===================================== Boundary conditions and constraints ===================================== .. currentmodule:: fedoo Basic boundary conditions ============================== There is 3 basic types of boundary conditions in fedoo: #. Dirichlet boundary conditions: Value specified for a degree of freedom (for instance displacement). #. Neumann boundary conditions: Value specified for the dual value of a degree of freedom (for instance force) #. Multi-point constraints (MPC): linear coupling between degrees of freedom. MPC are not properly speaking boundary conditions. In fedoo they are considered as part of boundary conditions, because they often used to specify complexe boundary conditions, but they are more general that simple boundary conditions. Each time a problem is created, a list of boundary conditions is associated to the problem in the "*bc*" attribute of the problem instance. problem.bc is then a :py:class:`fedoo.ListBC` Object. .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.ListBC Dirichlet and Neumann Boundary conditions ____________________________________________ The recommanded way to apply some boundary conditions is to use the method :py:meth:`fedoo.ListBC.add`, directly from problem attribute :py:attr:`fedoo.Problem.bc`. This method build a :py:class:`fedoo.core.BoundaryCondition` object and add it to the problem boundary conditions. .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.core.BoundaryCondition Here are some examples to add some Dirichlet or Neumann Boundary conditions for a given problem *pb*: Displacement along the X axis blocked (=0) for the nodes 0, 1 and 8 >>> pb.bc.add('Dirichlet',[0,1,8], 'DispX', 0) Displacement along the all axis blocked (=0) for the nodes defined by the node sets 'node_sets' (the given node nets is supposed to be present in the associated mesh. If note, it will raise an error). >>> pb.bc.add('Dirichlet','node_sets', 'Disp', 0) External force on the node 112 with Fx = 5, Fy = 10 and Fz = 0. >>> pb.bc.add('Neumann', [112], 'Disp', [5, 10, 0]) Enforce a nul displacement on nodes 1, 2 and 3, and a rotation around X = 0 for node 1, 0.1 for node 2 and 0.2 for node 3. >>> pb.bc.add('Dirichlet', >>> [1,2,3], >>> ['Disp','RotX'], >>> [0, np.array([0,0.1,0.2])] >>> ) Instead of adding directly the boundary conditions to the problem, it may be convenient to create boundary conditions and add them afterwards >>> my_bc = fd.BoundaryCondition.create('Dirichlet', [1,2,3], 'Disp', 0)]) >>> pb.bc.add(my_bc) For non linear problem, we can also defined the time_func to sepcify how the boundary condition evolve during time. By default, a linear evolution is enforced. The time function depend on the time_factor. The time_factor is 0 at the begining and 1 at the end of the iteration. The time function is also a factor to the prescribed value and should be between 0 and 1. >>> def step_function(t_fact): >>> if t_fact == 0: return 0 >>> else: return 1 >>> pb.bc.add('Dirichlet', 'nodeset', 'Disp', 1, time_func = step_function)]) Multi Point Constraints ____________________________________________ .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.MPC Avdanced BC and constraints ============================== Distributed loads are applied to a Problem by building dedicated assembly objects. To add them to a problem, one should add the constraint assembly to the assembly defining the stiffness matrix. .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.constraint.DistributedForce fedoo.constraint.Pressure fedoo.constraint.SurfaceForce Some advanced constraints base on multiple linearized MPC are available in fedoo. They can be created and add to the problem with the pb.bc.add method. .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.constraint.PeriodicBC fedoo.constraint.RigidTie fedoo.constraint.RigidTie2D Contact ============================== Fedoo provides two contact approaches: a **penalty-based** method and an **IPC (Incremental Potential Contact)** method. Both are implemented as assembly objects and can be combined with other assemblies using :py:meth:`fedoo.Assembly.sum`. Penalty-based contact ______________________ The penalty method uses a node-to-surface formulation. It is available for 2D problems and supports frictionless contact. .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.constraint.Contact fedoo.constraint.SelfContact The contact class is derived from assembly. To add a contact contraint to a problem, we need first to create the contact assembly (using the class :py:class:`fedoo.constraint.Contact`) and then to add it to the global assembly with :py:meth:`fedoo.Assembly.sum`. IPC contact ______________________ The IPC (Incremental Potential Contact) method uses barrier potentials from the `ipctk `_ library to guarantee intersection-free configurations. It supports both 2D and 3D problems, friction, and optional CCD (Continuous Collision Detection) line search. Unlike the penalty method, IPC does **not** require tuning a penalty parameter. The barrier stiffness :math:`\kappa` is automatically computed and adaptively updated to balance the elastic and contact forces. The only physical parameter is ``dhat`` — the barrier activation distance that controls the minimum gap between surfaces (default: 0.1% of the bounding box diagonal). **Choosing dhat** --- The default ``dhat=1e-3`` (relative) means the barrier activates when surfaces are within 0.1 % of the bounding-box diagonal. For problems with a very small initial gap, increase ``dhat`` (e.g. ``1e-2``) so the barrier catches contact early. For tight-fitting assemblies where a visible gap is unacceptable, decrease it (e.g. ``1e-4``), but expect more Newton–Raphson iterations. **CCD line search** --- Enabling ``use_ccd=True`` is recommended for problems where first contact occurs suddenly (e.g. a punch hitting a plate) or where self-contact can cause rapid topology changes. **Energy-based backtracking** --- When ``use_ccd=True``, an energy-based backtracking phase is automatically enabled after CCD filtering: the step is halved until total energy (exact barrier + quadratic elastic approximation) decreases. This matches the reference IPC algorithm and improves convergence robustness. Set ``line_search_energy=False`` to disable (faster but may degrade convergence for difficult contact scenarios). **Convergence criterion** --- The ``'Force'`` convergence criterion is recommended for IPC contact problems. It measures the relative decrease of the force residual, matching the gradient-norm convergence used by reference IPC implementations:: pb.set_nr_criterion('Force', tol=5e-3, max_subiter=15) The ``'Displacement'`` criterion may become unreliable as contact stiffness grows. The ``ipctk`` package is required and can be installed with: .. code-block:: bash pip install ipctk # or pip install fedoo[ipc] .. autosummary:: :toctree: generated/ :template: custom-class-template.rst fedoo.constraint.IPCContact fedoo.constraint.IPCSelfContact Penalty contact example __________________________ Here an example of a contact between a square and a disk using the penalty method. .. code-block:: python import fedoo as fd import numpy as np fd.ModelingSpace("2D") filename = 'disk_rectangle_contact' #file to save results #---- Create geometries -------------- mesh_rect = fd.mesh.rectangle_mesh(nx=11, ny=21, x_min=0, x_max=1, y_min=0, y_max=1, elm_type = 'quad4', name = 'Domain' ) mesh_rect.element_sets['rect'] = np.arange(0, mesh_rect.n_elements) mesh_disk = fd.mesh.disk_mesh(radius=0.5, nr=6, nt=6, elm_type = 'quad4') mesh_disk.nodes+=np.array([1.5,0.48]) # translate disk on the right mesh_disk.element_sets['disk'] = np.arange(0,mesh_disk.n_elements) mesh = fd.Mesh.stack(mesh_rect,mesh_disk) #node sets for boundary conditions nodes_left = mesh.find_nodes('X',0) nodes_right = mesh.find_nodes('X',1) nodes_bc = mesh.find_nodes('X>1.5') nodes_bc = list(set(nodes_bc).intersection(mesh.node_sets['boundary'])) #---- Define contact -------------- #slave surface = right face of rectangle mesh nodes_contact = nodes_right surf = fd.mesh.extract_surface(mesh.extract_elements('disk')) contact = fd.constraint.Contact(nodes_contact, surf) contact.contact_search_once = True contact.eps_n = 5e5 #---- Material properties -------------- props = np.array([200e3, 0.3, 1e-5, 300, 1000, 0.3]) # E, nu, alpha (non used), Re, k, m material_rect = fd.constitutivelaw.Simcoon("EPICP", props) material_disk = fd.constitutivelaw.ElasticIsotrop(50e3, 0.3) #E, nu material = fd.constitutivelaw.Heterogeneous( (material_rect, material_disk), ('rect', 'disk') ) #---- Build problem -------------- wf = fd.weakform.StressEquilibrium(material, nlgeom = True) solid_assembly = fd.Assembly.create(wf, mesh) assembly = fd.Assembly.sum(solid_assembly, contact) pb = fd.problem.NonLinear(assembly) results = pb.add_output(filename, solid_assembly, ['Disp', 'Stress', 'Strain', 'Fext'] ) pb.bc.add('Dirichlet',nodes_left, 'Disp',0) pb.bc.add('Dirichlet',nodes_bc, 'Disp', [-0.4,0.2]) pb.set_nr_criterion("Displacement", tol = 5e-3, max_subiter = 5) #---- Solve problem in two steps: load, unload -------------- pb.nlsolve(dt = 0.005, tmax = 1, update_dt = True, interval_output = 0.01) pb.bc.remove(-1) #remove last boundary contidion pb.bc.add('Dirichlet',nodes_bc, 'Disp', [0,0]) pb.nlsolve(dt = 0.005, tmax = 1, update_dt = True, interval_output = 0.01) # ============================================================= # Example of plots with pyvista - uncomment the desired plot # ============================================================= # ------------------------------------ # Simple plot with default options # ------------------------------------ results.plot('Stress', component='vm', data_type='Node') results.plot('Disp', component = 0, data_type='Node') # ------------------------------------ # Write movie with default options # ------------------------------------ results.write_movie(filename, 'Stress', component = 'XX', data_type = 'Node', framerate = 24, quality = 5, clim = [-3e3, 3e3] ) Video of results: :download:`contact video <./_static/examples/disk_rectangle_contact.mp4>` IPC contact example __________________________ The same disk-rectangle contact problem can be solved with the IPC method. The IPC method does not require choosing slave/master nodes or tuning a penalty parameter. The barrier stiffness is automatically computed and adapted. .. code-block:: python import fedoo as fd import numpy as np fd.ModelingSpace("2D") #---- Create geometries (same as penalty example) -------------- mesh_rect = fd.mesh.rectangle_mesh(nx=11, ny=21, x_min=0, x_max=1, y_min=0, y_max=1, elm_type='quad4', name='Domain') mesh_disk = fd.mesh.disk_mesh(radius=0.5, nr=6, nt=6, elm_type='quad4') mesh_disk.nodes += np.array([1.5, 0.48]) mesh = fd.Mesh.stack(mesh_rect, mesh_disk) #---- Define IPC contact -------------- surf = fd.mesh.extract_surface(mesh) ipc_contact = fd.constraint.IPCContact( mesh, surface_mesh=surf, friction_coefficient=0.3, # Coulomb friction coefficient use_ccd=True, # enable CCD line search for robustness ) # barrier_stiffness is auto-computed; dhat defaults to 1e-3 * bbox_diag #---- Material and problem setup -------------- material = fd.constitutivelaw.ElasticIsotrop(200e3, 0.3) wf = fd.weakform.StressEquilibrium(material, nlgeom=True) solid_assembly = fd.Assembly.create(wf, mesh) assembly = fd.Assembly.sum(solid_assembly, ipc_contact) pb = fd.problem.NonLinear(assembly) res = pb.add_output('results', solid_assembly, ['Disp', 'Stress']) # ... add BCs ... pb.nlsolve(dt=0.005, tmax=1) .. note:: When using ``add_output``, pass the **solid assembly** (not the sum). ``AssemblySum`` objects cannot be used directly for output extraction. IPC self-contact example __________________________ For self-contact problems, use :py:class:`~fedoo.constraint.IPCSelfContact` which automatically extracts the surface from the volumetric mesh. .. code-block:: python import fedoo as fd import numpy as np fd.ModelingSpace("3D") mesh = fd.Mesh.read("gyroid.vtk") material = fd.constitutivelaw.ElasticIsotrop(1e5, 0.3) # Self-contact: auto surface extraction, auto barrier stiffness # Add line_search_energy=True for extra robustness (slower) contact = fd.constraint.IPCSelfContact(mesh, use_ccd=True) wf = fd.weakform.StressEquilibrium(material, nlgeom="UL") solid = fd.Assembly.create(wf, mesh) assembly = fd.Assembly.sum(solid, contact) pb = fd.problem.NonLinear(assembly) res = pb.add_output("results", solid, ["Disp", "Stress"]) # ... add BCs ... pb.nlsolve(dt=0.05, tmax=1, update_dt=True)