Error: unable to find closest node! in the mortar contact introduction

[b1llg]

Hi,

I tried the examples in the contact module (https://mooseframework.inl.gov/modules/contact/tutorials/introduction/step02.html) and came up with this error while doing the step 2:

Time Step 4, time = 2, dt = 0.5
  Applying predictor with scale factor = 1
 0 Nonlinear |R| = 8.693401e+05
 1 Nonlinear |R| = 4.300712e+06
  Linear solve did not converge due to DIVERGED_PC_FAILED iterations 0
                 PC failed due to FACTOR_NUMERIC_ZEROPIVOT 


*** ERROR ***
Unable to find closest node!

Stack frames: 37
0: libMesh::print_trace(std::ostream&)
1: moose::internal::mooseErrorRaw(std::__cxx11::basic_string<char, std::char_traits<char>, std::allocator<char> >, std::__cxx11::basic_string<char, std::char_traits<char>, std::allocator<char> >)
2: void mooseError<char const (&) [29]>(char const (&) [29])
3: /home/bill/projects/moose/framework/libmoose-opt.so.0(+0x21d1ec7) [0x7f52d2347ec7]
4: KDTree::neighborSearch(libMesh::Point const&, unsigned int, std::vector<unsigned long, std::allocator<unsigned long> >&)
5: SecondaryNeighborhoodThread::operator()(libMesh::StoredRange<__gnu_cxx::__normal_iterator<unsigned long*, std::vector<unsigned long, std::allocator<unsigned long> > >, unsigned long> const&)
6: /home/bill/projects/moose/framework/libmoose-opt.so.0(+0x1b8977c) [0x7f52d1cff77c]
7: NearestNodeLocator::findNodes()
8: GeometricSearchData::update(GeometricSearchData::GeometricSearchType)
9: DisplacedProblem::updateMesh(bool)
10: FEProblemBase::computeResidualTags(std::set<unsigned int, std::less<unsigned int>, std::allocator<unsigned int> > const&)
11: FEProblemBase::computeResidualInternal(libMesh::NumericVector<double> const&, libMesh::NumericVector<double>&, std::set<unsigned int, std::less<unsigned int>, std::allocator<unsigned int> > const&)
12: FEProblemBase::computeResidualSys(libMesh::NonlinearImplicitSystem&, libMesh::NumericVector<double> const&, libMesh::NumericVector<double>&)
13: ComputeResidualFunctor::residual(libMesh::NumericVector<double> const&, libMesh::NumericVector<double>&, libMesh::NonlinearImplicitSystem&)
14: libmesh_petsc_snes_residual
15: SNESComputeFunction
16: /home/bill/miniforge/envs/moose/lib/libpetsc.so.3.20(+0xf8f5aa) [0x7f52cbade5aa]
17: SNESLineSearchApply
18: /home/bill/miniforge/envs/moose/lib/libpetsc.so.3.20(+0xf6afdc) [0x7f52cbab9fdc]
19: SNESSolve
20: libMesh::PetscNonlinearSolver<double>::solve(libMesh::SparseMatrix<double>&, libMesh::NumericVector<double>&, libMesh::NumericVector<double>&, double, unsigned int)
21: libMesh::NonlinearImplicitSystem::solve()
22: TimeIntegrator::solve()
23: NonlinearSystem::solve()
24: FEProblemBase::solve(unsigned int)
25: FEProblemSolve::solve()
26: FixedPointSolve::solveStep(double&, double&, std::set<unsigned long, std::less<unsigned long>, std::allocator<unsigned long> > const&)
27: FixedPointSolve::solve()
28: TimeStepper::step()
29: Transient::takeStep(double)
30: Transient::execute()
31: MooseApp::executeExecutioner()
32: MooseApp::run()
33: main
34: /lib/x86_64-linux-gnu/libc.so.6(+0x29d90) [0x7f52c7da3d90]
35: __libc_start_main
36: ./contact_mech-opt(+0x33ef) [0x5629024053ef]
application called MPI_Abort(MPI_COMM_WORLD, 1) - process 0
[unset]: write_line error; fd=-1 buf=:cmd=abort exitcode=1
:
system msg for write_line failure : Bad file descriptor

I copy and pasted the whole input file from the link above. The only difference between step01 and step02 is replacing the penalty formulation by mortar. Here is the input file, is the the exact same as the one in the link above:

#
# A first attempt at mechanical contact
# https://mooseframework.inl.gov/modules/contact/tutorials/introduction/step01.html
#

[GlobalParams]
  displacements = 'disp_x disp_y'
  block = 0
[]

[Mesh]
  [generated1]
    type = GeneratedMeshGenerator
    dim = 2
    nx = 5
    ny = 15
    xmin = -0.6
    xmax = -0.1
    ymax = 5
    bias_y = 0.9
    boundary_name_prefix = pillar1
  []
  [generated2]
    type = GeneratedMeshGenerator
    dim = 2
    nx = 5
    ny = 15
    xmin = 0.1
    xmax = 0.6
    ymax = 5
    bias_y = 0.9
    boundary_name_prefix = pillar2
    boundary_id_offset = 4
  []
  [collect_meshes]
    type = MeshCollectionGenerator
    inputs = 'generated1 generated2'
  []

  patch_update_strategy = iteration
[]

[Modules/TensorMechanics/Master]
  [all]
    add_variables = true
    strain = FINITE
    generate_output = 'vonmises_stress'
  []
[]

[Contact]
  [pillars]
    primary = pillar1_right
    secondary = pillar2_left
    model = frictionless
    formulation = mortar

  []
[]

[BCs]
  [bottom_x]
    type = DirichletBC
    variable = disp_x
    boundary = 'pillar1_bottom pillar2_bottom'
    value = 0
  []
  [bottom_y]
    type = DirichletBC
    variable = disp_y
    boundary = 'pillar1_bottom pillar2_bottom'
    value = 0
  []
  [Pressure]
    [sides]
      boundary = 'pillar1_left pillar2_right'
      # we square time here to get a more progressive loading curve
      # (more pressure later on once contact is established)
      function = 1e4*t^2
    []
  []
[]

[Materials]
  [elasticity]
    type = ComputeIsotropicElasticityTensor
    youngs_modulus = 1e9
    poissons_ratio = 0.3
  []
  [stress]
    type = ComputeFiniteStrainElasticStress
  []
[]

[Executioner]
  type = Transient
  solve_type = NEWTON
  line_search = none
  petsc_options_iname = '-pc_type'
  petsc_options_value = 'lu'
  end_time = 5
  dt = 0.5
  [Predictor]
    type = SimplePredictor
    scale = 1
  []
[]

[Outputs]
  exodus = true
  print_linear_residuals = false
  perf_graph = true
[]

I started using Moose 2 days ago and I made sure it was up to date after the install.

[GiudGiud]

Thanks for reporting. It looks like this input has fallen in disrepair.
@recuero should be able to help next week. Let's use issue #26442 for the patch

[lindsayad]

The solve will go to completion if you add the petsc option -pc_factor_shift_type NONZERO

[lindsayad]

Did you make other modifications to the input? The largest penetration I see is 2.1e-9

[b1llg]

Apparently, if you use the input from the tensor mechanics module and work your way up to the contact tutorial (as it is suggested), there is a difference in the dimension:

On the left: the input if you start from tensor mechanics tutorials. (8.6e-9)
On the right: the input from step 2 in the contact tutorials. (2.1e-9)

So the difference is the number of elements.

In both case I added -pc_factor_shift_type=NONZERO

[lindsayad]

The relevant parameter is actually ymax. If you have ymax = 4.999 and you vary the number of elements you should hopefully always see the penetration of order 1e-9 or less.

However, if you keep ymax = 5, can you try adding correct_edge_dropping = true in the Contact/pillars block? That resolves the 1e-4 penetration issue for me (as well as dramatically improves the solver convergence)

[b1llg]

I get 1.5e-11.

[lindsayad]

sounds good!