.. _demo_hyperelasticity: Hyperelasticity =============== This demo is implemented in a single Python file, :download:`demo_hyperelasticity.py`, which contains both the variational forms and the solver. Background ---------- This example demonstrates the solution of a three-dimensional elasticity problem. In addition to illustrating how to use FunctionSpaces, Expressions and how to apply Dirichlet boundary conditions, it focuses on how to: * Minimise a non-quadratic functional * Use automatic computation of the directional derivative * Solve a nonlinear variational problem * Define compiled sub-domains * Use specific form compiler optimization options Equation and problem definition ------------------------------- By definition, boundary value problems for hyperelastic media can be expressed as minimisation problems, and the minimization approach is adopted in this example. For a domain :math:`\Omega \subset \mathbb{R}^{d}`, where :math:`d` denotes the spatial dimension, the task is to find the displacement field :math:`u: \Omega \rightarrow \mathbb{R}^{d}` that minimises the total potential energy :math:`\Pi`: .. math:: \min_{u \in V} \Pi, where :math:`V` is a suitable function space that satisfies boundary conditions on :math:`u`. The total potential energy is given by .. math:: \Pi = \int_{\Omega} \psi(u) \, {\rm d} x - \int_{\Omega} B \cdot u \, {\rm d} x - \int_{\partial\Omega} T \cdot u \, {\rm d} s, where :math:`\psi` is the elastic stored energy density, :math:`B` is a body force (per unit reference volume) and :math:`T` is a traction force (per unit reference area). At minimum points of :math:`\Pi`, the directional derivative of :math:`\Pi` with respect to change in :math:`u` .. math:: :label: first_variation L(u; v) = D_{v} \Pi = \left. \frac{d \Pi(u + \epsilon v)}{d\epsilon} \right|_{\epsilon = 0} is equal to zero for all :math:`v \in V`: .. math:: L(u; v) = 0 \quad \forall \ v \in V. To minimise the potential energy, a solution to the variational equation above is sought. Depending on the potential energy :math:`\psi`, :math:`L(u; v)` can be nonlinear in :math:`u`. In such a case, the Jacobian of :math:`L` is required in order to solve this problem using Newton's method. The Jacobian of :math:`L` is defined as .. math:: :label: second_variation a(u; du, v) = D_{du} L = \left. \frac{d L(u + \epsilon du; v)}{d\epsilon} \right|_{\epsilon = 0} . Elastic stored energy density ^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^ To define the elastic stored energy density, consider the deformation gradient :math:`F` .. math:: F = I + \nabla u, the right Cauchy-Green tensor :math:`C` .. math:: C = F^{T} F, and the scalars :math:`J` and :math:`I_{c}` .. math:: J &= \det(F), \\ I_{c} &= {\rm trace}(C). This demo considers a common neo-Hookean stored energy model of the form .. math:: \psi = \frac{\mu}{2} (I_{c} - 3) - \mu \ln(J) + \frac{\lambda}{2}\ln(J)^{2}, where :math:`\mu` and :math:`\lambda` are the Lame parameters. These can be expressed in terms of the more common Young's modulus :math:`E` and Poisson ratio :math:`\nu` by: .. math:: \lambda = \frac{E \nu}{(1 + \nu)(1 - 2\nu)}, \quad \quad \mu = \frac{E}{2(1 + \nu)} . Demo parameters ^^^^^^^^^^^^^^^ We consider a unit cube domain: * :math:`\Omega = (0, 1) \times (0, 1) \times (0, 1)` (unit cube) We use the following definitions of the boundary and boundary conditions: * :math:`\Gamma_{D_{0}} = 0 \times (0, 1) \times (0, 1)` (Dirichlet boundary) * :math:`\Gamma_{D_{1}} = 1 \times (0, 1) \times (0, 1)` (Dirichlet boundary) * :math:`\Gamma_{N} = \partial \Omega \backslash \Gamma_{D}` (Neumann boundary) * On :math:`\Gamma_{D_{0}}`: :math:`u = (0, 0, 0)` * On :math:`\Gamma_{D_{1}}` .. math:: u = (&0, \\ &(0.5 + (y - 0.5)\cos(\pi/3) - (z - 0.5)\sin(\pi/3) - y)/2, \\ &(0.5 + (y - 0.5)\sin(\pi/3) + (z - 0.5)\cos(\pi/3) - z))/2) * On :math:`\Gamma_{N}`: :math:`T = (0.1, 0, 0)` These are the body forces and material parameters used: * :math:`B = (0, -0.5, 0)` * :math:`E = 10.0` * :math:`\nu = 0.3` With the above input the solution for :math:`u` will look as follows: .. image:: hyperelasticity_u0.png :scale: 75 :align: center .. image:: hyperelasticity_u1.png :scale: 75 :align: center Implementation -------------- This demo is implemented in the :download:`demo_hyperelasticity.py` file. First, the required modules are imported:: import matplotlib.pyplot as plt from dolfin import * The behavior of the form compiler FFC can be adjusted by prescribing various parameters. Here, we want to use the UFLACS backend of FFC:: # Optimization options for the form compiler parameters["form_compiler"]["cpp_optimize"] = True parameters["form_compiler"]["representation"] = "uflacs" The first line tells the form compiler to use C++ compiler optimizations when compiling the generated code. The remainder is a dictionary of options which will be passed to the form compiler. It lists the optimizations strategies that we wish the form compiler to use when generating code. .. index:: VectorFunctionSpace First, we need a tetrahedral mesh of the domain and a function space on this mesh. Here, we choose to create a unit cube mesh with 25 ( = 24 + 1) vertices in one direction and 17 ( = 16 + 1) vertices in the other two direction. On this mesh, we define a function space of continuous piecewise linear vector polynomials (a Lagrange vector element space):: # Create mesh and define function space mesh = UnitCubeMesh(24, 16, 16) V = VectorFunctionSpace(mesh, "Lagrange", 1) Note that :py:class:`VectorFunctionSpace ` creates a function space of vector fields. The dimension of the vector field (the number of components) is assumed to be the same as the spatial dimension, unless otherwise specified. .. index:: compiled subdomain The portions of the boundary on which Dirichlet boundary conditions will be applied are now defined:: # Mark boundary subdomians left = CompiledSubDomain("near(x[0], side) && on_boundary", side = 0.0) right = CompiledSubDomain("near(x[0], side) && on_boundary", side = 1.0) The boundary subdomain ``left`` corresponds to the part of the boundary on which :math:`x=0` and the boundary subdomain ``right`` corresponds to the part of the boundary on which :math:`x=1`. Note that C++ syntax is used in the :py:func:`CompiledSubDomain` ` function since the function will be automatically compiled into C++ code for efficiency. The (built-in) variable ``on_boundary`` is true for points on the boundary of a domain, and false otherwise. .. index:: compiled expression The Dirichlet boundary values are defined using compiled expressions:: # Define Dirichlet boundary (x = 0 or x = 1) c = Constant((0.0, 0.0, 0.0)) r = Expression(("scale*0.0", "scale*(y0 + (x[1] - y0)*cos(theta) - (x[2] - z0)*sin(theta) - x[1])", "scale*(z0 + (x[1] - y0)*sin(theta) + (x[2] - z0)*cos(theta) - x[2])"), scale = 0.5, y0 = 0.5, z0 = 0.5, theta = pi/3, degree=2) Note the use of setting named parameters in the :py:class:`Expression ` for ``r``. The boundary subdomains and the boundary condition expressions are collected together in two :py:class:`DirichletBC ` objects, one for each part of the Dirichlet boundary:: bcl = DirichletBC(V, c, left) bcr = DirichletBC(V, r, right) bcs = [bcl, bcr] The Dirichlet (essential) boundary conditions are constraints on the function space :math:`V`. The function space is therefore required as an argument to :py:class:`DirichletBC `. .. index:: TestFunction, TrialFunction, Constant Trial and test functions, and the most recent approximate displacement ``u`` are defined on the finite element space ``V``, and two objects of type :py:class:`Constant ` are declared for the body force (``B``) and traction (``T``) terms:: # Define functions du = TrialFunction(V) # Incremental displacement v = TestFunction(V) # Test function u = Function(V) # Displacement from previous iteration B = Constant((0.0, -0.5, 0.0)) # Body force per unit volume T = Constant((0.1, 0.0, 0.0)) # Traction force on the boundary In place of :py:class:`Constant `, it is also possible to use ``as_vector``, e.g. ``B = as_vector( [0.0, -0.5, 0.0] )``. The advantage of Constant is that its values can be changed without requiring re-generation and re-compilation of C++ code. On the other hand, using ``as_vector`` can eliminate some function calls during assembly. With the functions defined, the kinematic quantities involved in the model are defined using UFL syntax:: # Kinematics d = len(u) I = Identity(d) # Identity tensor F = I + grad(u) # Deformation gradient C = F.T*F # Right Cauchy-Green tensor # Invariants of deformation tensors Ic = tr(C) J = det(F) Next, the material parameters are set and the strain energy density and the total potential energy are defined, again using UFL syntax:: # Elasticity parameters E, nu = 10.0, 0.3 mu, lmbda = Constant(E/(2*(1 + nu))), Constant(E*nu/((1 + nu)*(1 - 2*nu))) # Stored strain energy density (compressible neo-Hookean model) psi = (mu/2)*(Ic - 3) - mu*ln(J) + (lmbda/2)*(ln(J))**2 # Total potential energy Pi = psi*dx - dot(B, u)*dx - dot(T, u)*ds Just as for the body force and traction vectors, :py:class:`Constant ` has been used for the model parameters ``mu`` and ``lmbda`` to avoid re-generation of C++ code when changing model parameters. Note that ``lambda`` is a reserved keyword in Python, hence the misspelling ``lmbda``. .. index:: directional derivative; derivative, taking variations; derivative, automatic differentiation; derivative Directional derivatives are now computed of :math:`\Pi` and :math:`L` (see :eq:`first_variation` and :eq:`second_variation`):: # Compute first variation of Pi (directional derivative about u in the direction of v) F = derivative(Pi, u, v) # Compute Jacobian of F J = derivative(F, u, du) The complete variational problem can now be solved by a single call to :py:func:`solve `:: # Solve variational problem solve(F == 0, u, bcs, J=J) Finally, the solution ``u`` is saved to a file named ``displacement.pvd`` in VTK format, and the deformed mesh is plotted to the screen:: # Save solution in VTK format file = File("displacement.pvd"); file << u; # Plot solution plot(u) plt.show()