===================================== 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. .. autoclass:: fedoo.ListBC :members: Dirichlet and Neumann Boundary conditions ____________________________________________ 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 ============================== A first implementation of the contact is proposed for 2D problems. Contact is still in development and subject to slight change in future versions. For now, only frictionless contact is implemented. .. 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`. Example -------------- Here an example of a contact between a square and a disk. .. 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>`