simple_elasticity.cpp

Go to the documentation of this file.

/** \file simple_elasticity.cpp
 * \example simple_elasticity.cpp
 
 The example shows how to solve the linear elastic problem.
 
*/
 
#include <MoFEM.hpp>
 
using namespace boost::numeric;
using namespace MoFEM;
 
static char help[] = "-order approximation order\n"
                     "\n";
 
struct OpK : public VolumeElementForcesAndSourcesCore::UserDataOperator {
 
  // Finite element stiffness sub-matrix K_ij
  MatrixDouble K;
 
  // Elastic stiffness tensor (4th rank tensor with minor and major symmetry)
  FTensor::Ddg<double, 3, 3> tD;
 
  // Young's modulus
  double yOung;
  // Poisson's ratio
  double pOisson;
 
  OpK(bool symm = true)
      : VolumeElementForcesAndSourcesCore::UserDataOperator("U", "U", OPROWCOL,
                                                            symm) {
 
    // Evaluation of the elastic stiffness tensor, D
 
    // hardcoded choice of elastic parameters
    pOisson = 0.1;
    yOung = 10;
 
    // coefficient used in intermediate calculation
    const double coefficient = yOung / ((1 + pOisson) * (1 - 2 * pOisson));
 
    FTensor::Index<'i', 3> i;
    FTensor::Index<'j', 3> j;
    FTensor::Index<'k', 3> k;
    FTensor::Index<'l', 3> l;
 
    tD(i, j, k, l) = 0.;
 
    tD(0, 0, 0, 0) = 1 - pOisson;
    tD(1, 1, 1, 1) = 1 - pOisson;
    tD(2, 2, 2, 2) = 1 - pOisson;
 
    tD(0, 1, 0, 1) = 0.5 * (1 - 2 * pOisson);
    tD(0, 2, 0, 2) = 0.5 * (1 - 2 * pOisson);
    tD(1, 2, 1, 2) = 0.5 * (1 - 2 * pOisson);
 
    tD(0, 0, 1, 1) = pOisson;
    tD(1, 1, 0, 0) = pOisson;
    tD(0, 0, 2, 2) = pOisson;
    tD(2, 2, 0, 0) = pOisson;
    tD(1, 1, 2, 2) = pOisson;
    tD(2, 2, 1, 1) = pOisson;
 
    tD(i, j, k, l) *= coefficient;
  }
 
  /**
   * \brief Do calculations for give operator
   * @param  row_side row side number (local number) of entity on element
   * @param  col_side column side number (local number) of entity on element
   * @param  row_type type of row entity MBVERTEX, MBEDGE, MBTRI or MBTET
   * @param  col_type type of column entity MBVERTEX, MBEDGE, MBTRI or MBTET
   * @param  row_data data for row
   * @param  col_data data for column
   * @return          error code
   */
  MoFEMErrorCode doWork(int row_side, int col_side, EntityType row_type,
                        EntityType col_type,
                        EntitiesFieldData::EntData &row_data,
                        EntitiesFieldData::EntData &col_data) {
 
    MoFEMFunctionBegin;
 
    // get number of dofs on row
    nbRows = row_data.getIndices().size();
    // if no dofs on row, exit that work, nothing to do here
    if (!nbRows)
      MoFEMFunctionReturnHot(0);
 
    // get number of dofs on column
    nbCols = col_data.getIndices().size();
    // if no dofs on Columbia, exit nothing to do here
    if (!nbCols)
      MoFEMFunctionReturnHot(0);
 
    // K_ij matrix will have 3 times the number of degrees of freedom of the
    // i-th entity set (nbRows)
    // and 3 times the number of degrees of freedom of the j-th entity set
    // (nbCols)
    K.resize(nbRows, nbCols, false);
    K.clear();
 
    // get number of integration points
    nbIntegrationPts = getGaussPts().size2();
    // check if entity block is on matrix diagonal
    if (row_side == col_side && row_type == col_type) {
      isDiag = true;
    } else {
      isDiag = false;
    }
 
    // integrate local matrix for entity block
    CHKERR iNtegrate(row_data, col_data);
 
    // assemble local matrix
    CHKERR aSsemble(row_data, col_data);
 
    MoFEMFunctionReturn(0);
  }
 
protected:
  int nbRows;           ///< number of dofs on rows
  int nbCols;           ///< number if dof on column
  int nbIntegrationPts; ///< number of integration points
  bool isDiag;          ///< true if this block is on diagonal
 
  /**
   * \brief Integrate B^T D B operator
   * @param  row_data row data (consist base functions on row entity)
   * @param  col_data column data (consist base functions on column entity)
   * @return error code
   */
  MoFEMErrorCode iNtegrate(EntitiesFieldData::EntData &row_data,
                           EntitiesFieldData::EntData &col_data) {
    MoFEMFunctionBegin;
 
    // get sub-block (3x3) of local stiffens matrix, here represented by second
    // order tensor
    auto get_tensor2 = [](MatrixDouble &m, const int r, const int c) {
      return FTensor::Tensor2<FTensor::PackPtr<double *, 3>, 3, 3>(
          &m(r + 0, c + 0), &m(r + 0, c + 1), &m(r + 0, c + 2),
          &m(r + 1, c + 0), &m(r + 1, c + 1), &m(r + 1, c + 2),
          &m(r + 2, c + 0), &m(r + 2, c + 1), &m(r + 2, c + 2));
    };
 
    FTensor::Index<'i', 3> i;
    FTensor::Index<'j', 3> j;
    FTensor::Index<'k', 3> k;
    FTensor::Index<'l', 3> l;
 
    // get element volume
    double vol = getVolume();
 
    // get intergration weights
    auto t_w = getFTensor0IntegrationWeight();
 
    // get derivatives of base functions on rows
    auto t_row_diff_base = row_data.getFTensor1DiffN<3>();
    // iterate over integration points
    for (int gg = 0; gg != nbIntegrationPts; ++gg) {
 
      // calculate scalar weight times element volume
      const double a = t_w * vol;
 
      // iterate over row base functions
      for (int rr = 0; rr != nbRows / 3; ++rr) {
 
        // get sub matrix for the row
        auto t_m = get_tensor2(K, 3 * rr, 0);
 
        // get derivatives of base functions for columns
        auto t_col_diff_base = col_data.getFTensor1DiffN<3>(gg, 0);
 
        // iterate column base functions
        for (int cc = 0; cc != nbCols / 3; ++cc) {
 
          // integrate block local stiffens matrix
          t_m(i, k) +=
              a * (tD(i, j, k, l) * (t_row_diff_base(j) * t_col_diff_base(l)));
 
          // move to next column base function
          ++t_col_diff_base;
 
          // move to next block of local stiffens matrix
          ++t_m;
        }
 
        // move to next row base function
        ++t_row_diff_base;
      }
 
      // move to next integration weight
      ++t_w;
    }
 
    MoFEMFunctionReturn(0);
  }
 
  /**
   * \brief Assemble local entity block matrix
   * @param  row_data row data (consist base functions on row entity)
   * @param  col_data column data (consist base functions on column entity)
   * @return          error code
   */
  MoFEMErrorCode aSsemble(EntitiesFieldData::EntData &row_data,
                          EntitiesFieldData::EntData &col_data) {
    MoFEMFunctionBegin;
    // get pointer to first global index on row
    const int *row_indices = &*row_data.getIndices().data().begin();
    // get pointer to first global index on column
    const int *col_indices = &*col_data.getIndices().data().begin();
    Mat B = getFEMethod()->ksp_B != PETSC_NULLPTR ? getFEMethod()->ksp_B
                                               : getFEMethod()->snes_B;
    // assemble local matrix
    CHKERR MatSetValues(B, nbRows, row_indices, nbCols, col_indices,
                        &*K.data().begin(), ADD_VALUES);
 
    if (!isDiag && sYmm) {
      // if not diagonal term and since global matrix is symmetric assemble
      // transpose term.
      K = trans(K);
      CHKERR MatSetValues(B, nbCols, col_indices, nbRows, row_indices,
                          &*K.data().begin(), ADD_VALUES);
    }
    MoFEMFunctionReturn(0);
  }
};
 
struct OpPressure : MoFEM::FaceElementForcesAndSourcesCore::UserDataOperator {
 
  double pressureVal;
 
  OpPressure(const double pressure_val = 1)
      : MoFEM::FaceElementForcesAndSourcesCore::UserDataOperator("U", OPROW),
        pressureVal(pressure_val) {}
 
  // vector used to store force vector for each degree of freedom
  VectorDouble nF;
 
  FTensor::Index<'i', 3> i;
 
  MoFEMErrorCode doWork(int side, EntityType type,
                        EntitiesFieldData::EntData &data) {
 
    MoFEMFunctionBegin;
    // check that the faces have associated degrees of freedom
    const int nb_dofs = data.getIndices().size();
    if (nb_dofs == 0)
      MoFEMFunctionReturnHot(0);
 
    // size of force vector associated to the entity
    // set equal to the number of degrees of freedom of associated with the
    // entity
    nF.resize(nb_dofs, false);
    nF.clear();
 
    // get number of gauss points
    const int nb_gauss_pts = data.getN().size1();
 
    // create a 3d vector to be used as the normal to the face with length equal
    // to the face area
    auto t_normal = getFTensor1Normal();
 
    // get intergration weights
    auto t_w = getFTensor0IntegrationWeight();
 
    // vector of base functions
    auto t_base = data.getFTensor0N();
 
    // loop over all gauss points of the face
    for (int gg = 0; gg != nb_gauss_pts; ++gg) {
      // weight of gg gauss point
      double w = 0.5 * t_w;
 
      // create a vector t_nf whose pointer points an array of 3 pointers
      // pointing to nF  memory location of components
      FTensor::Tensor1<FTensor::PackPtr<double *, 3>, 3> t_nf(&nF[0], &nF[1],
                                                              &nF[2]);
      for (int bb = 0; bb != nb_dofs / 3; ++bb) {
        // scale the three components of t_normal and pass them to the t_nf
        // (hence to nF)
        t_nf(i) += (w * pressureVal * t_base) * t_normal(i);
        // move the pointer to next element of t_nf
        ++t_nf;
        // move to next base function
        ++t_base;
      }
 
      // move to next integration weight
      ++t_w;
    }
 
    // add computed values of pressure in the global right hand side vector
    CHKERR VecSetValues(getFEMethod()->ksp_f, nb_dofs, &data.getIndices()[0],
                        &nF[0], ADD_VALUES);
 
    MoFEMFunctionReturn(0);
  }
};
 
struct ApplyDirichletBc : public MoFEM::FEMethod {
 
  Range fixFaces, fixNodes, fixSecondNode;
 
  ApplyDirichletBc(const Range &fix_faces, const Range &fix_nodes,
                   const Range &fix_second_node)
      : MoFEM::FEMethod(), fixFaces(fix_faces), fixNodes(fix_nodes),
        fixSecondNode(fix_second_node) {
    // constructor
  }
 
  MoFEMErrorCode postProcess() {
 
    MoFEMFunctionBegin;
    std::set<int> set_fix_dofs;
 
    for (_IT_NUMEREDDOF_ROW_FOR_LOOP_(problemPtr, dit)) {
      if (dit->get()->getDofCoeffIdx() == 2) {
        if (fixFaces.find(dit->get()->getEnt()) != fixFaces.end()) {
          set_fix_dofs.insert(dit->get()->getPetscGlobalDofIdx());
        }
      }
 
      if (fixSecondNode.find(dit->get()->getEnt()) != fixSecondNode.end()) {
        if (dit->get()->getDofCoeffIdx() == 1) {
          set_fix_dofs.insert(dit->get()->getPetscGlobalDofIdx());
        }
      }
 
      if (fixNodes.find(dit->get()->getEnt()) != fixNodes.end()) {
        set_fix_dofs.insert(dit->get()->getPetscGlobalDofIdx());
      }
    }
 
    std::vector<int> fix_dofs(set_fix_dofs.size());
 
    std::copy(set_fix_dofs.begin(), set_fix_dofs.end(), fix_dofs.begin());
 
    CHKERR MatAssemblyBegin(ksp_B, MAT_FINAL_ASSEMBLY);
    CHKERR MatAssemblyEnd(ksp_B, MAT_FINAL_ASSEMBLY);
    CHKERR VecAssemblyBegin(ksp_f);
    CHKERR VecAssemblyEnd(ksp_f);
 
    Vec x;
 
    CHKERR VecDuplicate(ksp_f, &x);
    CHKERR VecZeroEntries(x);
    CHKERR MatZeroRowsColumns(ksp_B, fix_dofs.size(), &fix_dofs[0], 1, x,
                              ksp_f);
 
    CHKERR VecDestroy(&x);
 
    MoFEMFunctionReturn(0);
  }
};
 
/**
 * \brief Set integration rule to volume elements
 *
 * This rule is used to integrate \f$\nabla v \cdot \nabla u\f$, thus
 * if the approximation field and the testing field are polynomials of order
 * "p", then the rule for the exact integration is 2*(p-1).
 *
 * Integration rule is order of polynomial which is calculated exactly. Finite
 * element selects integration method based on return of this function.
 *
 */
struct VolRule {
  int operator()(int, int, int p) const { return 2 * (p - 1); }
};
 
/**
 * \brief Set integration rule to boundary elements
 *
 * This rule is used to integrate the work of external forces on a face,
 * i.e. \f$f \cdot v\f$, where f is the traction vector and v is the test
 * vector function. The current problem features a Neumann bc with
 * a pre-defined constant pressure. Therefore, if the test field is
 * represented by polynomials of order "p", then the rule for the exact
 * integration is also p.
 *
 * Integration rule is order of polynomial which is calculated exactly. Finite
 * element selects integration method based on return of this function.
 *
 */
struct FaceRule {
  int operator()(int, int, int p) const { return p; }
};
 
int main(int argc, char *argv[]) {
 
  const string default_options = "-ksp_type fgmres \n"
                                 "-pc_type lu \n"
                                 "-pc_factor_mat_solver_type mumps \n"
                                 "-mat_mumps_icntl_20 0 \n"
                                 "-ksp_monitor\n";
 
  string param_file = "param_file.petsc";
  if (!static_cast<bool>(ifstream(param_file))) {
    std::ofstream file(param_file.c_str(), std::ios::ate);
    if (file.is_open()) {
      file << default_options;
      file.close();
    }
  }
 
  MoFEM::Core::Initialize(&argc, &argv, param_file.c_str(), help);
 
  // Create mesh database
  moab::Core mb_instance;              // create database
  moab::Interface &moab = mb_instance; // create interface to database
 
  try {
    // Create MoFEM database and link it to MoAB
    MoFEM::Core core(moab);
    MoFEM::Interface &m_field = core;
 
    CHKERR DMRegister_MoFEM("DMMOFEM");
 
    // Get command line options
    int order = 3;                    // default approximation order
    PetscBool flg_test = PETSC_FALSE; // true check if error is numerical error
    PetscOptionsBegin(PETSC_COMM_WORLD, "", "SimpleElasticProblem",
                             "none");
 
    // Set approximation order
    CHKERR PetscOptionsInt("-order", "approximation order", "", order, &order,
                           PETSC_NULLPTR);
 
    // Set testing (used by CTest)
    CHKERR PetscOptionsBool("-test", "if true is ctest", "", flg_test,
                            &flg_test, PETSC_NULLPTR);
 
    PetscOptionsEnd();
 
    Simple *simple_interface = m_field.getInterface<MoFEM::Simple>();
 
    CHKERR simple_interface->getOptions();
    CHKERR simple_interface->loadFile();
 
    Range fix_faces, pressure_faces, fix_nodes, fix_second_node;
 
    enum MyBcTypes {
      FIX_BRICK_FACES = 1,
      FIX_NODES = 2,
      BRICK_PRESSURE_FACES = 3,
      FIX_NODES_Y_DIR = 4
    };
 
    for (_IT_CUBITMESHSETS_BY_BCDATA_TYPE_FOR_LOOP_(m_field, BLOCKSET, bit)) {
      EntityHandle meshset = bit->getMeshset();
      int id = bit->getMeshsetId();
 
      if (id == FIX_BRICK_FACES) { // brick-faces
 
        CHKERR m_field.get_moab().get_entities_by_dimension(meshset, 2,
                                                            fix_faces, true);
 
        Range adj_ents;
        CHKERR m_field.get_moab().get_adjacencies(fix_faces, 0, false, adj_ents,
                                                  moab::Interface::UNION);
 
        CHKERR m_field.get_moab().get_adjacencies(fix_faces, 1, false, adj_ents,
                                                  moab::Interface::UNION);
        fix_faces.merge(adj_ents);
      } else if (id == FIX_NODES) { // node(s)
 
        CHKERR m_field.get_moab().get_entities_by_dimension(meshset, 0,
                                                            fix_nodes, true);
 
      } else if (id == BRICK_PRESSURE_FACES) { // brick pressure faces
        CHKERR m_field.get_moab().get_entities_by_dimension(
            meshset, 2, pressure_faces, true);
 
      } else if (id ==
                 FIX_NODES_Y_DIR) { // restrained second node in y direction
        CHKERR m_field.get_moab().get_entities_by_dimension(
            meshset, 0, fix_second_node, true);
 
      } else {
        SETERRQ(PETSC_COMM_WORLD, MOFEM_DATA_INCONSISTENCY, "Unknown blockset");
      }
    }
 
    CHKERR simple_interface->addDomainField("U", H1, AINSWORTH_LEGENDRE_BASE,
                                            3);
    CHKERR simple_interface->setFieldOrder("U", order);
 
    CHKERR simple_interface->defineFiniteElements();
 
    // Add pressure element
    CHKERR m_field.add_finite_element("PRESSURE");
    CHKERR m_field.modify_finite_element_add_field_row("PRESSURE", "U");
    CHKERR m_field.modify_finite_element_add_field_col("PRESSURE", "U");
    CHKERR m_field.modify_finite_element_add_field_data("PRESSURE", "U");
 
    CHKERR simple_interface->defineProblem();
 
    DM dm;
    CHKERR simple_interface->getDM(&dm);
 
    CHKERR DMMoFEMAddElement(dm, "PRESSURE");
    CHKERR DMMoFEMSetIsPartitioned(dm, PETSC_TRUE);
 
    CHKERR simple_interface->buildFields();
    CHKERR simple_interface->buildFiniteElements();
 
    CHKERR m_field.add_ents_to_finite_element_by_dim(pressure_faces, 2,
                                                     "PRESSURE");
    CHKERR m_field.build_finite_elements("PRESSURE", &pressure_faces);
 
    CHKERR simple_interface->buildProblem();
 
    // Create elements instances
    boost::shared_ptr<VolumeElementForcesAndSourcesCore> elastic_fe(
        new VolumeElementForcesAndSourcesCore(m_field));
    boost::shared_ptr<FaceElementForcesAndSourcesCore> pressure_fe(
        new FaceElementForcesAndSourcesCore(m_field));
 
    // Set integration rule to elements instances
    elastic_fe->getRuleHook = VolRule();
    pressure_fe->getRuleHook = FaceRule();
 
    // Add operators to element instances
    // push operators to elastic_fe
    elastic_fe->getOpPtrVector().push_back(new OpK());
    // push operators to pressure_fe
    pressure_fe->getOpPtrVector().push_back(new OpPressure());
 
    boost::shared_ptr<FEMethod> fix_dofs_fe(
        new ApplyDirichletBc(fix_faces, fix_nodes, fix_second_node));
 
    boost::shared_ptr<FEMethod> null_fe;
 
    // Set operators for KSP solver
    CHKERR DMMoFEMKSPSetComputeOperators(
        dm, simple_interface->getDomainFEName(), elastic_fe, null_fe, null_fe);
 
    CHKERR DMMoFEMKSPSetComputeRHS(dm, "PRESSURE", pressure_fe, null_fe,
                                   null_fe);
 
    // initialise matrix A used as the global stiffness matrix
    Mat A;
 
    // initialise left hand side vector x and right hand side vector f
    Vec x, f;
 
    // allocate memory handled by MoFEM discrete manager for matrix A
    CHKERR DMCreateMatrix(dm, &A);
 
    // allocate memory handled by MoFEM discrete manager for vector x
    CHKERR DMCreateGlobalVector(dm, &x);
 
    // allocate memory handled by MoFEM discrete manager for vector f of the
    // same size as x
    CHKERR VecDuplicate(x, &f);
 
    // precondition matrix A according to fix_dofs_fe  and elastic_fe finite
    // elements
    elastic_fe->ksp_B = A;
    fix_dofs_fe->ksp_B = A;
 
    // precondition the right hand side vector f according to fix_dofs_fe  and
    // elastic_fe finite elements
    fix_dofs_fe->ksp_f = f;
    pressure_fe->ksp_f = f;
 
    CHKERR DMoFEMLoopFiniteElements(dm, simple_interface->getDomainFEName(),
                                    elastic_fe);
 
    CHKERR DMoFEMLoopFiniteElements(dm, "PRESSURE", pressure_fe);
 
    // This is done because only post processor is implemented in the
    // ApplyDirichletBc struct
    CHKERR DMoFEMPostProcessFiniteElements(dm, fix_dofs_fe.get());
 
    // make available a KSP solver
    KSP solver;
 
    // make the solver available for parallel computing by determining its MPI
    // communicator
    CHKERR KSPCreate(PETSC_COMM_WORLD, &solver);
 
    // making available running all options available for KSP solver in running
    // command
    CHKERR KSPSetFromOptions(solver);
 
    // set A matrix with preconditioner
    CHKERR KSPSetOperators(solver, A, A);
 
    // set up the solver data strucure for the iterative solver
    CHKERR KSPSetUp(solver);
 
    // solve the system of linear equations
    CHKERR KSPSolve(solver, f, x);
 
    // destroy solver no needed any more
    CHKERR KSPDestroy(&solver);
 
    // make vector x available for parallel computations for visualization
    // context
    VecView(x, PETSC_VIEWER_STDOUT_WORLD);
 
    // save solution in vector x on mesh
    CHKERR DMoFEMMeshToGlobalVector(dm, x, INSERT_VALUES, SCATTER_REVERSE);
 
    // Set up post-processor. It is some generic implementation of finite
    // element
    auto get_post_proc_ele = [&]() {
      auto jac_ptr = boost::make_shared<MatrixDouble>();
      auto inv_jac_ptr = boost::make_shared<MatrixDouble>();
      auto det_ptr = boost::make_shared<VectorDouble>();
 
      auto post_proc_ele = boost::make_shared<
          PostProcBrokenMeshInMoab<VolumeElementForcesAndSourcesCore>>(m_field);
      // Add operators to the elements, starting with some generic
      constexpr int SPACE_DIM = 3;
      post_proc_ele->getOpPtrVector().push_back(
          new OpCalculateHOJac<SPACE_DIM>(jac_ptr));
      post_proc_ele->getOpPtrVector().push_back(
          new OpInvertMatrix<SPACE_DIM>(jac_ptr, det_ptr, inv_jac_ptr));
      post_proc_ele->getOpPtrVector().push_back(
          new OpSetHOInvJacToScalarBases<SPACE_DIM>(H1, inv_jac_ptr));
 
      auto u_ptr = boost::make_shared<MatrixDouble>();
      auto grad_ptr = boost::make_shared<MatrixDouble>();
      post_proc_ele->getOpPtrVector().push_back(
          new OpCalculateVectorFieldValues<SPACE_DIM>("U", u_ptr));
      post_proc_ele->getOpPtrVector().push_back(
          new OpCalculateVectorFieldGradient<SPACE_DIM, SPACE_DIM>("U",
                                                                   grad_ptr));
      using OpPPMap = OpPostProcMapInMoab<SPACE_DIM, SPACE_DIM>;
 
      post_proc_ele->getOpPtrVector().push_back(
 
          new OpPPMap(
 
              post_proc_ele->getPostProcMesh(), post_proc_ele->getMapGaussPts(),
              {},
 
              {{"U", u_ptr}},
 
              {{"GRAD", grad_ptr}},
 
              {})
 
      );
 
      return post_proc_ele;
    };
 
    if (auto post_proc = get_post_proc_ele()) {
      CHKERR DMoFEMLoopFiniteElements(dm, simple_interface->getDomainFEName(),
                                      post_proc);
      // write output
      CHKERR post_proc->writeFile("out.h5m");
    }
 
    {
      if (flg_test == PETSC_TRUE) {
        const double x_vec_norm_const = 0.4;
        // Check norm_1  value
        double norm_check;
        // Takes maximal element of the vector, that should be maximal
        // displacement at the end of the bar
        CHKERR VecNorm(x, NORM_INFINITY, &norm_check);
        if (std::abs(norm_check - x_vec_norm_const) / x_vec_norm_const >
            1.e-10) {
          SETERRQ(PETSC_COMM_SELF, MOFEM_ATOM_TEST_INVALID,
                   "test failed (nrm 2 %6.4e)", norm_check);
        }
      }
    }
 
    // free memory handled by mofem discrete manager for A, x and f
    CHKERR MatDestroy(&A);
    CHKERR VecDestroy(&x);
    CHKERR VecDestroy(&f);
 
    // free memory allocated for mofem discrete manager
    CHKERR DMDestroy(&dm);
 
    // This is a good reference for the future
  }
  CATCH_ERRORS;
 
  // finish work cleaning memory, getting statistics, etc
  MoFEM::Core::Finalize();
 
  return 0;
}