boundary condition
STATIC_STRUCTURAL.Activate()
PRESSURE = STATIC_STRUCTURAL.AddPressure()
PRESSURE.Location = NS_PRESSURE_FACE
PRESSURE.Magnitude.Output.DiscreteValues = [Quantity('-100 [MPa]')]

# Scenario 8 Add Deformation and Fracture specific results
SOLUTION.Activate()
TOTAL_DEFORMATION = SOLUTION.AddTotalDeformation() 

FRACTURE_TOOL = SOLUTION.AddFractureTool()
FRACTURE_TOOL.CrackSelection = SEMI_ELLIPTICAL_CRACK

SIFS_K1 = [i for i in FRACTURE_TOOL.GetChildren[Ansys.ACT.Automation.Mechanical.Results.FractureToolResults.FractureToolResult](True) if i.Name == 'SIFS (K1)'][0]
SIFS_K2 = FRACTURE_TOOL.AddSIFSK2()
SIFS_K3 = FRACTURE_TOOL.AddSIFSK3()
J_INTEGRAL = FRACTURE_TOOL.AddJINT()
MATERIAL_FORCE_X = FRACTURE_TOOL.AddMaterialForceX()
MATERIAL_FORCE_Y = FRACTURE_TOOL.AddMaterialForceY()
MATERIAL_FORCE_Z = FRACTURE_TOOL.AddMaterialForceZ()
T_STRESS = FRACTURE_TOOL.AddTSTRESS()

# Scenario 9 Solve and review Results
STATIC_STRUCTURAL.Activate()
STATIC_STRUCTURAL.Solve(True)

TOTAL_DEFORMATION.Activate()
MAX_TOTAL_DEFORMATION = TOTAL_DEFORMATION.Maximum.Value

SIFS_K1.Activate()
MIN_SIFS_K1_C6 = SIFS_K1.Minimum.Value
MAX_SIFS_K1_C6 = SIFS_K1.Maximum.Value

SIFS_K2.Activate()
MIN_SIFS_K2_C6 = SIFS_K2.Minimum.Value
MAX_SIFS_K2_C6 = SIFS_K2.Maximum.Value

SIFS_K3.Activate()
MIN_SIFS_K3_C6 = SIFS_K3.Minimum.Value
MAX_SIFS_K3_C6 = SIFS_K3.Maximum.Value

J_INTEGRAL.Activate()
MIN_J_INTEGRAL_C6 = J_INTEGRAL.Minimum.Value
MAX_J_INTEGRAL_C6 = J_INTEGRAL.Maximum.Value

MATERIAL_FORCE_X.Activate()
MIN_MATERIAL_FORCE_X_C6 = MATERIAL_FORCE_X.Minimum.Value
MAX_MATERIAL_FORCE_X_C6 = MATERIAL_FORCE_X.Maximum.Value

MATERIAL_FORCE_Y.Activate()
MIN_MATERIAL_FORCE_Y_C6 = MATERIAL_FORCE_Y.Minimum.Value
MAX_MATERIAL_FORCE_Y_C6 = MATERIAL_FORCE_Y.Maximum.Value

MATERIAL_FORCE_Z.Activate()
MIN_MATERIAL_FORCE_Z_C6 = MATERIAL_FORCE_Z.Minimum.Value
MAX_MATERIAL_FORCE_Z_C6 = MATERIAL_FORCE_Z.Maximum.Value

T_STRESS.Activate()
MIN_T_STRESS_C6 = T_STRESS.Minimum.Value
MAX_T_STRESS_C6 = T_STRESS.Maximum.Value

Summary

This example demonstrates how scripting in Mechanical can be used to automate your actions.