Skip to content
Permalink
Branch: master
Find file Copy path
Find file Copy path
Fetching contributors…
Cannot retrieve contributors at this time
367 lines (328 sloc) 13.5 KB
// MFEM Example 21
//
// Compile with: make ex21p
//
// Sample runs: mpirun -np 4 ex21p
// mpirun -np 4 ex21p -o 3
// mpirun -np 4 ex21p -m ../data/beam-quad.mesh
// mpirun -np 4 ex21p -m ../data/beam-quad.mesh -o 3
// mpirun -np 4 ex21p -m ../data/beam-tet.mesh
// mpirun -np 4 ex21p -m ../data/beam-tet.mesh -o 2
// mpirun -np 4 ex21p -m ../data/beam-hex.mesh
// mpirun -np 4 ex21p -m ../data/beam-hex.mesh -o 2
//
// Description: This is a version of Example 2p with a simple adaptive mesh
// refinement loop. The problem being solved is again the linear
// elasticity describing a multi-material cantilever beam.
// The problem is solved on a sequence of meshes which
// are locally refined in a conforming (triangles, tetrahedrons)
// or non-conforming (quadrilaterals, hexahedra) manner according
// to a simple ZZ error estimator.
//
// The example demonstrates MFEM's capability to work with both
// conforming and nonconforming refinements, in 2D and 3D, on
// linear and curved meshes. Interpolation of functions from
// coarse to fine meshes, as well as persistent GLVis
// visualization are also illustrated.
//
// We recommend viewing Examples 2p and 6p before viewing this
// example.
#include "mfem.hpp"
#include <fstream>
#include <iostream>
using namespace std;
using namespace mfem;
int main(int argc, char *argv[])
{
// 0. Initialize MPI.
int num_procs, myid;
MPI_Init(&argc, &argv);
MPI_Comm_size(MPI_COMM_WORLD, &num_procs);
MPI_Comm_rank(MPI_COMM_WORLD, &myid);
// 1. Parse command-line options.
const char *mesh_file = "../data/beam-tri.mesh";
int serial_ref_levels = 0;
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(&serial_ref_levels, "-rs", "--refine-serial",
"Number of uniform serial refinements (before parallel"
" partitioning)");
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())
{
if (myid == 0)
{
args.PrintUsage(cout);
}
MPI_Finalize();
return 1;
}
if (myid == 0)
{
args.PrintOptions(cout);
}
// 2. Read the mesh from the given mesh file. We can handle triangular,
// quadrilateral, tetrahedral, and hexahedral meshes with the same code.
Mesh mesh(mesh_file, 1, 1);
int dim = mesh.Dimension();
MFEM_VERIFY(mesh.SpaceDimension() == dim, "invalid mesh");
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;
MPI_Finalize();
return 3;
}
// 3. Refine the mesh before parallel partitioning. Since a NURBS mesh can
// currently only be refined uniformly, we need to convert it to a
// piecewise-polynomial curved mesh. First we refine the NURBS mesh a bit
// more and then project the curvature to quadratic Nodes.
if (mesh.NURBSext && serial_ref_levels == 0)
{
serial_ref_levels = 2;
}
for (int i = 0; i < serial_ref_levels; i++)
{
mesh.UniformRefinement();
}
if (mesh.NURBSext)
{
mesh.SetCurvature(2);
}
mesh.EnsureNCMesh();
ParMesh pmesh(MPI_COMM_WORLD, mesh);
mesh.Clear();
// 4. Define a finite element space on the mesh. The polynomial order is
// one (linear) by default, but this can be changed on the command line.
H1_FECollection fec(order, dim);
ParFiniteElementSpace fespace(&pmesh, &fec, dim);
// 5. As in Example 2, we 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. We don't assemble the discrete problem yet, this will be
// done in the main loop.
VectorArrayCoefficient f(dim);
for (int i = 0; i < dim-1; i++)
{
f.Set(i, new ConstantCoefficient(0.0));
}
{
Vector pull_force(pmesh.bdr_attributes.Max());
pull_force = 0.0;
pull_force(1) = -1.0e-2;
f.Set(dim-1, new PWConstCoefficient(pull_force));
}
ParLinearForm b(&fespace);
b.AddDomainIntegrator(new VectorBoundaryLFIntegrator(f));
// 6. 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(pmesh.attributes.Max());
lambda = 1.0;
lambda(0) = lambda(1)*50;
PWConstCoefficient lambda_func(lambda);
Vector mu(pmesh.attributes.Max());
mu = 1.0;
mu(0) = mu(1)*50;
PWConstCoefficient mu_func(mu);
ParBilinearForm a(&fespace);
BilinearFormIntegrator *integ =
new ElasticityIntegrator(lambda_func,mu_func);
a.AddDomainIntegrator(integ);
if (static_cond) { a.EnableStaticCondensation(); }
// 7. The solution vector x and the associated finite element grid function
// will be maintained over the AMR iterations. We initialize it to zero.
Vector zero_vec(dim);
zero_vec = 0.0;
VectorConstantCoefficient zero_vec_coeff(zero_vec);
ParGridFunction x(&fespace);
x = 0.0;
// 8. 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. The conversion to true dofs will be done in the
// main loop.
Array<int> ess_bdr(pmesh.bdr_attributes.Max());
ess_bdr = 0;
ess_bdr[0] = 1;
// 9. GLVis visualization.
char vishost[] = "localhost";
int visport = 19916;
socketstream sol_sock;
// 10. Set up an error estimator. Here we use the Zienkiewicz-Zhu estimator
// that uses the ComputeElementFlux method of the ElasticityIntegrator to
// recover a smoothed flux (stress) that is subtracted from the element
// flux to get an error indicator. We need to supply the space for the
// smoothed flux: an (H1)^tdim (i.e., vector-valued) space is used here.
// Here, tdim represents the number of components for a symmetric (dim x
// dim) tensor.
const int tdim = dim*(dim+1)/2;
L2_FECollection flux_fec(order, dim);
ParFiniteElementSpace flux_fespace(&pmesh, &flux_fec, tdim);
ParFiniteElementSpace smooth_flux_fespace(&pmesh, &fec, tdim);
L2ZienkiewiczZhuEstimator estimator(*integ, x, flux_fespace,
smooth_flux_fespace);
// 11. A refiner selects and refines elements based on a refinement strategy.
// The strategy here is to refine elements with errors larger than a
// fraction of the maximum element error. Other strategies are possible.
// The refiner will call the given error estimator.
ThresholdRefiner refiner(estimator);
refiner.SetTotalErrorFraction(0.7);
// 12. The main AMR loop. In each iteration we solve the problem on the
// current mesh, visualize the solution, and refine the mesh.
const int max_dofs = 50000;
const int max_amr_itr = 20;
for (int it = 0; it <= max_amr_itr; it++)
{
HYPRE_Int global_dofs = fespace.GlobalTrueVSize();
if (myid == 0)
{
cout << "\nAMR iteration " << it << endl;
cout << "Number of unknowns: " << global_dofs << endl;
}
// 13. Assemble the stiffness matrix and the right-hand side.
a.Assemble();
b.Assemble();
// 14. Set Dirichlet boundary values in the GridFunction x.
// Determine the list of Dirichlet true DOFs in the linear system.
Array<int> ess_tdof_list;
x.ProjectBdrCoefficient(zero_vec_coeff, ess_bdr);
fespace.GetEssentialTrueDofs(ess_bdr, ess_tdof_list);
// 15. Create the linear system: eliminate boundary conditions, constrain
// hanging nodes and possibly apply other transformations. The system
// will be solved for true (unconstrained) DOFs only.
HypreParMatrix A;
Vector B, X;
const int copy_interior = 1;
a.FormLinearSystem(ess_tdof_list, x, b, A, X, B, copy_interior);
// 16. Define and apply a parallel PCG solver for AX=B with the BoomerAMG
// preconditioner from hypre.
HypreBoomerAMG amg;
amg.SetPrintLevel(0);
// amg.SetSystemsOptions(dim); // optional
CGSolver pcg(A.GetComm());
pcg.SetPreconditioner(amg);
pcg.SetOperator(A);
pcg.SetRelTol(1e-6);
pcg.SetMaxIter(500);
pcg.SetPrintLevel(3); // print the first and the last iterations only
pcg.Mult(B, X);
// 17. After solving the linear system, reconstruct the solution as a
// finite element GridFunction. Constrained nodes are interpolated
// from true DOFs (it may therefore happen that x.Size() >= X.Size()).
a.RecoverFEMSolution(X, b, x);
// 18. Send solution by socket to the GLVis server.
if (visualization && it == 0)
{
sol_sock.open(vishost, visport);
sol_sock.precision(8);
}
if (visualization && sol_sock.good())
{
GridFunction nodes(&fespace), *nodes_p = &nodes;
pmesh.GetNodes(nodes);
nodes += x;
int own_nodes = 0;
pmesh.SwapNodes(nodes_p, own_nodes);
x.Neg(); // visualize the backward displacement
sol_sock << "parallel " << num_procs << ' ' << myid << '\n';
sol_sock << "solution\n" << pmesh << x << flush;
x.Neg();
pmesh.SwapNodes(nodes_p, own_nodes);
if (it == 0)
{
sol_sock << "keys '" << ((dim == 2) ? "Rjl" : "") << "m'" << endl;
}
sol_sock << "window_title 'AMR iteration: " << it << "'\n"
<< "pause" << endl;
if (myid == 0)
{
cout << "Visualization paused. "
"Press <space> in the GLVis window to continue." << endl;
}
}
if (global_dofs > max_dofs)
{
if (myid == 0)
{
cout << "Reached the maximum number of dofs. Stop." << endl;
}
break;
}
// 19. Call the refiner to modify the mesh. The refiner calls the error
// estimator to obtain element errors, then it selects elements to be
// refined and finally it modifies the mesh. The Stop() method can be
// used to determine if a stopping criterion was met.
refiner.Apply(pmesh);
if (refiner.Stop())
{
if (myid == 0)
{
cout << "Stopping criterion satisfied. Stop." << endl;
}
break;
}
// 20. Update the space to reflect the new state of the mesh. Also,
// interpolate the solution x so that it lies in the new space but
// represents the same function. This saves solver iterations later
// since we'll have a good initial guess of x in the next step.
// Internally, FiniteElementSpace::Update() calculates an
// interpolation matrix which is then used by GridFunction::Update().
fespace.Update();
x.Update();
// 21. Load balance the mesh, and update the space and solution. Currently
// available only for nonconforming meshes.
if (pmesh.Nonconforming())
{
pmesh.Rebalance();
// Update the space and the GridFunction. This time the update matrix
// redistributes the GridFunction among the processors.
fespace.Update();
x.Update();
}
// 21. Inform also the bilinear and linear forms that the space has
// changed.
a.Update();
b.Update();
}
{
ostringstream mref_name, mesh_name, sol_name;
mref_name << "ex21p_reference_mesh." << setfill('0') << setw(6) << myid;
mesh_name << "ex21p_deformed_mesh." << setfill('0') << setw(6) << myid;
sol_name << "ex21p_displacement." << setfill('0') << setw(6) << myid;
ofstream mesh_ref_out(mref_name.str().c_str());
mesh_ref_out.precision(16);
pmesh.Print(mesh_ref_out);
ofstream mesh_out(mesh_name.str().c_str());
mesh_out.precision(16);
GridFunction nodes(&fespace), *nodes_p = &nodes;
pmesh.GetNodes(nodes);
nodes += x;
int own_nodes = 0;
pmesh.SwapNodes(nodes_p, own_nodes);
pmesh.Print(mesh_out);
pmesh.SwapNodes(nodes_p, own_nodes);
ofstream x_out(sol_name.str().c_str());
x_out.precision(16);
x.Save(x_out);
}
MPI_Finalize();
return 0;
}
You can’t perform that action at this time.