Fracture Analysis - Contact debonding

The following example demonstrates the use of the Contact Debonding featuring in Mechanical using the Cohesive Zone Material (CZM) method. This example displaces two two-dimensional parts on a double cantilever beam.

Import necessary libraries

import os

from PIL import Image
from ansys.mechanical.core import App
from ansys.mechanical.core.examples import delete_downloads, download_file
from matplotlib import image as mpimg
from matplotlib import pyplot as plt
from matplotlib.animation import FuncAnimation

Embed mechanical and set global variables

app = App()
app.update_globals(globals())
print(app)

cwd = os.path.join(os.getcwd(), "out")


def display_image(image_name):
    plt.figure(figsize=(16, 9))
    plt.imshow(mpimg.imread(os.path.join(cwd, image_name)))
    plt.xticks([])
    plt.yticks([])
    plt.axis("off")
    plt.show()

Ansys Mechanical [Ansys Mechanical Enterprise]
Product Version:242
Software build date: 06/03/2024 09:35:09

Configure graphics for image export

Graphics.Camera.SetSpecificViewOrientation(ViewOrientationType.Front)
image_export_format = GraphicsImageExportFormat.PNG
settings_720p = Ansys.Mechanical.Graphics.GraphicsImageExportSettings()
settings_720p.Resolution = GraphicsResolutionType.EnhancedResolution
settings_720p.Background = GraphicsBackgroundType.White
settings_720p.Width = 1280
settings_720p.Height = 720
settings_720p.CurrentGraphicsDisplay = False

Download geometry and materials files

geometry_path = download_file(
    "Contact_Debonding_Example.agdb", "pymechanical", "embedding"
)
mat1_path = download_file(
    "Contact_Debonding_Example_Mat1.xml", "pymechanical", "embedding"
)
mat2_path = download_file(
    "Contact_Debonding_Example_Mat2.xml", "pymechanical", "embedding"
)

Import the geometry

geometry_import = Model.GeometryImportGroup.AddGeometryImport()
geometry_import_format = (
    Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.Format.Automatic
)
geometry_import_preferences = Ansys.ACT.Mechanical.Utilities.GeometryImportPreferences()
geometry_import_preferences.ProcessNamedSelections = True
geometry_import_preferences.AnalysisType = (
    Ansys.Mechanical.DataModel.Enums.GeometryImportPreference.AnalysisType.Type2D
)
geometry_import.Import(
    geometry_path, geometry_import_format, geometry_import_preferences
)

app.plot()

Static Scene

Interactive Scene

Material import, named selections, and connections

Import materials

MODEL = Model
GEOMETRY = Model.Geometry
MAT_GRP = MODEL.Materials
MAT_GRP.Import(mat1_path)
MAT_GRP.Import(mat2_path)

PART = [x for x in Tree.AllObjects if x.Name == "Part 2"][0]
MAT_BODY = [
    i
    for i in MAT_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.Material](True)
    if i.Name == "Interface Body Material"
][0]
MAT_CZM = [
    i
    for i in MAT_GRP.GetChildren[Ansys.ACT.Automation.Mechanical.Material](True)
    if i.Name == "CZM Crack Material"
][0]

Connections

connections = MODEL.AddConnections()
CONNECTIONS_GRP = connections.AddConnectionGroup()
MODEL.Connections.CreateAutomaticConnections()
CONNECTIONS_GRP = Model.Connections
CONTACTS = [
    i
    for i in CONNECTIONS_GRP.GetChildren[
        Ansys.ACT.Automation.Mechanical.Connections.ConnectionGroup
    ](True)
    if i.Name == "Contacts"
][0]
CONTACT_REGION = [
    i
    for i in CONTACTS.GetChildren[
        Ansys.ACT.Automation.Mechanical.Connections.ContactRegion
    ](True)
    if i.Name == "Contact Region"
][0]

Named selections

NAMED_SELECTIONS = Model.NamedSelections
NS_EDGE_HIGH = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "High_Edge"
][0]
NS_EDGE_LOW = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Low_Edge"
][0]
NS_EDGES_SHORT = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Short_Edges"
][0]
NS_EDGES_LONG = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Long_Edges"
][0]
NS_EDGES_FIXED = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Fixed_Edges"
][0]
NS_VERTEX_DISP1 = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Disp1_Vertex"
][0]
NS_VERTEX_DISP2 = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Disp2_Vertex"
][0]
NS_FACES_BOTH = [
    i
    for i in NAMED_SELECTIONS.GetChildren[
        Ansys.ACT.Automation.Mechanical.NamedSelection
    ](True)
    if i.Name == "Both_Faces"
][0]

Define static structural analysis and settings

MODEL.AddStaticStructuralAnalysis()
STATIC_STRUCTURAL = DataModel.AnalysisByName("Static Structural")
ANALYSIS_SETTINGS = STATIC_STRUCTURAL.AnalysisSettings
SOLUTION = STATIC_STRUCTURAL.Solution
MESH = Model.Mesh

# Set unit system

ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMM

# Set 2D behavior

GEOMETRY.Activate()
GEOMETRY.Model2DBehavior = Model2DBehavior.PlaneStrain

# Assign material

PART.Activate()
PART.Material = MAT_BODY.Name

# Define contact Region

CONTACT_REGION.Activate()
CONTACT_REGION.SourceLocation = NS_EDGE_HIGH
CONTACT_REGION.TargetLocation = NS_EDGE_LOW
CONTACT_REGION.ContactType = ContactType.Bonded
CONTACT_REGION.ContactFormulation = ContactFormulation.PurePenalty

Define mesh controls and generate mesh

MESH.Activate()
MESH.ElementOrder = ElementOrder.Quadratic
MESH.UseAdaptiveSizing = False
MESH.ElementSize = Quantity("0.75 [mm]")

SIZING_MESH = MESH.AddSizing()
SIZING_MESH.Location = NS_EDGES_SHORT
SIZING_MESH.ElementSize = Quantity("0.75 [mm]")
SIZING_MESH.Behavior = SizingBehavior.Hard

SIZING_MESH2 = MESH.AddSizing()
SIZING_MESH2.Location = NS_EDGES_LONG
SIZING_MESH2.ElementSize = Quantity("0.5 [mm]")
SIZING_MESH2.Behavior = SizingBehavior.Hard

FACE_MESHING = MESH.AddFaceMeshing()
FACE_MESHING.Location = NS_FACES_BOTH
FACE_MESHING.Method = FaceMeshingMethod.Quadrilaterals

MESH.Activate()
MESH.GenerateMesh()

Graphics.Camera.SetFit()
Graphics.ExportImage(os.path.join(cwd, "mesh.png"), image_export_format, settings_720p)
display_image("mesh.png")

Add contact debonding object

MODEL.Activate()
FRACTURE = MODEL.AddFracture()

CONTACT_DEBONDING = FRACTURE.AddContactDebonding()
CONTACT_DEBONDING.Material = MAT_CZM.Name
CONTACT_DEBONDING.ContactRegion = CONTACT_REGION

Define analysis settings

ANALYSIS_SETTINGS.Activate()
ANALYSIS_SETTINGS.AutomaticTimeStepping = AutomaticTimeStepping.On
ANALYSIS_SETTINGS.DefineBy = TimeStepDefineByType.Substeps
ANALYSIS_SETTINGS.MaximumSubsteps = 100
ANALYSIS_SETTINGS.InitialSubsteps = 100
ANALYSIS_SETTINGS.MinimumSubsteps = 100
ANALYSIS_SETTINGS.LargeDeflection = True

Define boundary conditions

Add fixed support

STATIC_STRUCTURAL.Activate()
FIXED_SUPPORT = STATIC_STRUCTURAL.AddFixedSupport()
FIXED_SUPPORT.Location = NS_EDGES_FIXED

Add displacement

STATIC_STRUCTURAL.Activate()
DISPLACEMENT = STATIC_STRUCTURAL.AddDisplacement()
DISPLACEMENT.Location = NS_VERTEX_DISP1
DISPLACEMENT.DefineBy = LoadDefineBy.Components
DISPLACEMENT.YComponent.Output.DiscreteValues = [Quantity("10 [mm]")]

STATIC_STRUCTURAL.Activate()
DISPLACEMENT2 = STATIC_STRUCTURAL.AddDisplacement()
DISPLACEMENT2.Location = NS_VERTEX_DISP2
DISPLACEMENT2.DefineBy = LoadDefineBy.Components
DISPLACEMENT2.YComponent.Output.DiscreteValues = [Quantity("-10 [mm]")]

STATIC_STRUCTURAL.Activate()

Graphics.Camera.SetFit()
Graphics.ExportImage(
    os.path.join(cwd, "boundary_conditions.png"), image_export_format, settings_720p
)
display_image("boundary_conditions.png")

Add results

SOLUTION.Activate()
DIRECTIONAL_DEFORMATION = SOLUTION.AddDirectionalDeformation()
DIRECTIONAL_DEFORMATION.NormalOrientation = NormalOrientationType.YAxis

FORCE_REACTION = SOLUTION.AddForceReaction()
FORCE_REACTION.BoundaryConditionSelection = DISPLACEMENT

Solve

STATIC_STRUCTURAL.Activate()
SOLUTION.Solve(True)

Messages

Messages = ExtAPI.Application.Messages
if Messages:
    for message in Messages:
        print(f"[{message.Severity}] {message.DisplayString}")
else:
    print("No [Info]/[Warning]/[Error] Messages")

[Warning] Large deformation effects are active which may have invalidated some of your applied supports such as displacement, cylindrical, frictionless, or compression only.  Refer to Troubleshooting in the Help System for more details.
[Warning] Contact status has experienced an abrupt change.  Check results carefully for possible contact separation.

Display results

Directional deformation

DIRECTIONAL_DEFORMATION.Activate()

Graphics.ExportImage(
    os.path.join(cwd, "directional_deformation.png"), image_export_format, settings_720p
)
display_image("directional_deformation.png")

Force reaction

FORCE_REACTION.Activate()

Graphics.Camera.SetFit()
Graphics.ExportImage(
    os.path.join(cwd, "force_reaction.png"), image_export_format, settings_720p
)
display_image("force_reaction.png")

Export animation

animation_export_format = (
    Ansys.Mechanical.DataModel.Enums.GraphicsAnimationExportFormat.GIF
)
settings_720p = Ansys.Mechanical.Graphics.AnimationExportSettings()
settings_720p.Width = 1280
settings_720p.Height = 720

FORCE_REACTION.ExportAnimation(
    os.path.join(cwd, "force_reaction.gif"), animation_export_format, settings_720p
)
gif = Image.open(os.path.join(cwd, "force_reaction.gif"))
fig, ax = plt.subplots(figsize=(16, 9))
ax.axis("off")
img = ax.imshow(gif.convert("RGBA"))


def update(frame):
    gif.seek(frame)
    img.set_array(gif.convert("RGBA"))
    return [img]


ani = FuncAnimation(
    fig, update, frames=range(gif.n_frames), interval=100, repeat=True, blit=True
)
plt.show()

Once Loop Reflect