Permalink
Fetching contributors…
Cannot retrieve contributors at this time
261 lines (235 sloc) 9.57 KB
// MFEM Example 2
//
// Compile with: make ex2
//
// Sample runs: ex2 -m ../data/beam-tri.mesh
// ex2 -m ../data/beam-quad.mesh
// ex2 -m ../data/beam-tet.mesh
// ex2 -m ../data/beam-hex.mesh
// ex2 -m ../data/beam-quad.mesh -o 3 -sc
// ex2 -m ../data/beam-quad-nurbs.mesh
// ex2 -m ../data/beam-hex-nurbs.mesh
//
// Description: This example code solves a simple linear elasticity problem
// describing a multi-material cantilever beam.
//
// Specifically, we approximate the weak form of -div(sigma(u))=0
// where sigma(u)=lambda*div(u)*I+mu*(grad*u+u*grad) is the stress
// tensor corresponding to displacement field u, and lambda and mu
// are the material Lame constants. The boundary conditions are
// u=0 on the fixed part of the boundary with attribute 1, and
// sigma(u).n=f on the remainder with f being a constant pull down
// vector on boundary elements with attribute 2, and zero
// otherwise. The geometry of the domain is assumed to be as
// follows:
//
// +----------+----------+
// boundary --->| material | material |<--- boundary
// attribute 1 | 1 | 2 | attribute 2
// (fixed) +----------+----------+ (pull down)
//
// The example demonstrates the use of high-order and NURBS vector
// finite element spaces with the linear elasticity bilinear form,
// meshes with curved elements, and the definition of piece-wise
// constant and vector coefficient objects. Static condensation is
// also illustrated.
//
// We recommend viewing Example 1 before viewing this example.
#include "mfem.hpp"
#include <fstream>
#include <iostream>
using namespace std;
using namespace mfem;
int main(int argc, char *argv[])
{
// 1. Parse command-line options.
const char *mesh_file = "../data/beam-tri.mesh";
int order = 1;
bool static_cond = false;
bool visualization = 1;
OptionsParser args(argc, argv);
args.AddOption(&mesh_file, "-m", "--mesh",
"Mesh file to use.");
args.AddOption(&order, "-o", "--order",
"Finite element order (polynomial degree).");
args.AddOption(&static_cond, "-sc", "--static-condensation", "-no-sc",
"--no-static-condensation", "Enable static condensation.");
args.AddOption(&visualization, "-vis", "--visualization", "-no-vis",
"--no-visualization",
"Enable or disable GLVis visualization.");
args.Parse();
if (!args.Good())
{
args.PrintUsage(cout);
return 1;
}
args.PrintOptions(cout);
// 2. Read the mesh from the given mesh file. We can handle triangular,
// quadrilateral, tetrahedral or hexahedral elements with the same code.
Mesh *mesh = new Mesh(mesh_file, 1, 1);
int dim = mesh->Dimension();
if (mesh->attributes.Max() < 2 || mesh->bdr_attributes.Max() < 2)
{
cerr << "\nInput mesh should have at least two materials and "
<< "two boundary attributes! (See schematic in ex2.cpp)\n"
<< endl;
return 3;
}
// 3. Select the order of the finite element discretization space. For NURBS
// meshes, we increase the order by degree elevation.
if (mesh->NURBSext)
{
mesh->DegreeElevate(order, order);
}
// 4. Refine the mesh to increase the resolution. In this example we do
// 'ref_levels' of uniform refinement. We choose 'ref_levels' to be the
// largest number that gives a final mesh with no more than 5,000
// elements.
{
int ref_levels =
(int)floor(log(5000./mesh->GetNE())/log(2.)/dim);
for (int l = 0; l < ref_levels; l++)
{
mesh->UniformRefinement();
}
}
// 5. Define a finite element space on the mesh. Here we use vector finite
// elements, i.e. dim copies of a scalar finite element space. The vector
// dimension is specified by the last argument of the FiniteElementSpace
// constructor. For NURBS meshes, we use the (degree elevated) NURBS space
// associated with the mesh nodes.
FiniteElementCollection *fec;
FiniteElementSpace *fespace;
if (mesh->NURBSext)
{
fec = NULL;
fespace = mesh->GetNodes()->FESpace();
}
else
{
fec = new H1_FECollection(order, dim);
fespace = new FiniteElementSpace(mesh, fec, dim);
}
cout << "Number of finite element unknowns: " << fespace->GetTrueVSize()
<< endl << "Assembling: " << flush;
// 6. Determine the list of true (i.e. conforming) essential boundary dofs.
// In this example, the boundary conditions are defined by marking only
// boundary attribute 1 from the mesh as essential and converting it to a
// list of true dofs.
Array<int> ess_tdof_list, ess_bdr(mesh->bdr_attributes.Max());
ess_bdr = 0;
ess_bdr[0] = 1;
fespace->GetEssentialTrueDofs(ess_bdr, ess_tdof_list);
// 7. Set up the linear form b(.) which corresponds to the right-hand side of
// the FEM linear system. In this case, b_i equals the boundary integral
// of f*phi_i where f represents a "pull down" force on the Neumann part
// of the boundary and phi_i are the basis functions in the finite element
// fespace. The force is defined by the VectorArrayCoefficient object f,
// which is a vector of Coefficient objects. The fact that f is non-zero
// on boundary attribute 2 is indicated by the use of piece-wise constants
// coefficient for its last component.
VectorArrayCoefficient f(dim);
for (int i = 0; i < dim-1; i++)
{
f.Set(i, new ConstantCoefficient(0.0));
}
{
Vector pull_force(mesh->bdr_attributes.Max());
pull_force = 0.0;
pull_force(1) = -1.0e-2;
f.Set(dim-1, new PWConstCoefficient(pull_force));
}
LinearForm *b = new LinearForm(fespace);
b->AddBoundaryIntegrator(new VectorBoundaryLFIntegrator(f));
cout << "r.h.s. ... " << flush;
b->Assemble();
// 8. Define the solution vector x as a finite element grid function
// corresponding to fespace. Initialize x with initial guess of zero,
// which satisfies the boundary conditions.
GridFunction x(fespace);
x = 0.0;
// 9. Set up the bilinear form a(.,.) on the finite element space
// corresponding to the linear elasticity integrator with piece-wise
// constants coefficient lambda and mu.
Vector lambda(mesh->attributes.Max());
lambda = 1.0;
lambda(0) = lambda(1)*50;
PWConstCoefficient lambda_func(lambda);
Vector mu(mesh->attributes.Max());
mu = 1.0;
mu(0) = mu(1)*50;
PWConstCoefficient mu_func(mu);
BilinearForm *a = new BilinearForm(fespace);
a->AddDomainIntegrator(new ElasticityIntegrator(lambda_func,mu_func));
// 10. Assemble the bilinear form and the corresponding linear system,
// applying any necessary transformations such as: eliminating boundary
// conditions, applying conforming constraints for non-conforming AMR,
// static condensation, etc.
cout << "matrix ... " << flush;
if (static_cond) { a->EnableStaticCondensation(); }
a->Assemble();
SparseMatrix A;
Vector B, X;
a->FormLinearSystem(ess_tdof_list, x, *b, A, X, B);
cout << "done." << endl;
cout << "Size of linear system: " << A.Height() << endl;
#ifndef MFEM_USE_SUITESPARSE
// 11. Define a simple symmetric Gauss-Seidel preconditioner and use it to
// solve the system Ax=b with PCG.
GSSmoother M(A);
PCG(A, M, B, X, 1, 500, 1e-8, 0.0);
#else
// 11. If MFEM was compiled with SuiteSparse, use UMFPACK to solve the system.
UMFPackSolver umf_solver;
umf_solver.Control[UMFPACK_ORDERING] = UMFPACK_ORDERING_METIS;
umf_solver.SetOperator(A);
umf_solver.Mult(B, X);
#endif
// 12. Recover the solution as a finite element grid function.
a->RecoverFEMSolution(X, *b, x);
// 13. For non-NURBS meshes, make the mesh curved based on the finite element
// space. This means that we define the mesh elements through a fespace
// based transformation of the reference element. This allows us to save
// the displaced mesh as a curved mesh when using high-order finite
// element displacement field. We assume that the initial mesh (read from
// the file) is not higher order curved mesh compared to the chosen FE
// space.
if (!mesh->NURBSext)
{
mesh->SetNodalFESpace(fespace);
}
// 14. Save the displaced mesh and the inverted solution (which gives the
// backward displacements to the original grid). This output can be
// viewed later using GLVis: "glvis -m displaced.mesh -g sol.gf".
{
GridFunction *nodes = mesh->GetNodes();
*nodes += x;
x *= -1;
ofstream mesh_ofs("displaced.mesh");
mesh_ofs.precision(8);
mesh->Print(mesh_ofs);
ofstream sol_ofs("sol.gf");
sol_ofs.precision(8);
x.Save(sol_ofs);
}
// 15. Send the above data by socket to a GLVis server. Use the "n" and "b"
// keys in GLVis to visualize the displacements.
if (visualization)
{
char vishost[] = "localhost";
int visport = 19916;
socketstream sol_sock(vishost, visport);
sol_sock.precision(8);
sol_sock << "solution\n" << *mesh << x << flush;
}
// 16. Free the used memory.
delete a;
delete b;
if (fec)
{
delete fespace;
delete fec;
}
delete mesh;
return 0;
}