r""" .. _ref_1711: Single edge notched tension test ^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^ A well-known benchmark simulation in fracture mechanics is performed, relying on the simulation conducted by [Miehe]_. This simulation considers an anisotropic formulation with spectral energy decomposition, although we have also repeated the simulations with the isotropic formulation. The model consists of a square plate with a notch located halfway up, extending from the left to the center, as shown in the figure below. The bottom part is fixed in all directions, while the upper part can slide vertically. A vertical displacement is applied at the top. The geometry and boundary conditions are depicted in the figure. We discretize the model with triangular elements, refining the areas (element size h) where crack evolution is expected. The element size $h$ must be sufficiently small to avoid mesh dependencies. .. code-block:: # u/\/\/\/\/\/\ # |||||||||||| # *----------* # | | # | a=0.5 | # |--- | # | | # | | # *----------* # /_\/_\/_\/_\ # |Y ///////////// # | # ---X # Z / The Young's modulus, Poisson's ratio, and the critical energy release rate are given in the table :ref:`Properties `. Young's modulus $E$ and Poisson's ratio $\nu$ can be represented with the Lamé parameters as: $\lambda=\frac{E\nu}{(1+\nu)(1-2\nu)}$; $\mu=\frac{E}{2(1+\nu)}$. .. _table_properties_label: +----+---------+--------+ | | VALUE | UNITS | +====+=========+========+ | E | 210 | kN/mm2 | +----+---------+--------+ | nu | 0.3 | [-] | +----+---------+--------+ | Gc | 0.0027 | kN/mm | +----+---------+--------+ | l | 0.015 | mm | +----+---------+--------+ .. [Miehe] A phase field model for rate-independent crack propagation: Robust algorithmic implementation based on operator splits, https://doi.org/10.1016/j.cma.2010.04.011. """ ############################################################################### # Import necessary libraries # -------------------------- import numpy as np import matplotlib.pyplot as plt import pyvista as pv import dolfinx import mpi4py import petsc4py import os ############################################################################### # Import from phasefieldx package # ------------------------------- from phasefieldx.Element.Phase_Field_Fracture.Input import Input from phasefieldx.Element.Phase_Field_Fracture.solver.solver import solve from phasefieldx.Boundary.boundary_conditions import bc_xy, bc_y, get_ds_bound_from_marker from phasefieldx.PostProcessing.ReferenceResult import AllResults ############################################################################### # Parameters Definition # --------------------- # `Data` is an input object containing essential parameters for simulation setup # and result storage: # # - `E`: Young's modulus, set to 210 $kN/mm^2$. # - `nu`: Poisson's ratio, set to 0.3. # - `Gc`: Critical energy release rate, set to 0.005 $kN/mm$. # - `l`: Length scale parameter, set to 0.1 $mm$. # - `degradation`: Specifies the degradation type. Options are "isotropic" or "anisotropic". # - `split_energy`: Controls how the energy is split; options include "no" (default), "spectral," or "deviatoric." # - `degradation_function`: Specifies the degradation function; here, it is "quadratic." # - `irreversibility`: Determines the irreversibility criterion; in this case, set to "miehe." # - `fatigue`: Enables fatigue simulation when set to `True`. # - `fatigue_degradation_function`: Defines the function for fatigue degradation, set to "asymptotic." # - `fatigue_val`: Fatigue parameter value (used only in fatigue simulations, not in this one). # - `k`: Stiffness penalty parameter, set to 0.0. # - `min_stagger_iter`: Minimum number of staggered iterations, set to 2. # - `max_stagger_iter`: Maximum number of staggered iterations, set to 500. # - `stagger_error_tol`: Error tolerance for staggered iterations, set to 1e-8. # - `save_solution_xdmf` and `save_solution_vtu`: Specify the file formats to save displacement results. # In this case, results are saved as `.vtu` files. # - `results_folder_name`: Name of the folder for saving results. If it exists, # it will be replaced with a new empty folder. Data = Input(E=210.0, # young modulus nu=0.3, # poisson Gc=0.0027, # critical energy release rate l=0.015, # lenght scale parameter degradation="isotropic", # "isotropic" "anisotropic" split_energy="no", # "spectral" "deviatoric" degradation_function="quadratic", irreversibility="miehe", # "miehe" fatigue=False, fatigue_degradation_function="asymptotic", fatigue_val=0.0, k=0.0, save_solution_xdmf=False, save_solution_vtu=True, results_folder_name="1711_Single_Edge_Notched_Tension_Test") ############################################################################### # Mesh Definition # --------------- # The mesh is generated using Gmsh and saved as a 'mesh.msh' file. For more details # on how to create the mesh, refer to the :ref:`ref_examples_91` examples. msh_file = os.path.join("mesh", "mesh.msh") # Path to the mesh file gdim = 2 # Geometric dimension of the mesh gmsh_model_rank = 0 # Rank of the Gmsh model in a parallel setting mesh_comm = mpi4py.MPI.COMM_WORLD # MPI communicator for parallel computation # %% # The mesh, cell markers, and facet markers are extracted from the 'mesh.msh' file # using the `read_from_msh` function. mesh_data = dolfinx.io.gmsh.read_from_msh(msh_file, mesh_comm, gmsh_model_rank, gdim) msh = mesh_data.mesh cell_markers = mesh_data.cell_tags facet_markers = mesh_data.facet_tags fdim = msh.topology.dim - 1 # Dimension of the mesh facets # %% # Facets defined in the .geo file used to generate the 'mesh.msh' file are identified here. # Each marker variable corresponds to a specific region on the specimen: # # - `bottom_facet_marker`: Refers to the bottom part of the specimen. # - `top_facet_marker`: Refers to the top part of the specimen. # - `right_facet_marker`: Refers to the right side of the specimen. # - `left_facet_marker`: Refers to the left side of the specimen. bottom_facet_marker = facet_markers.find(9) top_facet_marker = facet_markers.find(10) right_facet_marker = facet_markers.find(11) left_facet_marker = facet_markers.find(12) # %% # The `get_ds_bound_from_marker` function creates measures for applying boundary conditions # on specific facets. These measures are generated for: # # - `bottom_facet_marker` → Stored in `ds_bottom` # - `top_facet_marker` → Stored in `ds_top` ds_bottom = get_ds_bound_from_marker(bottom_facet_marker, msh, fdim) ds_top = get_ds_bound_from_marker(top_facet_marker, msh, fdim) # %% # `ds_list` is an array that organizes boundary condition measures alongside descriptive names. # Each entry in `ds_list` consists of two elements: # # - A measure (e.g., `ds_bottom`) # - A corresponding name (e.g., `"bottom"`) # This structure simplifies the process of saving results by associating each boundary condition # measure with a clear label. For instance: # # - `ds_bottom` is labeled as `"bottom"`. # - `ds_top` is labeled as `"top"`. ds_list = np.array([ [ds_top, "top"], [ds_bottom, "bottom"], ]) ############################################################################### # Function Space Definition # ------------------------- # Define function spaces for displacement and phase-field using Lagrange elements. V_u = dolfinx.fem.functionspace(msh, ("Lagrange", 1, (msh.geometry.dim, ))) V_phi = dolfinx.fem.functionspace(msh, ("Lagrange", 1)) ############################################################################### # Boundary Conditions # ------------------- # Dirichlet boundary conditions are defined as follows: # # - `bc_bottom`: Constrains both x and y displacements to 0 on the bottom boundary, # ensuring that the bottom edge remains fixed. # - `bc_top`: Constrains the x displacement, while the vertical displacement on the # top boundary is updated dynamically in the quasi-static solver to impose the desired # vertical displacement. bc_bottom = bc_xy(bottom_facet_marker, V_u, fdim) bc_top = bc_y(top_facet_marker, V_u, fdim) # %% # The bcs_list_u variable is a list that stores all boundary conditions for the displacement # field $\boldsymbol u$. This list facilitates easy management of multiple boundary # conditions and can be expanded if additional conditions are needed. bcs_list_u = [bc_top, bc_bottom] bcs_list_u_names = ["top", "bottom"] ############################################################################### # Function: `update_boundary_conditions` # -------------------------------------- # The `update_boundary_conditions` function updates the displacement boundary # conditions dynamically at each time step. This enables quasi-static analysis # by incrementally adjusting the displacements applied to specific degrees of freedom. # # Parameters: # # - `bcs`: A list of boundary conditions, where each element corresponds to a # boundary condition applied to a specific facet of the mesh. # - `time`: A scalar representing the current time step in the analysis. # # Function Details: # # - The displacement value `val` is computed based on the current `time`: # - For `time <= 50`, `val` increases linearly as `val = dt0 * time`, where `dt0` # is a small time step factor (`10^-4`), simulating gradual displacement along the y-axis. # - For `time > 50`, `val` increases more gradually as `val = 50 * dt0 + (dt0 / 10) * (time - 50)`, # which represents a slower displacement rate after the initial period. # # - This calculated value is assigned to the y-component of the displacement field # on the top boundary by modifying `bcs[0].g.value[1]`, where `bcs[0]` represents the # top boundary condition. # # Return Value: # # - A tuple `(0, val, 0)` is returned, representing the incremental displacement vector: # - The first element (0) corresponds to no update for the x-displacement. # - The second element (`val`) is the calculated y-displacement. # - The third element (0) corresponds to no update for the z-displacement, applicable in 2D simulations. # # Purpose: # # - This function facilitates quasi-static analysis by applying controlled, time-dependent # boundary displacements. It is essential for simulations that involve gradual loading or unloading, # with a slower displacement evolution after an initial phase. def update_boundary_conditions(bcs, time): dt0 = 10**-4 if time <= 50: val = dt0 * time else: val = 50 * dt0 + dt0 / 10 * (time - 50) bcs[0].g.value[...] = petsc4py.PETSc.ScalarType(val) return 0, val, 0 T_list_u = None update_loading = None f = None T = dolfinx.fem.Constant(msh, petsc4py.PETSc.ScalarType((0.0, 0.0))) ############################################################################### # Boundary Conditions for phase field bcs_list_phi = [] ############################################################################### # Solver Call for a Phase-Field Fracture Problem # ---------------------------------------------- # This section sets up and calls the solver for a phase-field fracture problem. # # **Key Points:** # # - The simulation is run for a final time of 150, with a time step of 1.0. # - The solver will manage the mesh, boundary conditions, and update the solution # over the specified time steps. # # **Parameters:** # # - `dt`: The time step for the simulation, set to 1.0. # - `final_time`: The total simulation time, set to 200.0, which determines how # long the problem will be solved. # - `path`: Optional parameter for specifying the folder where results will be saved; # here it is set to `None`, meaning results will be saved to the default location. # # **Function Call:** # The `solve` function is invoked with the following arguments: # # - `Data`: Contains the simulation parameters and configurations. # - `msh`: The mesh representing the domain for the problem. # - `final_time`: The total duration of the simulation (200.0). # - `V_u`: Function space for the displacement field, $\boldsymbol{u}$. # - `V_phi`: Function space for the phase field, $\phi$. # - `bcs_list_u`: List of Dirichlet boundary conditions for the displacement field. # - `bcs_list_phi`: List of boundary conditions for the phase field (empty in this case). # - `update_boundary_conditions`: Function to update boundary conditions for the displacement field. # - `f`: The body force applied to the domain (if any). # - `T_list_u`: Time-dependent loading parameters for the displacement field. # - `update_loading`: Function to update loading parameters for the quasi-static analysis. # - `ds_list`: Boundary measures for integration over the domain boundaries. # - `dt`: The time step for the simulation. # - `path`: Directory for saving results (if specified). # # This setup provides a framework for solving static problems with specified boundary # conditions and loading parameters. dt = 1.0 final_time = 150.0 # %% # Uncomment the following lines to run the solver with the specified parameters. # solve(Data, # msh, # final_time, # V_u, # V_phi, # bcs_list_u, # bcs_list_phi, # update_boundary_conditions, # f, # T_list_u, # update_loading, # ds_list, # dt, # path=None, # bcs_list_u_names=bcs_list_u_names, # min_stagger_iter=2, # max_stagger_iter=500, # stagger_error_tol=1e-8) ############################################################################### # Load results # ------------ # Once the simulation finishes, the results are loaded from the results folder. # The AllResults class takes the folder path as an argument and stores all # the results, including logs, energy, convergence, and DOF files. # Note that it is possible to load results from other results folders to compare results. # It is also possible to define a custom label and color to automate plot labels. S = AllResults(Data.results_folder_name) S.set_label('Simulation') S.set_color('b') ############################################################################### # Plot: phase-field $\phi$ # ------------------------ # The phase-field result saved in the .vtu file is shown. # For this, the file is loaded using PyVista. file_vtu = pv.read(os.path.join(Data.results_folder_name, "paraview-solutions_vtu", "phasefieldx_p0_000149.vtu")) file_vtu.plot(scalars='phi', cpos='xy', show_scalar_bar=True, show_edges=False) ############################################################################### # Plot: displacement $\boldsymbol u$ # ---------------------------------- # The displacements results saved in the .vtu file are shown. # For this, the file is loaded using PyVista. file_vtu = pv.read(os.path.join(Data.results_folder_name, "paraview-solutions_vtu", "phasefieldx_p0_000149.vtu")) file_vtu.plot(scalars='u', cpos='xy', show_scalar_bar=True, show_edges=False) ############################################################################### # Plot: Displacement vs Fracture Energy # ------------------------------------- # The vertical displacement is saved in S.dof_files["top.dof"]["Uy"]. displacement = S.dof_files["top.dof"]["Uy"] fig, energyW = plt.subplots() energyW.plot(displacement, S.energy_files['total.energy']["W"], 'b-', linewidth=2.0, label=r'$W$') energyW.plot(displacement, S.energy_files['total.energy']["W_phi"], 'y-', linewidth=2.0, label=r'$W_{\phi}$') energyW.plot(displacement, S.energy_files['total.energy']["W_gradphi"], 'g-', linewidth=2.0, label=r'$W_{\nabla \phi}$') energyW.grid(color='k', linestyle='-', linewidth=0.3) energyW.set_xlabel('displacement - u $[mm]$') energyW.set_ylabel('Energy') energyW.legend() ############################################################################### # Plot: Displacement vs Gamma # --------------------------- fig, gamma = plt.subplots() gamma.plot(displacement, S.energy_files['total.energy']["gamma"], 'b-', linewidth=2.0, label=r'$\Gamma$') gamma.plot(displacement, S.energy_files['total.energy']["gamma_phi"], 'y-', linewidth=2.0, label=r'$\Gamma_{\phi}$') gamma.plot(displacement, S.energy_files['total.energy']["gamma_gradphi"], 'g-', linewidth=2.0, label=r'$\Gamma_{\nabla \phi}$') gamma.grid(color='k', linestyle='-', linewidth=0.3) gamma.set_xlabel('displacement - u $[mm]$') gamma.set_ylabel(r'$\Gamma$') gamma.legend() ############################################################################### # Plot: Force vs Vertical Displacement # ------------------------------------ Miehe = np.loadtxt(os.path.join("reference_solutions", "miehe_solution.csv")) fig, ax_reaction = plt.subplots() ax_reaction.plot(Miehe[:, 0], Miehe[:, 1], 'g-', linewidth=2.0, label='Miehe') ax_reaction.plot(displacement, -S.reaction_files['bottom.reaction']["Ry"], 'k.', linewidth=2.0, label=S.label) ax_reaction.grid(color='k', linestyle='-', linewidth=0.3) ax_reaction.set_xlabel('displacement - u $[mm]$') ax_reaction.set_ylabel('reaction force - F $[kN]$') ax_reaction.set_title('Reaction Force vs Vertical Displacement') ax_reaction.legend() ############################################################################### # Plot: Staggered Iterations vs Vertical Displacement # --------------------------------------------------- fig, ax_convergence = plt.subplots() ax_convergence.plot(displacement, S.convergence_files["phasefieldx.conv"]["stagger"], 'k.', linewidth=2.0, label='Stagger iterations') ax_convergence.grid(color='k', linestyle='-', linewidth=0.3) ax_convergence.set_xlabel('displacement - u $[mm]$') ax_convergence.set_ylabel('stagger iterations - []') ax_convergence.set_title('Stagger iterations vs vertical displacement') ax_convergence.legend() plt.show()