Dear Amir (and Hamed),
> Integration stress on external faces is correct when the material
> constitutive model is linear (for example elastic material model in which
> behavior is not history dependent). It is better to extract residual forces
> at the boundary from the system residual vector.
>
I disagree and consider both statements that you've made to be incorrect.
For starters, in a nonlinear problem one uses a nonlinear solution scheme
to drive the residual (a consequence of equilibrium imbalance) down to
zero. So not only does the residual not represent any measure of external
force, but also one expects this vector to be zero in for a balanced system!
In general (for a linear/nonlinear hyperelastic/dissipative material), to
compute the total force acting on the surface of a domain one should
integrate the tractions acting on that surface. As the body is in
equilibrium, they are balanced by the stresses generated by the material.
Using Cauchy's theorum
<https://en.wikipedia.org/wiki/Cauchy_stress_tensor#Cauchy.E2.80.99s_stress_theorem.E2.80.94stress_tensor>
one can re-express this traction in terms of the internal stresses and
compute the forces developed on any arbitrary cut-plane in the material
domain.
To demonstrate, I've attached an example for one-field elasticity that
shows the computation of the reaction forces on either side of a cube under
uniaxial stress conditions. All of the computations are done in the
post-processing step (Solid<dim>::output_results). Since this cube has flat
faces, computing the nodal reaction forces (which, by the way, are
outputted so that you can visualise them as well) and then summing them is
equivalent to directly integrating the contributions over the surface.
I hope that this helps provide you with some clarification on the point
that you made.
Regards,
Jean-Paul
--
The deal.II project is located at http://www.dealii.org/
For mailing list/forum options, see
https://groups.google.com/d/forum/dealii?hl=en
---
You received this message because you are subscribed to the Google Groups
"deal.II User Group" group.
To unsubscribe from this group and stop receiving emails from it, send an email
to dealii+unsubscr...@googlegroups.com.
For more options, visit https://groups.google.com/d/optout.
/* ---------------------------------------------------------------------
* $Id: step-44.cc 30526 2013-08-29 20:06:27Z felix.gruber $
*
* Copyright (C) 2010 - 2013 by the deal.II authors and
* & Jean-Paul Pelteret and Andrew McBride
*
* This file is part of the deal.II library.
*
* The deal.II library is free software; you can use it, redistribute
* it, and/or modify it under the terms of the GNU Lesser General
* Public License as published by the Free Software Foundation; either
* version 2.1 of the License, or (at your option) any later version.
* The full text of the license can be found in the file LICENSE at
* the top level of the deal.II distribution.
*
* ---------------------------------------------------------------------
*/
/*
* Authors: Jean-Paul Pelteret, University of Cape Town,
* Andrew McBride, University of Erlangen-Nuremberg, 2010
*/
// We start by including all the necessary deal.II header files and some C++
// related ones. They have been discussed in detail in previous tutorial
// programs, so you need only refer to past tutorials for details.
#include <deal.II/base/function.h>
#include <deal.II/base/parameter_handler.h>
#include <deal.II/base/point.h>
#include <deal.II/base/quadrature_lib.h>
#include <deal.II/base/symmetric_tensor.h>
#include <deal.II/base/tensor.h>
#include <deal.II/base/timer.h>
#include <deal.II/base/work_stream.h>
#include <deal.II/dofs/dof_renumbering.h>
#include <deal.II/dofs/dof_tools.h>
#include <deal.II/grid/grid_generator.h>
#include <deal.II/grid/grid_tools.h>
#include <deal.II/grid/grid_in.h>
#include <deal.II/grid/tria.h>
#include <deal.II/grid/tria_boundary_lib.h>
#include <deal.II/fe/fe_dgp_monomial.h>
#include <deal.II/fe/fe_q.h>
#include <deal.II/fe/fe_system.h>
#include <deal.II/fe/fe_tools.h>
#include <deal.II/fe/fe_values.h>
#include <deal.II/fe/mapping_q_eulerian.h>
#include <deal.II/lac/block_sparse_matrix.h>
#include <deal.II/lac/block_vector.h>
#include <deal.II/lac/dynamic_sparsity_pattern.h>
#include <deal.II/lac/full_matrix.h>
#include <deal.II/lac/precondition_selector.h>
#include <deal.II/lac/solver_cg.h>
#include <deal.II/lac/sparse_direct.h>
#include <deal.II/lac/constraint_matrix.h>
#include <deal.II/numerics/data_out.h>
#include <deal.II/numerics/vector_tools.h>
#include <iostream>
#include <fstream>
// We then stick everything that relates to this tutorial program into a
// namespace of its own, and import all the deal.II function and class names
// into it:
namespace Step44
{
using namespace dealii;
// @sect3{Run-time parameters}
//
// There are several parameters that can be set in the code so we set up a
// ParameterHandler object to read in the choices at run-time.
namespace Parameters
{
// @sect4{Finite Element system}
// As mentioned in the introduction, a different order interpolation should be
// used for the displacement $\mathbf{u}$ than for the pressure
// $\widetilde{p}$ and the dilatation $\widetilde{J}$. Choosing
// $\widetilde{p}$ and $\widetilde{J}$ as discontinuous (constant) functions
// at the element level leads to the mean-dilatation method. The discontinuous
// approximation allows $\widetilde{p}$ and $\widetilde{J}$ to be condensed
// out and a classical displacement based method is recovered. Here we
// specify the polynomial order used to approximate the solution. The
// quadrature order should be adjusted accordingly.
struct FESystem
{
unsigned int poly_degree;
unsigned int quad_order;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void FESystem::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Finite element system");
{
prm.declare_entry("Polynomial degree", "2",
Patterns::Integer(0),
"Displacement system polynomial order");
prm.declare_entry("Quadrature order", "3",
Patterns::Integer(0),
"Gauss quadrature order");
}
prm.leave_subsection();
}
void FESystem::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Finite element system");
{
poly_degree = prm.get_integer("Polynomial degree");
quad_order = prm.get_integer("Quadrature order");
}
prm.leave_subsection();
}
// @sect4{Geometry}
// Make adjustments to the problem geometry and the applied load. Since the
// problem modelled here is quite specific, the load scale can be altered to
// specific values to compare with the results given in the literature.
struct Geometry
{
unsigned int global_refinement;
double scale;
double pressure;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void Geometry::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Geometry");
{
prm.declare_entry("Global refinement", "2",
Patterns::Integer(0),
"Global refinement level");
prm.declare_entry("Grid scale", "1e-3",
Patterns::Double(0.0),
"Global grid scaling factor");
prm.declare_entry("Pressure", "100",
Patterns::Double(),
"Applied pressure");
}
prm.leave_subsection();
}
void Geometry::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Geometry");
{
global_refinement = prm.get_integer("Global refinement");
scale = prm.get_double("Grid scale");
pressure = prm.get_double("Pressure");
}
prm.leave_subsection();
}
// @sect4{Materials}
// We also need the shear modulus $ \mu $ and Poisson ration $ \nu $ for the
// neo-Hookean material.
struct Materials
{
double nu;
double mu;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void Materials::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Material properties");
{
prm.declare_entry("Poisson's ratio", "0.4999",
Patterns::Double(-1.0,0.5),
"Poisson's ratio");
prm.declare_entry("Shear modulus", "80.194e6",
Patterns::Double(),
"Shear modulus");
}
prm.leave_subsection();
}
void Materials::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Material properties");
{
nu = prm.get_double("Poisson's ratio");
mu = prm.get_double("Shear modulus");
}
prm.leave_subsection();
}
// @sect4{Linear solver}
// Next, we choose both solver and preconditioner settings. The use of an
// effective preconditioner is critical to ensure convergence when a large
// nonlinear motion occurs within a Newton increment.
struct LinearSolver
{
std::string type_lin;
double tol_lin;
double max_iterations_lin;
std::string preconditioner_type;
double preconditioner_relaxation;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void LinearSolver::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Linear solver");
{
prm.declare_entry("Solver type", "CG",
Patterns::Selection("CG|Direct"),
"Type of solver used to solve the linear system");
prm.declare_entry("Residual", "1e-6",
Patterns::Double(0.0),
"Linear solver residual (scaled by residual norm)");
prm.declare_entry("Max iteration multiplier", "1",
Patterns::Double(0.0),
"Linear solver iterations (multiples of the system matrix size)");
prm.declare_entry("Preconditioner type", "ssor",
Patterns::Selection("jacobi|ssor"),
"Type of preconditioner");
prm.declare_entry("Preconditioner relaxation", "0.65",
Patterns::Double(0.0),
"Preconditioner relaxation value");
}
prm.leave_subsection();
}
void LinearSolver::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Linear solver");
{
type_lin = prm.get("Solver type");
tol_lin = prm.get_double("Residual");
max_iterations_lin = prm.get_double("Max iteration multiplier");
preconditioner_type = prm.get("Preconditioner type");
preconditioner_relaxation = prm.get_double("Preconditioner relaxation");
}
prm.leave_subsection();
}
// @sect4{Nonlinear solver}
// A Newton-Raphson scheme is used to solve the nonlinear system of governing
// equations. We now define the tolerances and the maximum number of
// iterations for the Newton-Raphson nonlinear solver.
struct NonlinearSolver
{
unsigned int max_iterations_NR;
double tol_f;
double tol_u;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void NonlinearSolver::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Nonlinear solver");
{
prm.declare_entry("Max iterations Newton-Raphson", "10",
Patterns::Integer(0),
"Number of Newton-Raphson iterations allowed");
prm.declare_entry("Tolerance force", "1.0e-9",
Patterns::Double(0.0),
"Force residual tolerance");
prm.declare_entry("Tolerance displacement", "1.0e-6",
Patterns::Double(0.0),
"Displacement error tolerance");
}
prm.leave_subsection();
}
void NonlinearSolver::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Nonlinear solver");
{
max_iterations_NR = prm.get_integer("Max iterations Newton-Raphson");
tol_f = prm.get_double("Tolerance force");
tol_u = prm.get_double("Tolerance displacement");
}
prm.leave_subsection();
}
// @sect4{Time}
// Set the timestep size $ \varDelta t $ and the simulation end-time.
struct Time
{
double delta_t;
double end_time;
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
void Time::declare_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Time");
{
prm.declare_entry("End time", "1",
Patterns::Double(),
"End time");
prm.declare_entry("Time step size", "0.1",
Patterns::Double(),
"Time step size");
}
prm.leave_subsection();
}
void Time::parse_parameters(ParameterHandler &prm)
{
prm.enter_subsection("Time");
{
end_time = prm.get_double("End time");
delta_t = prm.get_double("Time step size");
}
prm.leave_subsection();
}
// @sect4{All parameters}
// Finally we consolidate all of the above structures into a single container
// that holds all of our run-time selections.
struct AllParameters : public FESystem,
public Geometry,
public Materials,
public LinearSolver,
public NonlinearSolver,
public Time
{
AllParameters(const std::string &input_file);
static void
declare_parameters(ParameterHandler &prm);
void
parse_parameters(ParameterHandler &prm);
};
AllParameters::AllParameters(const std::string &input_file)
{
ParameterHandler prm;
declare_parameters(prm);
prm.parse_input(input_file);
parse_parameters(prm);
}
void AllParameters::declare_parameters(ParameterHandler &prm)
{
FESystem::declare_parameters(prm);
Geometry::declare_parameters(prm);
Materials::declare_parameters(prm);
LinearSolver::declare_parameters(prm);
NonlinearSolver::declare_parameters(prm);
Time::declare_parameters(prm);
}
void AllParameters::parse_parameters(ParameterHandler &prm)
{
FESystem::parse_parameters(prm);
Geometry::parse_parameters(prm);
Materials::parse_parameters(prm);
LinearSolver::parse_parameters(prm);
NonlinearSolver::parse_parameters(prm);
Time::parse_parameters(prm);
}
}
// @sect3{Some standard tensors}
// Now we define some frequently used second and fourth-order tensors:
template <int dim>
class StandardTensors
{
public:
// $\mathbf{I}$
static const SymmetricTensor<2, dim> I;
// $\mathbf{I} \otimes \mathbf{I}$
static const SymmetricTensor<4, dim> IxI;
// $\mathcal{S}$, note that as we only use this fourth-order unit tensor
// to operate on symmetric second-order tensors. To maintain notation
// consistent with Holzapfel (2001) we name the tensor $\mathcal{I}$
static const SymmetricTensor<4, dim> II;
// Fourth-order deviatoric tensor such that
// $\textrm{dev} \{ \bullet \} = \{ \bullet \} -
// [1/\textrm{dim}][ \{ \bullet\} :\mathbf{I}]\mathbf{I}$
static const SymmetricTensor<4, dim> dev_P;
};
template <int dim>
const SymmetricTensor<2, dim>
StandardTensors<dim>::I = unit_symmetric_tensor<dim>();
template <int dim>
const SymmetricTensor<4, dim>
StandardTensors<dim>::IxI = outer_product(I, I);
template <int dim>
const SymmetricTensor<4, dim>
StandardTensors<dim>::II = identity_tensor<dim>();
template <int dim>
const SymmetricTensor<4, dim>
StandardTensors<dim>::dev_P = deviator_tensor<dim>();
// @sect3{Time class}
// A simple class to store time data. Its functioning is transparent so no
// discussion is necessary. For simplicity we assume a constant time step
// size.
class Time
{
public:
Time (const double time_end,
const double delta_t)
:
timestep(0),
time_current(0.0),
time_end(time_end),
delta_t(delta_t)
{}
virtual ~Time()
{}
double current() const
{
return time_current;
}
double end() const
{
return time_end;
}
double get_delta_t() const
{
return delta_t;
}
unsigned int get_timestep() const
{
return timestep;
}
void increment()
{
time_current += delta_t;
++timestep;
}
private:
unsigned int timestep;
double time_current;
const double time_end;
const double delta_t;
};
// @sect3{Compressible neo-Hookean material within a three-field formulation}
// As discussed in the Introduction, Neo-Hookean materials are a type of
// hyperelastic materials. The entire domain is assumed to be composed of a
// compressible neo-Hookean material. This class defines the behaviour of
// this material within a three-field formulation. Compressible neo-Hookean
// materials can be described by a strain-energy function (SEF) $ \Psi =
// \Psi_{\text{iso}}(\overline{\mathbf{b}}) + \Psi_{\text{vol}}(\widetilde{J})
// $.
//
// The isochoric response is given by $
// \Psi_{\text{iso}}(\overline{\mathbf{b}}) = c_{1} [\overline{I}_{1} - 3] $
// where $ c_{1} = \frac{\mu}{2} $ and $\overline{I}_{1}$ is the first
// invariant of the left- or right-isochoric Cauchy-Green deformation tensors.
// That is $\overline{I}_1 :=\textrm{tr}(\overline{\mathbf{b}})$. In this
// example the SEF that governs the volumetric response is defined as $
// \Psi_{\text{vol}}(\widetilde{J}) = \kappa \frac{1}{4} [ \widetilde{J}^2 - 1
// - 2\textrm{ln}\; \widetilde{J} ]$, where $\kappa:= \lambda + 2/3 \mu$ is
// the <a href="http://en.wikipedia.org/wiki/Bulk_modulus";>bulk modulus</a>
// and $\lambda$ is <a
// href="http://en.wikipedia.org/wiki/Lam%C3%A9_parameters";>Lame's first
// parameter</a>.
//
// The following class will be used to characterize the material we work with,
// and provides a central point that one would need to modify if one were to
// implement a different material model. For it to work, we will store one
// object of this type per quadrature point, and in each of these objects
// store the current state (characterized by the values or measures of the three fields)
// so that we can compute the elastic coefficients linearized around the
// current state.
template <int dim>
class Material_Compressible_Neo_Hook_One_Field
{
public:
Material_Compressible_Neo_Hook_One_Field(const double mu,
const double nu)
:
kappa((2.0 * mu * (1.0 + nu)) / (3.0 * (1.0 - 2.0 * nu))),
c_1(mu / 2.0),
det_F(1.0),
b_bar(StandardTensors<dim>::I)
{
Assert(kappa > 0, ExcInternalError());
}
~Material_Compressible_Neo_Hook_One_Field()
{}
// We update the material model with various deformation dependent data
// based on $F$ and the pressure $\widetilde{p}$ and dilatation
// $\widetilde{J}$, and at the end of the function include a physical
// check for internal consistency:
void update_material_data(const Tensor<2, dim> &F)
{
det_F = determinant(F);
b_bar = std::pow(det_F, -2.0 / 3.0) * symmetrize(F * transpose(F));
Assert(det_F > 0, ExcInternalError());
}
// The second function determines the Kirchhoff stress $\boldsymbol{\tau}
// = \boldsymbol{\tau}_{\textrm{iso}} + \boldsymbol{\tau}_{\textrm{vol}}$
SymmetricTensor<2, dim> get_tau()
{
// See Holzapfel p231 eq6.98 onwards
return get_tau_iso() + get_tau_vol();
}
// The fourth-order elasticity tensor in the spatial setting
// $\mathfrak{c}$ is calculated from the SEF $\Psi$ as $ J
// \mathfrak{c}_{ijkl} = F_{iA} F_{jB} \mathfrak{C}_{ABCD} F_{kC} F_{lD}$
// where $ \mathfrak{C} = 4 \frac{\partial^2 \Psi(\mathbf{C})}{\partial
// \mathbf{C} \partial \mathbf{C}}$
SymmetricTensor<4, dim> get_Jc() const
{
return get_Jc_vol() + get_Jc_iso();
}
// Derivative of the volumetric free energy with respect to
// $\widetilde{J}$ return $\frac{\partial
// \Psi_{\text{vol}}(\widetilde{J})}{\partial \widetilde{J}}$
double get_dPsi_vol_dJ() const
{
return (kappa / 2.0) * (det_F - 1.0 / det_F);
}
// Second derivative of the volumetric free energy wrt $\widetilde{J}$. We
// need the following computation explicitly in the tangent so we make it
// public. We calculate $\frac{\partial^2
// \Psi_{\textrm{vol}}(\widetilde{J})}{\partial \widetilde{J} \partial
// \widetilde{J}}$
double get_d2Psi_vol_dJ2() const
{
return ( (kappa / 2.0) * (1.0 + 1.0 / (det_F * det_F)));
}
// The next few functions return various data that we choose to store with
// the material:
double get_det_F() const
{
return det_F;
}
protected:
// Define constitutive model parameters $\kappa$ (bulk modulus) and the
// neo-Hookean model parameter $c_1$:
const double kappa;
const double c_1;
// Model specific data that is convenient to store with the material:
double det_F;
SymmetricTensor<2, dim> b_bar;
// The following functions are used internally in determining the result
// of some of the public functions above. The first one determines the
// volumetric Kirchhoff stress $\boldsymbol{\tau}_{\textrm{vol}}$:
SymmetricTensor<2, dim> get_tau_vol() const
{
return get_dPsi_vol_dJ() * det_F * StandardTensors<dim>::I;
}
// Next, determine the isochoric Kirchhoff stress
// $\boldsymbol{\tau}_{\textrm{iso}} =
// \mathcal{P}:\overline{\boldsymbol{\tau}}$:
SymmetricTensor<2, dim> get_tau_iso() const
{
return StandardTensors<dim>::dev_P * get_tau_bar();
}
// Then, determine the fictitious Kirchhoff stress
// $\overline{\boldsymbol{\tau}}$:
SymmetricTensor<2, dim> get_tau_bar() const
{
return 2.0 * c_1 * b_bar;
}
// Calculate the volumetric part of the tangent $J
// \mathfrak{c}_\textrm{vol}$:
SymmetricTensor<4, dim> get_Jc_vol() const
{
// See Holzapfel p265
return det_F
* ( (get_dPsi_vol_dJ() + det_F * get_d2Psi_vol_dJ2())*StandardTensors<dim>::IxI
- (2.0 * get_dPsi_vol_dJ())*StandardTensors<dim>::II );
}
// Calculate the isochoric part of the tangent $J
// \mathfrak{c}_\textrm{iso}$:
SymmetricTensor<4, dim> get_Jc_iso() const
{
const SymmetricTensor<2, dim> tau_bar = get_tau_bar();
const SymmetricTensor<2, dim> tau_iso = get_tau_iso();
const SymmetricTensor<4, dim> tau_iso_x_I
= outer_product(tau_iso,
StandardTensors<dim>::I);
const SymmetricTensor<4, dim> I_x_tau_iso
= outer_product(StandardTensors<dim>::I,
tau_iso);
const SymmetricTensor<4, dim> c_bar = get_c_bar();
return (2.0 / 3.0) * trace(tau_bar)
* StandardTensors<dim>::dev_P
- (2.0 / 3.0) * (tau_iso_x_I + I_x_tau_iso)
+ StandardTensors<dim>::dev_P * c_bar
* StandardTensors<dim>::dev_P;
}
// Calculate the fictitious elasticity tensor $\overline{\mathfrak{c}}$.
// For the material model chosen this is simply zero:
SymmetricTensor<4, dim> get_c_bar() const
{
return SymmetricTensor<4, dim>();
}
};
// @sect3{Quadrature point history}
// As seen in step-18, the <code> PointHistory </code> class offers a method
// for storing data at the quadrature points. Here each quadrature point
// holds a pointer to a material description. Thus, different material models
// can be used in different regions of the domain. Among other data, we
// choose to store the Kirchhoff stress $\boldsymbol{\tau}$ and the tangent
// $J\mathfrak{c}$ for the quadrature points.
template <int dim>
class PointHistory
{
public:
PointHistory()
:
material(NULL),
F_inv(StandardTensors<dim>::I),
tau(SymmetricTensor<2, dim>()),
Jc(SymmetricTensor<4, dim>())
{}
virtual ~PointHistory()
{
delete material;
material = NULL;
}
// The first function is used to create a material object and to
// initialize all tensors correctly: The second one updates the stored
// values and stresses based on the current deformation measure
// $\textrm{Grad}\mathbf{u}_{\textrm{n}}$, pressure $\widetilde{p}$ and
// dilation $\widetilde{J}$ field values.
void setup_lqp (const Parameters::AllParameters ¶meters)
{
material = new Material_Compressible_Neo_Hook_One_Field<dim>(parameters.mu,
parameters.nu);
update_values(Tensor<2, dim>());
}
// To this end, we calculate the deformation gradient $\mathbf{F}$ from
// the displacement gradient $\textrm{Grad}\ \mathbf{u}$, i.e.
// $\mathbf{F}(\mathbf{u}) = \mathbf{I} + \textrm{Grad}\ \mathbf{u}$ and
// then let the material model associated with this quadrature point
// update itself. When computing the deformation gradient, we have to take
// care with which data types we compare the sum $\mathbf{I} +
// \textrm{Grad}\ \mathbf{u}$: Since $I$ has data type SymmetricTensor,
// just writing <code>I + Grad_u_n</code> would convert the second
// argument to a symmetric tensor, perform the sum, and then cast the
// result to a Tensor (i.e., the type of a possibly nonsymmetric
// tensor). However, since <code>Grad_u_n</code> is nonsymmetric in
// general, the conversion to SymmetricTensor will fail. We can avoid this
// back and forth by converting $I$ to Tensor first, and then performing
// the addition as between nonsymmetric tensors:
void update_values (const Tensor<2, dim> &Grad_u_n)
{
const Tensor<2, dim> F
= (Tensor<2, dim>(StandardTensors<dim>::I) +
Grad_u_n);
material->update_material_data(F);
// The material has been updated so we now calculate the Kirchhoff
// stress $\mathbf{\tau}$, the tangent $J\mathfrak{c}$ and the first and
// second derivatives of the volumetric free energy.
//
// We also store the inverse of the deformation gradient since we
// frequently use it:
F_inv = invert(F);
tau = material->get_tau();
Jc = material->get_Jc();
}
// We offer an interface to retrieve certain data. Here are the kinematic
// variables:
double get_det_F() const
{
return material->get_det_F();
}
const Tensor<2, dim> &get_F_inv() const
{
return F_inv;
}
// ...and the kinetic variables. These are used in the material and
// global tangent matrix and residual assembly operations:
const SymmetricTensor<2, dim> &get_tau() const
{
return tau;
}
// And finally the tangent:
const SymmetricTensor<4, dim> &get_Jc() const
{
return Jc;
}
// In terms of member functions, this class stores for the quadrature
// point it represents a copy of a material type in case different
// materials are used in different regions of the domain, as well as the
// inverse of the deformation gradient...
private:
Material_Compressible_Neo_Hook_One_Field<dim> *material;
Tensor<2, dim> F_inv;
// ... and stress-type variables along with the tangent $J\mathfrak{c}$:
SymmetricTensor<2, dim> tau;
SymmetricTensor<4, dim> Jc;
};
// @sect3{Quasi-static quasi-incompressible finite-strain solid}
// The Solid class is the central class in that it represents the problem at
// hand. It follows the usual scheme in that all it really has is a
// constructor, destructor and a <code>run()</code> function that dispatches
// all the work to private functions of this class:
template <int dim>
class Solid
{
public:
Solid(const std::string &input_file);
virtual
~Solid();
void
run();
private:
// In the private section of this class, we first forward declare a number
// of objects that are used in parallelizing work using the WorkStream
// object (see the @ref threads module for more information on this).
//
// We declare such structures for the computation of tangent (stiffness)
// matrix, right hand side, static condensation, and for updating
// quadrature points:
struct PerTaskData_K;
struct ScratchData_K;
struct PerTaskData_RHS;
struct ScratchData_RHS;
struct PerTaskData_UQPH;
struct ScratchData_UQPH;
// We start the collection of member functions with one that builds the
// grid:
void
make_grid();
// Set up the finite element system to be solved:
void
system_setup();
void
determine_component_extractors();
// Several functions to assemble the system and right hand side matrices
// using multithreading. Each of them comes as a wrapper function, one
// that is executed to do the work in the WorkStream model on one cell,
// and one that copies the work done on this one cell into the global
// object that represents it:
void
assemble_system_tangent();
void
assemble_system_tangent_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_K &scratch,
PerTaskData_K &data);
void
copy_local_to_global_K(const PerTaskData_K &data);
void
assemble_system_rhs();
void
assemble_system_rhs_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_RHS &scratch,
PerTaskData_RHS &data);
void
copy_local_to_global_rhs(const PerTaskData_RHS &data);
// Apply Dirichlet boundary conditions on the displacement field
void
make_constraints(const int &it_nr);
// Neumann boundary condition
double
get_pressure() const;
// Create and update the quadrature points. Here, no data needs to be
// copied into a global object, so the copy_local_to_global function is
// empty:
void
setup_qph();
void
update_qph_incremental(const BlockVector<double> &solution_delta);
void
update_qph_incremental_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_UQPH &scratch,
PerTaskData_UQPH &data);
void
copy_local_to_global_UQPH(const PerTaskData_UQPH &/*data*/)
{}
// Solve for the displacement using a Newton-Raphson method. We break this
// function into the nonlinear loop and the function that solves the
// linearized Newton-Raphson step:
void
solve_nonlinear_timestep(BlockVector<double> &solution_delta);
std::pair<unsigned int, double>
solve_linear_system(BlockVector<double> &newton_update);
// Solution retrieval as well as post-processing and writing data to file:
BlockVector<double>
get_total_solution(const BlockVector<double> &solution_delta) const;
void
output_results() const;
// Finally, some member variables that describe the current state: A
// collection of the parameters used to describe the problem setup...
Parameters::AllParameters parameters;
// ...the volume of the reference and current configurations...
double vol_reference;
double vol_current;
// ...and description of the geometry on which the problem is solved:
Triangulation<dim> triangulation;
// Also, keep track of the current time and the time spent evaluating
// certain functions
Time time;
TimerOutput timer;
// A storage object for quadrature point information. See step-18 for
// more on this:
std::vector<PointHistory<dim> > quadrature_point_history;
// A description of the finite-element system including the displacement
// polynomial degree, the degree-of-freedom handler, number of DoFs per
// cell and the extractor objects used to retrieve information from the
// solution vectors:
const unsigned int degree;
const FESystem<dim> fe;
DoFHandler<dim> dof_handler_ref;
const unsigned int dofs_per_cell;
const FEValuesExtractors::Vector u_fe;
// Description of how the block-system is arranged. There are 3 blocks,
// the first contains a vector DOF $\mathbf{u}$ while the other two
// describe scalar DOFs, $\widetilde{p}$ and $\widetilde{J}$.
static const unsigned int n_blocks = 1;
static const unsigned int n_components = dim;
static const unsigned int first_u_component = 0;
enum
{
u_dof = 0
};
std::vector<types::global_dof_index> dofs_per_block;
std::vector<types::global_dof_index> element_indices_u;
// Rules for Gauss-quadrature on both the cell and faces. The number of
// quadrature points on both cells and faces is recorded.
const QGauss<dim> qf_cell;
const QGauss<dim - 1> qf_face;
const unsigned int n_q_points;
const unsigned int n_q_points_f;
// Objects that store the converged solution and right-hand side vectors,
// as well as the tangent matrix. There is a ConstraintMatrix object used
// to keep track of constraints. We make use of a sparsity pattern
// designed for a block system.
ConstraintMatrix constraints;
BlockSparsityPattern sparsity_pattern;
BlockSparseMatrix<double> tangent_matrix;
BlockVector<double> system_rhs;
BlockVector<double> solution_n;
// Then define a number of variables to store norms and update norms and
// normalisation factors.
struct Errors
{
Errors()
:
norm(1.0), u(1.0)
{}
void reset()
{
norm = 1.0;
u = 1.0;
}
void normalise(const Errors &rhs)
{
if (rhs.norm != 0.0)
norm /= rhs.norm;
if (rhs.u != 0.0)
u /= rhs.u;
}
double norm, u;
};
Errors error_residual, error_residual_0, error_residual_norm, error_update,
error_update_0, error_update_norm;
// Methods to calculate error measures
void
get_error_residual(Errors &error_residual);
void
get_error_update(const BlockVector<double> &newton_update,
Errors &error_update);
// Print information to screen in a pleasing way...
static
void
print_conv_header();
void
print_conv_footer();
};
// @sect3{Implementation of the <code>Solid</code> class}
// @sect4{Public interface}
// We initialise the Solid class using data extracted from the parameter file.
template <int dim>
Solid<dim>::Solid(const std::string &input_file)
:
parameters(input_file),
triangulation(Triangulation<dim>::maximum_smoothing),
time(parameters.end_time, parameters.delta_t),
timer(std::cout,
TimerOutput::summary,
TimerOutput::wall_times),
degree(parameters.poly_degree),
// The Finite Element System is composed of dim continuous displacement
// DOFs, and discontinuous pressure and dilatation DOFs. In an attempt to
// satisfy the Babuska-Brezzi or LBB stability conditions (see Hughes
// (2000)), we setup a $Q_n \times DGPM_{n-1} \times DGPM_{n-1}$
// system. $Q_2 \times DGPM_1 \times DGPM_1$ elements satisfy this
// condition, while $Q_1 \times DGPM_0 \times DGPM_0$ elements do
// not. However, it has been shown that the latter demonstrate good
// convergence characteristics nonetheless.
fe(FE_Q<dim>(parameters.poly_degree), dim), // displacement
dof_handler_ref(triangulation),
dofs_per_cell (fe.dofs_per_cell),
u_fe(first_u_component),
dofs_per_block(n_blocks),
qf_cell(parameters.quad_order),
qf_face(parameters.quad_order),
n_q_points (qf_cell.size()),
n_q_points_f (qf_face.size())
{
determine_component_extractors();
}
// The class destructor simply clears the data held by the DOFHandler
template <int dim>
Solid<dim>::~Solid()
{
dof_handler_ref.clear();
}
// In solving the quasi-static problem, the time becomes a loading parameter,
// i.e. we increasing the loading linearly with time, making the two concepts
// interchangeable. We choose to increment time linearly using a constant time
// step size.
//
// We start the function with preprocessing, setting the initial dilatation
// values, and then output the initial grid before starting the simulation
// proper with the first time (and loading)
// increment.
//
// Care must be taken (or at least some thought given) when imposing the
// constraint $\widetilde{J}=1$ on the initial solution field. The constraint
// corresponds to the determinant of the deformation gradient in the undeformed
// configuration, which is the identity tensor.
// We use FE_DGPMonomial bases to interpolate the dilatation field, thus we can't
// simply set the corresponding dof to unity as they correspond to the
// monomial coefficients. Thus we use the VectorTools::project function to do
// the work for us. The VectorTools::project function requires an argument
// indicating the hanging node constraints. We have none in this program
// So we have to create a constraint object. In its original state, constraint
// objects are unsorted, and have to be sorted (using the ConstraintMatrix::close function)
// before they can be used. Have a look at step-21 for more information.
// We only need to enforce the initial condition on the dilatation.
// In order to do this, we make use of a ComponentSelectFunction which acts
// as a mask and sets the J_component of n_components to 1. This is exactly what
// we want. Have a look at its usage in step-20 for more information.
template <int dim>
void Solid<dim>::run()
{
make_grid();
system_setup();
output_results();
time.increment();
// We then declare the incremental solution update $\varDelta
// \mathbf{\Xi}:= \{\varDelta \mathbf{u},\varDelta \widetilde{p},
// \varDelta \widetilde{J} \}$ and start the loop over the time domain.
//
// At the beginning, we reset the solution update for this time step...
BlockVector<double> solution_delta(dofs_per_block);
while (time.current() < time.end())
{
solution_delta = 0.0;
// ...solve the current time step and update total solution vector
// $\mathbf{\Xi}_{\textrm{n}} = \mathbf{\Xi}_{\textrm{n-1}} +
// \varDelta \mathbf{\Xi}$...
solve_nonlinear_timestep(solution_delta);
solution_n += solution_delta;
// ...and plot the results before moving on happily to the next time
// step:
output_results();
time.increment();
}
}
// @sect3{Private interface}
// @sect4{Threading-building-blocks structures}
// The first group of private member functions is related to parallization.
// We use the Threading Building Blocks library (TBB) to perform as many
// computationally intensive distributed tasks as possible. In particular, we
// assemble the tangent matrix and right hand side vector, the static
// condensation contributions, and update data stored at the quadrature points
// using TBB. Our main tool for this is the WorkStream class (see the @ref
// threads module for more information).
// Firstly we deal with the tangent matrix assembly structures. The
// PerTaskData object stores local contributions.
template <int dim>
struct Solid<dim>::PerTaskData_K
{
FullMatrix<double> cell_matrix;
std::vector<types::global_dof_index> local_dof_indices;
PerTaskData_K(const unsigned int dofs_per_cell)
:
cell_matrix(dofs_per_cell, dofs_per_cell),
local_dof_indices(dofs_per_cell)
{}
void reset()
{
cell_matrix = 0.0;
}
};
// On the other hand, the ScratchData object stores the larger objects such as
// the shape-function values array (<code>Nx</code>) and a shape function
// gradient and symmetric gradient vector which we will use during the
// assembly.
template <int dim>
struct Solid<dim>::ScratchData_K
{
FEValues<dim> fe_values_ref;
std::vector<std::vector<double> > Nx;
std::vector<std::vector<Tensor<2, dim> > > grad_Nx;
std::vector<std::vector<SymmetricTensor<2, dim> > > symm_grad_Nx;
ScratchData_K(const FiniteElement<dim> &fe_cell,
const QGauss<dim> &qf_cell,
const UpdateFlags uf_cell)
:
fe_values_ref(fe_cell, qf_cell, uf_cell),
Nx(qf_cell.size(),
std::vector<double>(fe_cell.dofs_per_cell)),
grad_Nx(qf_cell.size(),
std::vector<Tensor<2, dim> >(fe_cell.dofs_per_cell)),
symm_grad_Nx(qf_cell.size(),
std::vector<SymmetricTensor<2, dim> >
(fe_cell.dofs_per_cell))
{}
ScratchData_K(const ScratchData_K &rhs)
:
fe_values_ref(rhs.fe_values_ref.get_fe(),
rhs.fe_values_ref.get_quadrature(),
rhs.fe_values_ref.get_update_flags()),
Nx(rhs.Nx),
grad_Nx(rhs.grad_Nx),
symm_grad_Nx(rhs.symm_grad_Nx)
{}
void reset()
{
const unsigned int n_q_points = Nx.size();
const unsigned int n_dofs_per_cell = Nx[0].size();
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
Assert( Nx[q_point].size() == n_dofs_per_cell, ExcInternalError());
Assert( grad_Nx[q_point].size() == n_dofs_per_cell,
ExcInternalError());
Assert( symm_grad_Nx[q_point].size() == n_dofs_per_cell,
ExcInternalError());
for (unsigned int k = 0; k < n_dofs_per_cell; ++k)
{
Nx[q_point][k] = 0.0;
grad_Nx[q_point][k] = 0.0;
symm_grad_Nx[q_point][k] = 0.0;
}
}
}
};
// Next, the same approach is used for the right-hand side assembly. The
// PerTaskData object again stores local contributions and the ScratchData
// object the shape function object and precomputed values vector:
template <int dim>
struct Solid<dim>::PerTaskData_RHS
{
Vector<double> cell_rhs;
std::vector<types::global_dof_index> local_dof_indices;
PerTaskData_RHS(const unsigned int dofs_per_cell)
:
cell_rhs(dofs_per_cell),
local_dof_indices(dofs_per_cell)
{}
void reset()
{
cell_rhs = 0.0;
}
};
template <int dim>
struct Solid<dim>::ScratchData_RHS
{
FEValues<dim> fe_values_ref;
FEFaceValues<dim> fe_face_values_ref;
std::vector<std::vector<double> > Nx;
std::vector<std::vector<SymmetricTensor<2, dim> > > symm_grad_Nx;
ScratchData_RHS(const FiniteElement<dim> &fe_cell,
const QGauss<dim> &qf_cell, const UpdateFlags uf_cell,
const QGauss<dim - 1> & qf_face, const UpdateFlags uf_face)
:
fe_values_ref(fe_cell, qf_cell, uf_cell),
fe_face_values_ref(fe_cell, qf_face, uf_face),
Nx(qf_cell.size(),
std::vector<double>(fe_cell.dofs_per_cell)),
symm_grad_Nx(qf_cell.size(),
std::vector<SymmetricTensor<2, dim> >
(fe_cell.dofs_per_cell))
{}
ScratchData_RHS(const ScratchData_RHS &rhs)
:
fe_values_ref(rhs.fe_values_ref.get_fe(),
rhs.fe_values_ref.get_quadrature(),
rhs.fe_values_ref.get_update_flags()),
fe_face_values_ref(rhs.fe_face_values_ref.get_fe(),
rhs.fe_face_values_ref.get_quadrature(),
rhs.fe_face_values_ref.get_update_flags()),
Nx(rhs.Nx),
symm_grad_Nx(rhs.symm_grad_Nx)
{}
void reset()
{
const unsigned int n_q_points = Nx.size();
const unsigned int n_dofs_per_cell = Nx[0].size();
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
Assert( Nx[q_point].size() == n_dofs_per_cell, ExcInternalError());
Assert( symm_grad_Nx[q_point].size() == n_dofs_per_cell,
ExcInternalError());
for (unsigned int k = 0; k < n_dofs_per_cell; ++k)
{
Nx[q_point][k] = 0.0;
symm_grad_Nx[q_point][k] = 0.0;
}
}
}
};
// And finally we define the structures to assist with updating the quadrature
// point information. Similar to the SC assembly process, we do not need the
// PerTaskData object (since there is nothing to store here) but must define
// one nonetheless. Note that this is because for the operation that we have
// here -- updating the data on quadrature points -- the operation is purely
// local: the things we do on every cell get consumed on every cell, without
// any global aggregation operation as is usually the case when using the
// WorkStream class. The fact that we still have to define a per-task data
// structure points to the fact that the WorkStream class may be ill-suited to
// this operation (we could, in principle simply create a new task using
// Threads::new_task for each cell) but there is not much harm done to doing
// it this way anyway.
// Furthermore, should there be different material models associated with a
// quadrature point, requiring varying levels of computational expense, then
// the method used here could be advantageous.
template <int dim>
struct Solid<dim>::PerTaskData_UQPH
{
void reset()
{}
};
// The ScratchData object will be used to store an alias for the solution
// vector so that we don't have to copy this large data structure. We then
// define a number of vectors to extract the solution values and gradients at
// the quadrature points.
template <int dim>
struct Solid<dim>::ScratchData_UQPH
{
const BlockVector<double> &solution_total;
std::vector<Tensor<2, dim> > solution_grads_u_total;
FEValues<dim> fe_values_ref;
ScratchData_UQPH(const FiniteElement<dim> &fe_cell,
const QGauss<dim> &qf_cell,
const UpdateFlags uf_cell,
const BlockVector<double> &solution_total)
:
solution_total(solution_total),
solution_grads_u_total(qf_cell.size()),
fe_values_ref(fe_cell, qf_cell, uf_cell)
{}
ScratchData_UQPH(const ScratchData_UQPH &rhs)
:
solution_total(rhs.solution_total),
solution_grads_u_total(rhs.solution_grads_u_total),
fe_values_ref(rhs.fe_values_ref.get_fe(),
rhs.fe_values_ref.get_quadrature(),
rhs.fe_values_ref.get_update_flags())
{}
void reset()
{
const unsigned int n_q_points = solution_grads_u_total.size();
for (unsigned int q = 0; q < n_q_points; ++q)
{
solution_grads_u_total[q] = 0.0;
}
}
};
// @sect4{Solid::make_grid}
// On to the first of the private member functions. Here we create the
// triangulation of the domain, for which we choose the scaled cube with each
// face given a boundary ID number. The grid must be refined at least once
// for the indentation problem.
//
// We then determine the volume of the reference configuration and print it
// for comparison:
template <int dim>
void Solid<dim>::make_grid()
{
GridGenerator::hyper_rectangle(triangulation,
Point<dim>(0.0, 0.0, 0.0),
Point<dim>(1.0, 1.0, 1.0),
true);
GridTools::scale(parameters.scale, triangulation);
triangulation.refine_global(std::max (1U, parameters.global_refinement));
vol_reference = GridTools::volume(triangulation);
vol_current = vol_reference;
std::cout << "Grid:\n\t Reference volume: " << vol_reference << std::endl;
}
// @sect4{Solid::system_setup}
// Next we describe how the FE system is setup. We first determine the number
// of components per block. Since the displacement is a vector component, the
// first dim components belong to it, while the next two describe scalar
// pressure and dilatation DOFs.
template <int dim>
void Solid<dim>::system_setup()
{
timer.enter_subsection("Setup system");
std::vector<unsigned int> block_component(n_components, u_dof); // Displacement
// The DOF handler is then initialised and we renumber the grid in an
// efficient manner. We also record the number of DOFs per block.
dof_handler_ref.distribute_dofs(fe);
DoFRenumbering::Cuthill_McKee(dof_handler_ref);
DoFRenumbering::component_wise(dof_handler_ref, block_component);
DoFTools::count_dofs_per_block(dof_handler_ref, dofs_per_block,
block_component);
std::cout << "Triangulation:"
<< "\n\t Number of active cells: " << triangulation.n_active_cells()
<< "\n\t Number of degrees of freedom: " << dof_handler_ref.n_dofs()
<< std::endl;
// Setup the sparsity pattern and tangent matrix
tangent_matrix.clear();
{
const types::global_dof_index n_dofs_u = dofs_per_block[u_dof];
BlockDynamicSparsityPattern dsp(n_blocks, n_blocks);
dsp.block(u_dof, u_dof).reinit(n_dofs_u, n_dofs_u);
dsp.collect_sizes();
// The global system matrix initially has the following structure
// @f{align*}
// \underbrace{\begin{bmatrix}
// \mathbf{\mathsf{K}}_{uu} & \mathbf{\mathsf{K}}_{u\widetilde{p}} & \mathbf{0}
// \\ \mathbf{\mathsf{K}}_{\widetilde{p}u} & \mathbf{0} & \mathbf{\mathsf{K}}_{\widetilde{p}\widetilde{J}}
// \\ \mathbf{0} & \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}} & \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{J}}
// \end{bmatrix}}_{\mathbf{\mathsf{K}}(\mathbf{\Xi}_{\textrm{i}})}
// \underbrace{\begin{bmatrix}
// d \mathbf{\mathsf{u}}
// \\ d \widetilde{\mathbf{\mathsf{p}}}
// \\ d \widetilde{\mathbf{\mathsf{J}}}
// \end{bmatrix}}_{d \mathbf{\Xi}}
// =
// \underbrace{\begin{bmatrix}
// \mathbf{\mathsf{F}}_{u}(\mathbf{u}_{\textrm{i}})
// \\ \mathbf{\mathsf{F}}_{\widetilde{p}}(\widetilde{p}_{\textrm{i}})
// \\ \mathbf{\mathsf{F}}_{\widetilde{J}}(\widetilde{J}_{\textrm{i}})
//\end{bmatrix}}_{ \mathbf{\mathsf{F}}(\mathbf{\Xi}_{\textrm{i}}) } \, .
// @f}
// We optimise the sparsity pattern to reflect this structure
// and prevent unnecessary data creation for the right-diagonal
// block components.
Table<2, DoFTools::Coupling> coupling(n_components, n_components);
for (unsigned int ii = 0; ii < n_components; ++ii)
for (unsigned int jj = 0; jj < n_components; ++jj)
coupling[ii][jj] = DoFTools::always;
DoFTools::make_sparsity_pattern(dof_handler_ref,
coupling,
dsp,
constraints,
false);
sparsity_pattern.copy_from(dsp);
}
tangent_matrix.reinit(sparsity_pattern);
// We then set up storage vectors
system_rhs.reinit(dofs_per_block);
system_rhs.collect_sizes();
solution_n.reinit(dofs_per_block);
solution_n.collect_sizes();
// ...and finally set up the quadrature
// point history:
setup_qph();
timer.leave_subsection();
}
// @sect4{Solid::determine_component_extractors}
// Next we compute some information from the FE system that describes which local
// element DOFs are attached to which block component. This is used later to
// extract sub-blocks from the global matrix.
//
// In essence, all we need is for the FESystem object to indicate to which
// block component a DOF on the reference cell is attached to. Currently, the
// interpolation fields are setup such that 0 indicates a displacement DOF, 1
// a pressure DOF and 2 a dilatation DOF.
template <int dim>
void
Solid<dim>::determine_component_extractors()
{
element_indices_u.clear();
for (unsigned int k = 0; k < fe.dofs_per_cell; ++k)
{
const unsigned int k_group = fe.system_to_base_index(k).first.first;
if (k_group == u_dof)
element_indices_u.push_back(k);
else
{
Assert(k_group <= u_dof, ExcInternalError());
}
}
}
// @sect4{Solid::setup_qph}
// The method used to store quadrature information is already described in
// step-18. Here we implement a similar setup for a SMP machine.
//
// Firstly the actual QPH data objects are created. This must be done only
// once the grid is refined to its finest level.
template <int dim>
void Solid<dim>::setup_qph()
{
std::cout << " Setting up quadrature point data..." << std::endl;
{
triangulation.clear_user_data();
{
std::vector<PointHistory<dim> > tmp;
tmp.swap(quadrature_point_history);
}
quadrature_point_history
.resize(triangulation.n_active_cells() * n_q_points);
unsigned int history_index = 0;
for (typename Triangulation<dim>::active_cell_iterator cell =
triangulation.begin_active(); cell != triangulation.end();
++cell)
{
cell->set_user_pointer(&quadrature_point_history[history_index]);
history_index += n_q_points;
}
Assert(history_index == quadrature_point_history.size(),
ExcInternalError());
}
// Next we setup the initial quadrature
// point data:
for (typename Triangulation<dim>::active_cell_iterator cell =
triangulation.begin_active(); cell != triangulation.end(); ++cell)
{
PointHistory<dim> *lqph =
reinterpret_cast<PointHistory<dim>*>(cell->user_pointer());
Assert(lqph >= &quadrature_point_history.front(), ExcInternalError());
Assert(lqph <= &quadrature_point_history.back(), ExcInternalError());
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
lqph[q_point].setup_lqp(parameters);
}
}
// @sect4{Solid::update_qph_incremental}
// As the update of QP information occurs frequently and involves a number of
// expensive operations, we define a multithreaded approach to distributing
// the task across a number of CPU cores.
//
// To start this, we first we need to obtain the total solution as it stands
// at this Newton increment and then create the initial copy of the scratch and
// copy data objects:
template <int dim>
void Solid<dim>::update_qph_incremental(const BlockVector<double> &solution_delta)
{
timer.enter_subsection("Update QPH data");
std::cout << " UQPH " << std::flush;
const BlockVector<double> solution_total(get_total_solution(solution_delta));
const UpdateFlags uf_UQPH(update_gradients);
PerTaskData_UQPH per_task_data_UQPH;
ScratchData_UQPH scratch_data_UQPH(fe, qf_cell, uf_UQPH, solution_total);
// We then pass them and the one-cell update function to the WorkStream to
// be processed:
WorkStream::run(dof_handler_ref.begin_active(),
dof_handler_ref.end(),
*this,
&Solid::update_qph_incremental_one_cell,
&Solid::copy_local_to_global_UQPH,
scratch_data_UQPH,
per_task_data_UQPH);
timer.leave_subsection();
}
// Now we describe how we extract data from the solution vector and pass it
// along to each QP storage object for processing.
template <int dim>
void
Solid<dim>::update_qph_incremental_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_UQPH &scratch,
PerTaskData_UQPH &/*data*/)
{
PointHistory<dim> *lqph =
reinterpret_cast<PointHistory<dim>*>(cell->user_pointer());
Assert(lqph >= &quadrature_point_history.front(), ExcInternalError());
Assert(lqph <= &quadrature_point_history.back(), ExcInternalError());
Assert(scratch.solution_grads_u_total.size() == n_q_points,
ExcInternalError());
scratch.reset();
// We first need to find the values and gradients at quadrature points
// inside the current cell and then we update each local QP using the
// displacement gradient and total pressure and dilatation solution
// values:
scratch.fe_values_ref.reinit(cell);
scratch.fe_values_ref[u_fe].get_function_gradients(scratch.solution_total,
scratch.solution_grads_u_total);
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
lqph[q_point].update_values(scratch.solution_grads_u_total[q_point]);
}
// @sect4{Solid::solve_nonlinear_timestep}
// The next function is the driver method for the Newton-Raphson scheme. At
// its top we create a new vector to store the current Newton update step,
// reset the error storage objects and print solver header.
template <int dim>
void
Solid<dim>::solve_nonlinear_timestep(BlockVector<double> &solution_delta)
{
std::cout << std::endl << "Timestep " << time.get_timestep() << " @ "
<< time.current() << "s" << std::endl;
BlockVector<double> newton_update(dofs_per_block);
error_residual.reset();
error_residual_0.reset();
error_residual_norm.reset();
error_update.reset();
error_update_0.reset();
error_update_norm.reset();
print_conv_header();
// We now perform a number of Newton iterations to iteratively solve the
// nonlinear problem. Since the problem is fully nonlinear and we are
// using a full Newton method, the data stored in the tangent matrix and
// right-hand side vector is not reusable and must be cleared at each
// Newton step. We then initially build the right-hand side vector to
// check for convergence (and store this value in the first iteration).
// The unconstrained DOFs of the rhs vector hold the out-of-balance
// forces. The building is done before assembling the system matrix as the
// latter is an expensive operation and we can potentially avoid an extra
// assembly process by not assembling the tangent matrix when convergence
// is attained.
unsigned int newton_iteration = 0;
for (; newton_iteration < parameters.max_iterations_NR;
++newton_iteration)
{
std::cout << " " << std::setw(2) << newton_iteration << " " << std::flush;
tangent_matrix = 0.0;
system_rhs = 0.0;
assemble_system_rhs();
get_error_residual(error_residual);
if (newton_iteration == 0)
error_residual_0 = error_residual;
// We can now determine the normalised residual error and check for
// solution convergence:
error_residual_norm = error_residual;
error_residual_norm.normalise(error_residual_0);
if (newton_iteration > 0 && error_update_norm.u <= parameters.tol_u
&& error_residual_norm.u <= parameters.tol_f)
{
std::cout << " CONVERGED! " << std::endl;
print_conv_footer();
break;
}
// If we have decided that we want to continue with the iteration, we
// assemble the tangent, make and impose the Dirichlet constraints,
// and do the solve of the linearised system:
assemble_system_tangent();
make_constraints(newton_iteration);
constraints.condense(tangent_matrix, system_rhs);
const std::pair<unsigned int, double>
lin_solver_output = solve_linear_system(newton_update);
get_error_update(newton_update, error_update);
if (newton_iteration == 0)
error_update_0 = error_update;
// We can now determine the normalised Newton update error, and
// perform the actual update of the solution increment for the current
// time step, update all quadrature point information pertaining to
// this new displacement and stress state and continue iterating:
error_update_norm = error_update;
error_update_norm.normalise(error_update_0);
solution_delta += newton_update;
update_qph_incremental(solution_delta);
std::cout << " | " << std::fixed << std::setprecision(3) << std::setw(7)
<< std::scientific << lin_solver_output.first << " "
<< lin_solver_output.second << " " << error_residual_norm.norm
<< " " << error_residual_norm.u << " "
<< " " << error_update_norm.norm << " " << error_update_norm.u
<< " " << std::endl;
}
// At the end, if it turns out that we have in fact done more iterations
// than the parameter file allowed, we raise an exception that can be
// caught in the main() function. The call <code>AssertThrow(condition,
// exc_object)</code> is in essence equivalent to <code>if (!cond) throw
// exc_object;</code> but the former form fills certain fields in the
// exception object that identify the location (filename and line number)
// where the exception was raised to make it simpler to identify where the
// problem happened.
AssertThrow (newton_iteration <= parameters.max_iterations_NR,
ExcMessage("No convergence in nonlinear solver!"));
}
// @sect4{Solid::print_conv_header and Solid::print_conv_footer}
// This program prints out data in a nice table that is updated
// on a per-iteration basis. The next two functions set up the table
// header and footer:
template <int dim>
void Solid<dim>::print_conv_header()
{
static const unsigned int l_width = 102;
for (unsigned int i = 0; i < l_width; ++i)
std::cout << "_";
std::cout << std::endl;
std::cout << " SOLVER STEP "
<< " | LIN_IT LIN_RES RES_NORM "
<< " RES_U NU_NORM "
<< " NU_U " << std::endl;
for (unsigned int i = 0; i < l_width; ++i)
std::cout << "_";
std::cout << std::endl;
}
template <int dim>
void Solid<dim>::print_conv_footer()
{
static const unsigned int l_width = 102;
for (unsigned int i = 0; i < l_width; ++i)
std::cout << "_";
std::cout << std::endl;
std::cout << "Relative errors:" << std::endl
<< "Displacement:\t" << error_update.u / error_update_0.u << std::endl
<< "Force: \t\t" << error_residual.u / error_residual_0.u << std::endl
<< "v / V_0:\t" << vol_current << " / " << vol_reference
<< std::endl;
}
// @sect4{Solid::get_error_residual}
// Determine the true residual error for the problem. That is, determine the
// error in the residual for the unconstrained degrees of freedom. Note that to
// do so, we need to ignore constrained DOFs by setting the residual in these
// vector components to zero.
template <int dim>
void Solid<dim>::get_error_residual(Errors &error_residual)
{
BlockVector<double> error_res(dofs_per_block);
for (unsigned int i = 0; i < dof_handler_ref.n_dofs(); ++i)
if (!constraints.is_constrained(i))
error_res(i) = system_rhs(i);
error_residual.norm = error_res.l2_norm();
error_residual.u = error_res.block(u_dof).l2_norm();
}
// @sect4{Solid::get_error_udpate}
// Determine the true Newton update error for the problem
template <int dim>
void Solid<dim>::get_error_update(const BlockVector<double> &newton_update,
Errors &error_update)
{
BlockVector<double> error_ud(dofs_per_block);
for (unsigned int i = 0; i < dof_handler_ref.n_dofs(); ++i)
if (!constraints.is_constrained(i))
error_ud(i) = newton_update(i);
error_update.norm = error_ud.l2_norm();
error_update.u = error_ud.block(u_dof).l2_norm();
}
// @sect4{Solid::get_total_solution}
// This function provides the total solution, which is valid at any Newton step.
// This is required as, to reduce computational error, the total solution is
// only updated at the end of the timestep.
template <int dim>
BlockVector<double>
Solid<dim>::get_total_solution(const BlockVector<double> &solution_delta) const
{
BlockVector<double> solution_total(solution_n);
solution_total += solution_delta;
return solution_total;
}
// @sect4{Solid::assemble_system_tangent}
// Since we use TBB for assembly, we simply setup a copy of the
// data structures required for the process and pass them, along
// with the memory addresses of the assembly functions to the
// WorkStream object for processing. Note that we must ensure that
// the matrix is reset before any assembly operations can occur.
template <int dim>
void Solid<dim>::assemble_system_tangent()
{
timer.enter_subsection("Assemble tangent matrix");
std::cout << " ASM_K " << std::flush;
tangent_matrix = 0.0;
const UpdateFlags uf_cell(update_values |
update_gradients |
update_JxW_values);
PerTaskData_K per_task_data(dofs_per_cell);
ScratchData_K scratch_data(fe, qf_cell, uf_cell);
WorkStream::run(dof_handler_ref.begin_active(),
dof_handler_ref.end(),
*this,
&Solid::assemble_system_tangent_one_cell,
&Solid::copy_local_to_global_K,
scratch_data,
per_task_data);
timer.leave_subsection();
}
// This function adds the local contribution to the system matrix.
// Note that we choose not to use the constraint matrix to do the
// job for us because the tangent matrix and residual processes have
// been split up into two separate functions.
template <int dim>
void Solid<dim>::copy_local_to_global_K(const PerTaskData_K &data)
{
for (unsigned int i = 0; i < dofs_per_cell; ++i)
for (unsigned int j = 0; j < dofs_per_cell; ++j)
tangent_matrix.add(data.local_dof_indices[i],
data.local_dof_indices[j],
data.cell_matrix(i, j));
}
// Of course, we still have to define how we assemble the tangent matrix
// contribution for a single cell. We first need to reset and initialise some
// of the scratch data structures and retrieve some basic information
// regarding the DOF numbering on this cell. We can precalculate the cell
// shape function values and gradients. Note that the shape function gradients
// are defined with regard to the current configuration. That is
// $\textrm{grad}\ \boldsymbol{\varphi} = \textrm{Grad}\ \boldsymbol{\varphi}
// \ \mathbf{F}^{-1}$.
template <int dim>
void
Solid<dim>::assemble_system_tangent_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_K &scratch,
PerTaskData_K &data)
{
data.reset();
scratch.reset();
scratch.fe_values_ref.reinit(cell);
cell->get_dof_indices(data.local_dof_indices);
PointHistory<dim> *lqph =
reinterpret_cast<PointHistory<dim>*>(cell->user_pointer());
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
const Tensor<2, dim> F_inv = lqph[q_point].get_F_inv();
for (unsigned int k = 0; k < dofs_per_cell; ++k)
{
const unsigned int k_group = fe.system_to_base_index(k).first.first;
if (k_group == u_dof)
{
scratch.grad_Nx[q_point][k] = scratch.fe_values_ref[u_fe].gradient(k, q_point)
* F_inv;
scratch.symm_grad_Nx[q_point][k] = symmetrize(scratch.grad_Nx[q_point][k]);
}
else
Assert(k_group <= u_dof, ExcInternalError());
}
}
// Now we build the local cell stiffness matrix. Since the global and
// local system matrices are symmetric, we can exploit this property by
// building only the lower half of the local matrix and copying the values
// to the upper half. So we only assemble half of the
// $\mathsf{\mathbf{k}}_{uu}$, $\mathsf{\mathbf{k}}_{\widetilde{p}
// \widetilde{p}} = \mathbf{0}$, $\mathsf{\mathbf{k}}_{\widetilde{J}
// \widetilde{J}}$ blocks, while the whole
// $\mathsf{\mathbf{k}}_{\widetilde{p} \widetilde{J}}$,
// $\mathsf{\mathbf{k}}_{\mathbf{u} \widetilde{J}} = \mathbf{0}$,
// $\mathsf{\mathbf{k}}_{\mathbf{u} \widetilde{p}}$ blocks are built.
//
// In doing so, we first extract some configuration dependent variables
// from our QPH history objects for the current quadrature point.
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
const Tensor<2, dim> tau = lqph[q_point].get_tau();
const SymmetricTensor<4, dim> Jc = lqph[q_point].get_Jc();
const double det_F = lqph[q_point].get_det_F();
// Next we define some aliases to make the assembly process easier to
// follow
const std::vector<double>
&N = scratch.Nx[q_point];
const std::vector<SymmetricTensor<2, dim> >
&symm_grad_Nx = scratch.symm_grad_Nx[q_point];
const std::vector<Tensor<2, dim> >
&grad_Nx = scratch.grad_Nx[q_point];
const double JxW = scratch.fe_values_ref.JxW(q_point);
for (unsigned int i = 0; i < dofs_per_cell; ++i)
{
const unsigned int component_i = fe.system_to_component_index(i).first;
const unsigned int i_group = fe.system_to_base_index(i).first.first;
for (unsigned int j = 0; j <= i; ++j)
{
const unsigned int component_j = fe.system_to_component_index(j).first;
const unsigned int j_group = fe.system_to_base_index(j).first.first;
// This is the $\mathsf{\mathbf{k}}_{\mathbf{u} \mathbf{u}}$
// contribution. It comprises a material contribution, and a
// geometrical stress contribution which is only added along
// the local matrix diagonals:
if ((i_group == j_group) && (i_group == u_dof))
{
data.cell_matrix(i, j) += symm_grad_Nx[i] * Jc // The material contribution:
* symm_grad_Nx[j] * JxW;
if (component_i == component_j) // geometrical stress contribution
data.cell_matrix(i, j) += grad_Nx[i][component_i] * tau
* grad_Nx[j][component_j] * JxW;
}
else
Assert((i_group <= u_dof) && (j_group <= u_dof),
ExcInternalError());
}
}
}
// Finally, we need to copy the lower half of the local matrix into the
// upper half:
for (unsigned int i = 0; i < dofs_per_cell; ++i)
for (unsigned int j = i + 1; j < dofs_per_cell; ++j)
data.cell_matrix(i, j) = data.cell_matrix(j, i);
}
// @sect4{Solid::assemble_system_rhs}
// The assembly of the right-hand side process is similar to the
// tangent matrix, so we will not describe it in too much detail.
// Note that since we are describing a problem with Neumann BCs,
// we will need the face normals and so must specify this in the
// update flags.
template <int dim>
void Solid<dim>::assemble_system_rhs()
{
timer.enter_subsection("Assemble system right-hand side");
std::cout << " ASM_R " << std::flush;
system_rhs = 0.0;
const UpdateFlags uf_cell(update_values |
update_gradients |
update_JxW_values);
const UpdateFlags uf_face(update_values |
update_normal_vectors |
update_JxW_values);
PerTaskData_RHS per_task_data(dofs_per_cell);
ScratchData_RHS scratch_data(fe, qf_cell, uf_cell, qf_face, uf_face);
WorkStream::run(dof_handler_ref.begin_active(),
dof_handler_ref.end(),
*this,
&Solid::assemble_system_rhs_one_cell,
&Solid::copy_local_to_global_rhs,
scratch_data,
per_task_data);
timer.leave_subsection();
}
template <int dim>
void Solid<dim>::copy_local_to_global_rhs(const PerTaskData_RHS &data)
{
for (unsigned int i = 0; i < dofs_per_cell; ++i)
system_rhs(data.local_dof_indices[i]) += data.cell_rhs(i);
}
template <int dim>
double
Solid<dim>::get_pressure() const
{
static const double p0 = parameters.pressure
/
(parameters.scale * parameters.scale);
const double time_ramp = (time.current() / time.end());
const double pressure = p0 * time_ramp;
return pressure;
}
template <int dim>
void
Solid<dim>::assemble_system_rhs_one_cell(const typename DoFHandler<dim>::active_cell_iterator &cell,
ScratchData_RHS &scratch,
PerTaskData_RHS &data)
{
data.reset();
scratch.reset();
scratch.fe_values_ref.reinit(cell);
cell->get_dof_indices(data.local_dof_indices);
PointHistory<dim> *lqph =
reinterpret_cast<PointHistory<dim>*>(cell->user_pointer());
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
const Tensor<2, dim> F_inv = lqph[q_point].get_F_inv();
for (unsigned int k = 0; k < dofs_per_cell; ++k)
{
const unsigned int k_group = fe.system_to_base_index(k).first.first;
if (k_group == u_dof)
scratch.symm_grad_Nx[q_point][k]
= symmetrize(scratch.fe_values_ref[u_fe].gradient(k, q_point)
* F_inv);
else
Assert(k_group <= u_dof, ExcInternalError());
}
}
for (unsigned int q_point = 0; q_point < n_q_points; ++q_point)
{
const SymmetricTensor<2, dim> tau = lqph[q_point].get_tau();
const std::vector<double>
&N = scratch.Nx[q_point];
const std::vector<SymmetricTensor<2, dim> >
&symm_grad_Nx = scratch.symm_grad_Nx[q_point];
const double JxW = scratch.fe_values_ref.JxW(q_point);
// We first compute the contributions
// from the internal forces. Note, by
// definition of the rhs as the negative
// of the residual, these contributions
// are subtracted.
for (unsigned int i = 0; i < dofs_per_cell; ++i)
{
const unsigned int i_group = fe.system_to_base_index(i).first.first;
if (i_group == u_dof)
data.cell_rhs(i) -= (symm_grad_Nx[i] * tau) * JxW;
else
Assert(i_group <= u_dof, ExcInternalError());
}
}
// Next we assemble the Neumann contribution. We first check to see it the
// cell face exists on a boundary on which a traction is applied and add
// the contribution if this is the case.
for (unsigned int face = 0; face < GeometryInfo<dim>::faces_per_cell;
++face)
if (cell->face(face)->at_boundary() == true
&& cell->face(face)->boundary_id() == 5)
{
scratch.fe_face_values_ref.reinit(cell, face);
for (unsigned int f_q_point = 0; f_q_point < n_q_points_f;
++f_q_point)
{
const Tensor<1, dim> &N =
scratch.fe_face_values_ref.normal_vector(f_q_point);
// Using the face normal at this quadrature point we specify the
// traction in reference configuration. For this problem, a
// defined pressure is applied in the reference configuration.
// The direction of the applied traction is assumed not to
// evolve with the deformation of the domain. The traction is
// defined using the first Piola-Kirchhoff stress is simply
// $\mathbf{t} = \mathbf{P}\mathbf{N} = [p_0 \mathbf{I}]
// \mathbf{N} = p_0 \mathbf{N}$ We use the time variable to
// linearly ramp up the pressure load.
//
// Note that the contributions to the right hand side vector we
// compute here only exist in the displacement components of the
// vector.
const double pressure = get_pressure();
const Tensor<1, dim> traction = pressure * N;
for (unsigned int i = 0; i < dofs_per_cell; ++i)
{
const unsigned int i_group =
fe.system_to_base_index(i).first.first;
if (i_group == u_dof)
{
const unsigned int component_i =
fe.system_to_component_index(i).first;
const double Ni =
scratch.fe_face_values_ref.shape_value(i,
f_q_point);
const double JxW = scratch.fe_face_values_ref.JxW(
f_q_point);
data.cell_rhs(i) += (Ni * traction[component_i])
* JxW;
}
}
}
}
}
// @sect4{Solid::make_constraints}
// The constraints for this problem are simple to describe.
// However, since we are dealing with an iterative Newton method,
// it should be noted that any displacement constraints should only
// be specified at the zeroth iteration and subsequently no
// additional contributions are to be made since the constraints
// are already exactly satisfied.
template <int dim>
void Solid<dim>::make_constraints(const int &it_nr)
{
std::cout << " CST " << std::flush;
// Since the constraints are different at different Newton iterations, we
// need to clear the constraints matrix and completely rebuild
// it. However, after the first iteration, the constraints remain the same
// and we can simply skip the rebuilding step if we do not clear it.
if (it_nr > 1)
return;
constraints.clear();
const bool apply_dirichlet_bc = (it_nr == 0);
// The boundary conditions for the indentation problem are as follows: On
// the -x, -y and -z faces (ID's 0,2,4) we set up a symmetry condition to
// allow only planar movement while the +x and +y faces (ID's 1,3) are
// traction free. In this contrived problem, part of the +z face (ID 5) is
// set to have no motion in the x- and y-component. Finally, as described
// earlier, the other part of the +z face has an the applied pressure but
// is also constrained in the x- and y-directions.
//
// In the following, we will have to tell the function interpolation
// boundary values which components of the solution vector should be
// constrained (i.e., whether it's the x-, y-, z-displacements or
// combinations thereof). This is done using ComponentMask objects (see
// @ref GlossComponentMask) which we can get from the finite element if we
// provide it with an extractor object for the component we wish to
// select. To this end we first set up such extractor objects and later
// use it when generating the relevant component masks:
const FEValuesExtractors::Scalar x_displacement(0);
const FEValuesExtractors::Scalar y_displacement(1);
const FEValuesExtractors::Scalar z_displacement(2);
{
const int boundary_id = 0;
if (apply_dirichlet_bc == true)
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(x_displacement));
else
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(x_displacement));
}
{
const int boundary_id = 2;
if (apply_dirichlet_bc == true)
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(y_displacement));
else
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(y_displacement));
}
{
const int boundary_id = 4;
if (apply_dirichlet_bc == true)
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(z_displacement));
else
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
fe.component_mask(z_displacement));
}
// {
// const int boundary_id = 5;
//
// if (apply_dirichlet_bc == true)
// VectorTools::interpolate_boundary_values(dof_handler_ref,
// boundary_id,
// ZeroFunction<dim>(n_components),
// constraints,
// (fe.component_mask(x_displacement)
// |
// fe.component_mask(y_displacement)));
// else
// VectorTools::interpolate_boundary_values(dof_handler_ref,
// boundary_id,
// ZeroFunction<dim>(n_components),
// constraints,
// (fe.component_mask(x_displacement)
// |
// fe.component_mask(y_displacement)));
// }
{
const int boundary_id = 6;
if (apply_dirichlet_bc == true)
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
(fe.component_mask(x_displacement)
|
fe.component_mask(y_displacement)));
else
VectorTools::interpolate_boundary_values(dof_handler_ref,
boundary_id,
ZeroFunction<dim>(n_components),
constraints,
(fe.component_mask(x_displacement)
|
fe.component_mask(y_displacement)));
}
constraints.close();
}
// @sect4{Solid::solve_linear_system}
// Solving the entire block system is a bit problematic as there are no
// contributions to the $\mathsf{\mathbf{k}}_{ \widetilde{J} \widetilde{J}}$
// block, rendering it noninvertible.
// Since the pressure and dilatation variables DOFs are discontinuous, we can
// condense them out to form a smaller displacement-only system which
// we will then solve and subsequently post-process to retrieve the
// pressure and dilatation solutions.
//
// At the top, we allocate two temporary vectors to help with the static
// condensation, and variables to store the number of linear solver iterations
// and the (hopefully converged) residual.
//
// For the following, recall that
// @f{align*}
// \mathbf{\mathsf{K}}_{\textrm{store}}
//:=
// \begin{bmatrix}
// \mathbf{\mathsf{K}}_{\textrm{con}} & \mathbf{\mathsf{K}}_{u\widetilde{p}} & \mathbf{0}
// \\ \mathbf{\mathsf{K}}_{\widetilde{p}u} & \mathbf{0} & \mathbf{\mathsf{K}}_{\widetilde{p}\widetilde{J}}^{-1}
// \\ \mathbf{0} & \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}} & \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{J}}
// \end{bmatrix} \, .
// @f}
// and
// @f{align*}
// d \widetilde{\mathbf{\mathsf{p}}}
// & = \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}}^{-1} \bigl[
// \mathbf{\mathsf{F}}_{\widetilde{J}}
// - \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{J}} d \widetilde{\mathbf{\mathsf{J}}} \bigr]
// \\ d \widetilde{\mathbf{\mathsf{J}}}
// & = \mathbf{\mathsf{K}}_{\widetilde{p}\widetilde{J}}^{-1} \bigl[
// \mathbf{\mathsf{F}}_{\widetilde{p}}
// - \mathbf{\mathsf{K}}_{\widetilde{p}u} d \mathbf{\mathsf{u}}
// \bigr]
// \\ \Rightarrow d \widetilde{\mathbf{\mathsf{p}}}
// &= \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}}^{-1} \mathbf{\mathsf{F}}_{\widetilde{J}}
// - \underbrace{\bigl[\mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}}^{-1} \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{J}}
// \mathbf{\mathsf{K}}_{\widetilde{p}\widetilde{J}}^{-1}\bigr]}_{\overline{\mathbf{\mathsf{K}}}}\bigl[ \mathbf{\mathsf{F}}_{\widetilde{p}}
// - \mathbf{\mathsf{K}}_{\widetilde{p}u} d \mathbf{\mathsf{u}} \bigr]
// @f}
// and thus
// @f[
// \underbrace{\bigl[ \mathbf{\mathsf{K}}_{uu} + \overline{\overline{\mathbf{\mathsf{K}}}}~ \bigr]
// }_{\mathbf{\mathsf{K}}_{\textrm{con}}} d \mathbf{\mathsf{u}}
// =
// \underbrace{
// \Bigl[
// \mathbf{\mathsf{F}}_{u}
// - \mathbf{\mathsf{K}}_{u\widetilde{p}} \bigl[ \mathbf{\mathsf{K}}_{\widetilde{J}\widetilde{p}}^{-1} \mathbf{\mathsf{F}}_{\widetilde{J}}
// - \overline{\mathbf{\mathsf{K}}}\mathbf{\mathsf{F}}_{\widetilde{p}} \bigr]
// \Bigr]}_{\mathbf{\mathsf{F}}_{\textrm{con}}}
// @f]
// where
// @f[
// \overline{\overline{\mathbf{\mathsf{K}}}} :=
// \mathbf{\mathsf{K}}_{u\widetilde{p}} \overline{\mathbf{\mathsf{K}}} \mathbf{\mathsf{K}}_{\widetilde{p}u} \, .
// @f]
template <int dim>
std::pair<unsigned int, double>
Solid<dim>::solve_linear_system(BlockVector<double> &newton_update)
{
BlockVector<double> A(dofs_per_block);
BlockVector<double> B(dofs_per_block);
unsigned int lin_it = 0;
double lin_res = 0.0;
// In the first step of this function, we solve for the incremental
// displacement $d\mathbf{u}$. To this end, we perform static
// condensation to make
// $\mathbf{\mathsf{K}}_{\textrm{con}}
// = \bigl[ \mathbf{\mathsf{K}}_{uu} + \overline{\overline{\mathbf{\mathsf{K}}}}~ \bigr]$
// and put
// $\mathsf{\mathbf{k}}^{-1}_{\widetilde{p} \widetilde{J}}$
// in the original $\mathsf{\mathbf{k}}_{\widetilde{p} \widetilde{J}}$ block.
// That is, we make $\mathbf{\mathsf{K}}_{\textrm{store}}$.
{
timer.enter_subsection("Linear solver");
std::cout << " SLV " << std::flush;
if (parameters.type_lin == "CG")
{
const int solver_its = tangent_matrix.block(u_dof, u_dof).m()
* parameters.max_iterations_lin;
const double tol_sol = parameters.tol_lin
* system_rhs.block(u_dof).l2_norm();
SolverControl solver_control(solver_its, tol_sol);
GrowingVectorMemory<Vector<double> > GVM;
SolverCG<Vector<double> > solver_CG(solver_control, GVM);
// We've chosen by default a SSOR preconditioner as it appears to
// provide the fastest solver convergence characteristics for this
// problem on a single-thread machine. However, for multicore
// computing, the Jacobi preconditioner which is multithreaded may
// converge quicker for larger linear systems.
PreconditionSelector<SparseMatrix<double>, Vector<double> >
preconditioner (parameters.preconditioner_type,
parameters.preconditioner_relaxation);
preconditioner.use_matrix(tangent_matrix.block(u_dof, u_dof));
solver_CG.solve(tangent_matrix.block(u_dof, u_dof),
newton_update.block(u_dof),
system_rhs.block(u_dof),
preconditioner);
lin_it = solver_control.last_step();
lin_res = solver_control.last_value();
}
else if (parameters.type_lin == "Direct")
{
// Otherwise if the problem is small
// enough, a direct solver can be
// utilised.
SparseDirectUMFPACK A_direct;
A_direct.initialize(tangent_matrix.block(u_dof, u_dof));
A_direct.vmult(newton_update.block(u_dof), system_rhs.block(u_dof));
lin_it = 1;
lin_res = 0.0;
}
else
Assert (false, ExcMessage("Linear solver type not implemented"));
timer.leave_subsection();
}
// Now that we have the displacement update, distribute the constraints
// back to the Newton update:
constraints.distribute(newton_update);
return std::make_pair(lin_it, lin_res);
}
// @sect4{Solid::output_results}
// Here we present how the results are written to file to be viewed
// using ParaView or Visit. The method is similar to that shown in previous
// tutorials so will not be discussed in detail.
template <int dim>
void Solid<dim>::output_results() const
{
DataOut<dim> data_out;
std::vector<DataComponentInterpretation::DataComponentInterpretation>
data_component_interpretation(dim,
DataComponentInterpretation::component_is_part_of_vector);
std::vector<std::string> solution_name(dim, "displacement");
data_out.attach_dof_handler(dof_handler_ref);
data_out.add_data_vector(solution_n,
solution_name,
DataOut<dim>::type_dof_data,
data_component_interpretation);
// Compute reaction forces
const double face_area_ref = (1.0*parameters.scale)*(1.0*parameters.scale);
const double pressure = get_pressure();
const double force_expected = pressure*face_area_ref;
double force_face_integral_bid_5 = 0.0;
BlockVector<double> reaction_forces_bid_4;
reaction_forces_bid_4.reinit(solution_n,false);
{
FEFaceValues<dim> fe_face_values_ref (fe, qf_face,
update_values | update_gradients |
update_JxW_values | update_normal_vectors);
std::vector<Tensor<2, dim> > solution_grads_u_total (qf_face.size());
// Stress computation assistant
PointHistory<dim> rf_ph;
rf_ph.setup_lqp(parameters);
// Time to assemble the reaction force vector
for (typename DoFHandler<dim>::active_cell_iterator cell =
dof_handler_ref.begin_active(); cell != dof_handler_ref.end();
++cell)
{
Vector<double> cell_rf(dofs_per_cell);
std::vector<types::global_dof_index> local_dof_indices(dofs_per_cell);
cell->get_dof_indices(local_dof_indices);
for (unsigned int face = 0; face < GeometryInfo<dim>::faces_per_cell;
++face)
if (cell->face(face)->at_boundary() == true
&& cell->face(face)->boundary_id() == 4) // -Z face
{
fe_face_values_ref.reinit(cell, face);
fe_face_values_ref[u_fe].get_function_gradients(solution_n,
solution_grads_u_total);
for (unsigned int f_q_point = 0; f_q_point < n_q_points_f;
++f_q_point)
{
rf_ph.update_values(solution_grads_u_total[f_q_point]);
const Tensor<2,dim> F = solution_grads_u_total[f_q_point]
+ static_cast< Tensor<2,dim> >(StandardTensors<dim>::I);
const Tensor<1, dim> &N =
fe_face_values_ref.normal_vector(f_q_point);
const double JxW = fe_face_values_ref.JxW(f_q_point);
const double pressure = get_pressure();
const SymmetricTensor<2,dim> tau = rf_ph.get_tau(); // J.sigma = P.F^{T}
const Tensor<2,dim> FPKST = static_cast< Tensor<2,dim> >(tau)*invert(transpose(F));
const Tensor<1, dim> reaction_traction = FPKST*N; // P.N.JxW = sigma.n.jxW
// Since this surface and that to which we applied the pressure
// have the same geometry, we can do a quick sanity check
// for our calculation.
// NOTE: This must be adapted if the pressure is applied in the
// current configuration.
// Note: This little bit won't work if the geometry of the surface
// is not planar
force_face_integral_bid_5 += pressure * JxW;
for (unsigned int i = 0; i < dofs_per_cell; ++i)
{
const unsigned int i_group =
fe.system_to_base_index(i).first.first;
if (i_group == u_dof)
{
const unsigned int component_i =
fe.system_to_component_index(i).first;
const double Ni =
fe_face_values_ref.shape_value(i,f_q_point);
// Produce "nodal" representation of force vector
// Note: traction * JxW --> force
cell_rf(i) += (Ni * reaction_traction[component_i]) * JxW;
}
}
}
for (unsigned int i = 0; i < dofs_per_cell; ++i)
reaction_forces_bid_4(local_dof_indices[i]) += cell_rf(i);
}
}
// Note that the reaction forces computed at the face support points
// now only need to be summed together since they're the nodal
// representation of the surface forces
// Since I can't think of a more simple way to RELIABLY determine the
// component index of a global DoF (in general, there might be some
// global reordering to that they are not {[x,y,z]_1, [x,y,z]_2} etc),
// I'm just going to extract the local components through a cell loop
Tensor<1,dim> force_reaction_bid_4;
std::set<types::global_dof_index> touched_dofs;
for (typename DoFHandler<dim>::active_cell_iterator cell =
dof_handler_ref.begin_active(); cell != dof_handler_ref.end();
++cell)
{
std::vector<types::global_dof_index> local_dof_indices(dofs_per_cell);
cell->get_dof_indices(local_dof_indices);
// Technically not required because of the lack of non-zero entries
// in the vector, but I suppose this is the most correct approach
for (unsigned int face = 0; face < GeometryInfo<dim>::faces_per_cell; ++face)
if (cell->face(face)->at_boundary() == true
&& cell->face(face)->boundary_id() == 4) // -Z face
{
for (unsigned int i = 0; i < dofs_per_cell; ++i)
{
// Don't sum a DoF that we've visited more than once
if (touched_dofs.find(local_dof_indices[i]) != touched_dofs.end())
continue;
const unsigned int i_group =
fe.system_to_base_index(i).first.first;
if (i_group == u_dof)
{
const unsigned int component_i =
fe.system_to_component_index(i).first;
force_reaction_bid_4[component_i] += reaction_forces_bid_4[local_dof_indices[i]];
touched_dofs.insert(local_dof_indices[i]); // Mark as visited
}
}
}
}
std::cout
<< "force_expected: " << force_expected
<< " force_face_integral_bid_5: " << force_face_integral_bid_5
<< " force_reaction_bid_4(z): " << force_reaction_bid_4[2]
<< " forces cancel: " << (force_face_integral_bid_5+force_reaction_bid_4[2] < 1e-6 ? "yes :-)" : "NO!!!")
<< std::endl
<< "force_reaction_bid_4(x): " << force_reaction_bid_4[0]
<< " force_reaction_bid_4(y): " << force_reaction_bid_4[1]
<< std::endl;
}
std::vector<std::string> reaction_force_name(dim, "reaction_forces_bid_4");
data_out.add_data_vector(reaction_forces_bid_4,
reaction_force_name,
DataOut<dim>::type_dof_data,
data_component_interpretation);
// Since we are dealing with a large deformation problem, it would be nice
// to display the result on a displaced grid! The MappingQEulerian class
// linked with the DataOut class provides an interface through which this
// can be achieved without physically moving the grid points in the
// Triangulation object ourselves. We first need to copy the solution to
// a temporary vector and then create the Eulerian mapping. We also
// specify the polynomial degree to the DataOut object in order to produce
// a more refined output data set when higher order polynomials are used.
Vector<double> soln(solution_n.size());
for (unsigned int i = 0; i < soln.size(); ++i)
soln(i) = solution_n(i);
MappingQEulerian<dim> q_mapping(degree, soln, dof_handler_ref);
data_out.build_patches(q_mapping, degree);
std::ostringstream filename;
filename << "solution-" << time.get_timestep() << ".vtk";
std::ofstream output(filename.str().c_str());
data_out.write_vtk(output);
}
}
// @sect3{Main function}
// Lastly we provide the main driver function which appears
// no different to the other tutorials.
int main (int argc, char *argv[])
{
using namespace dealii;
using namespace Step44;
Utilities::MPI::MPI_InitFinalize mpi_initialization(argc, argv, dealii::numbers::invalid_unsigned_int);
try
{
deallog.depth_console(0);
Solid<3> solid_3d("parameters.prm");
solid_3d.run();
}
catch (std::exception &exc)
{
std::cerr << std::endl << std::endl
<< "----------------------------------------------------"
<< std::endl;
std::cerr << "Exception on processing: " << std::endl << exc.what()
<< std::endl << "Aborting!" << std::endl
<< "----------------------------------------------------"
<< std::endl;
return 1;
}
catch (...)
{
std::cerr << std::endl << std::endl
<< "----------------------------------------------------"
<< std::endl;
std::cerr << "Unknown exception!" << std::endl << "Aborting!"
<< std::endl
<< "----------------------------------------------------"
<< std::endl;
return 1;
}
return 0;
}
