Linear elastic¶

Consider a uniform linear elastic bar that is extended by a uniform fixed displacement on both sides. This problem can be modelled and discretised using symmetry as show below. In this example we will furthermore assume that the bar is sufficiently thick in the out-of-plane direction to be modelled using two-dimensional plane strain.

Below an example is described line-by-line. The full example can be downloaded:

Note

This example is also available using the Python interface (example.py). Compared to the C++ API, the Python API requires more data-allocation, in particular for the functions AsElement and AssembleNode. See: Data allocation.

Include library¶

#include <GMatElastic/Cartesian3d.h>
#include <GooseFEM/GooseFEM.h>
#include <GooseFEM/MatrixPartitioned.h>
#include <highfive/H5Easy.hpp>


The first step is to include the header-only library. Note that for this example we also make use of a material model (GMatElastic) and a library to write (and read) HDF5 files (HighFive).

Define mesh¶

    // define mesh

// mesh dimensions
size_t nelem = mesh.nelem();
size_t nne = mesh.nne();
size_t ndim = mesh.ndim();

// mesh definitions
xt::xtensor<double, 2> coor = mesh.coor();
xt::xtensor<size_t, 2> conn = mesh.conn();
xt::xtensor<size_t, 2> dofs = mesh.dofs();

// node sets
xt::xtensor<size_t, 1> nodesLft = mesh.nodesLeftEdge();
xt::xtensor<size_t, 1> nodesRgt = mesh.nodesRightEdge();
xt::xtensor<size_t, 1> nodesTop = mesh.nodesTopEdge();
xt::xtensor<size_t, 1> nodesBot = mesh.nodesBottomEdge();


A mesh is defined using GooseFEM. As observed the mesh is a class that has methods to extract the relevant information such as the nodal coordinates (coor), the connectivity (conn), the degrees-of-freedom per node (dofs) and several node-sets that will be used to impose the sketched boundary conditions (nodesLeft, nodesRight, nodesTop, nodesBottom).

Note that:

• The connectivity (conn) contains information of which nodes, in which order, belong to which element.
• The degrees-of-freedom per node (dofs) contains information of how a nodal vector (a vector stored per node) can be transformed to a list of degrees-of-freedom as used in the linear system (although this can be mostly done automatically as we will see below).

Define partitioning¶

    xt::xtensor<size_t, 1> iip = xt::concatenate(xt::xtuple(
xt::view(dofs, xt::keep(nodesRgt), 0),
xt::view(dofs, xt::keep(nodesTop), 1),
xt::view(dofs, xt::keep(nodesLft), 0),
xt::view(dofs, xt::keep(nodesBot), 1)));


We will reorder such that degrees-of-freedom are ordered such that

where the subscript and respectively denote Unknown and Prescribed degrees-of-freedom. To achieve this we start by collecting all prescribed degrees-of-freedom in iip.

(Avoid) Book-keeping¶

    GooseFEM::VectorPartitioned vector(conn, dofs, iip);


To switch between the three of GooseFEM’s data-representations, an instance of the Vector class is used. This instance, vector, will enable us to switch between a vector field (e.g. the displacement)

1. collected per node,
2. collected per degree-of-freedom, or
3. collected per element.

Note

The Vector class collects most, if not all, the burden of book-keeping. It is thus here that conn, dofs, and iip are used. In particular,

• ‘nodevec’ ‘dofval’ using dofs and iip,
• ‘nodevec’ ‘elemvec’ using conn.

By contrast, most of GooseFEM’s other methods receive the relevant representation, and consequently require no problem specific knowledge. They thus do not have to supplied with conn, dofs, or iip.

System matrix¶

    GooseFEM::MatrixPartitioned K(conn, dofs, iip);
GooseFEM::MatrixPartitionedSolver<> Solver;


We now also allocate the system/stiffness system (stored as sparse matrix). Like vector, it can accept and return different vector representations, in addition to the ability to assemble from element system matrices.

In addition we allocate the accompanying sparse solver, that we will use to solve a linear system of equations. Note that the solver-class takes care of factorising only when needed (when the matrix has been changed).

Note

Here, the default solver is used (which is the default template, hence the “<>”). To use other solvers see: Linear solver.

Allocate nodal vectors¶

    xt::xtensor<double, 2> disp = xt::zeros<double>(coor.shape());
xt::xtensor<double, 2> fint = xt::zeros<double>(coor.shape());
xt::xtensor<double, 2> fext = xt::zeros<double>(coor.shape());
xt::xtensor<double, 2> fres = xt::zeros<double>(coor.shape());

• disp: nodal displacements
• fint: nodal internal forces
• fext: nodal external forces
• fres: nodal residual forces

Note

To allocate nodal vectors the convenience function:

vector.AllocateNodevec(); // allocate
vector.AllocateElemvec(0.0); // allocate & (zero-)initialise


is available, which takes care of getting the right shape. E.g.

auto disp = vector.AllocateNodevec(0.0);


Allocate element vectors¶

    xt::xtensor<double, 3> ue = xt::empty<double>({nelem, nne, ndim});
xt::xtensor<double, 3> fe = xt::empty<double>({nelem, nne, ndim});
xt::xtensor<double, 3> Ke = xt::empty<double>({nelem, nne * ndim, nne * ndim});

• ue: displacement
• fe: force
• Ke: tangent matrix

Warning

Upsizing (e.g. disp ue) can be done uniquely, but downsizing (e.g. fe fint) can be done in more than one way, see Conversion. We will get back to this point below.

Note

To allocate element vectors the convenience function:

vector.AllocateElemvec(); // allocate
vector.AllocateElemvec(0.0); // allocate & (zero-)initialise


is available, which takes care of getting the right shape. E.g.

auto ue = vector.AllocateElemvec(0.0);


Note

To allocate element matrices the convenience function:

vector.AllocateElemmat(); // allocate
vector.AllocateElemmat(0.0); // allocate & (zero-)initialise


is available, which takes care of getting the right shape. E.g.

auto Ke = vector.AllocateElemmat(0.0);


Element definition¶

    GooseFEM::Element::Quad4::QuadraturePlanar elem(vector.AsElement(coor));
size_t nip = elem.nip();


At this moment the interpolation and quadrature is allocated. The shape functions and integration points (that can be customised) are stored in this class. As observed, no further information is needed than the number of elements and the nodal coordinates per element. Both are contained in the output of vector.AsElement(coor), which is an ‘elemvec’ of shape “[nelem, nne, ndim]”. This illustrates that problem specific book-keeping is isolated to the main program, using Vector as tool.

Note

The shape-functions are computed when constructing this class, they are not recomputed when evaluating them. One can recompute them if the nodal coordinates change using “.update_x(…)”, however, this is only relevant in a large deformation setting.

Material definition¶

    GMatElastic::Cartesian3d::Matrix mat(nelem, nip, 1.0, 1.0);


We now define a uniform linear elastic material, using an external library that is tuned to GooseFEM. This material library will translate a strain tensor per integration point to a stress tensor per integration point and a stiffness tensor per integration point.

Material libraries tuned to GooseFEM include:

But other libraries can also be easily used with (simple) wrappers.

Integration point tensors¶

    xt::xtensor<double, 4> Eps = xt::empty<double>({nelem, nip, 3ul, 3ul});
xt::xtensor<double, 4> Sig = xt::empty<double>({nelem, nip, 3ul, 3ul});
xt::xtensor<double, 6> C = xt::empty<double>({nelem, nip, 3ul, 3ul, 3ul, 3ul});


These strain, stress, and stiffness tensors per integration point are now allocated. Note that these tensors are 3-d while our problem was 2-d. This is thanks to the plane strain assumption, and the element definition that ignores all third-dimension components.

Note

To allocate integration point the convenience function:

quad.AllocateQtensor<rank>(); // allocate


is available, which takes care of getting the right shape. E.g.

auto Eps = quad.AllocateQtensor<2>();


From Python simply use rank as the first function argument. Furthermore, for scalar you could use AllocateQscalar() which is equivalent to AllocateQtensor<0>().

Compute strain¶

    vector.asElement(disp, ue);


The strain per integration point is now computed using the current nodal displacements (stored as ‘elemvec’ in ue) and the gradient of the shape functions.

Note

ue is the output of vector.asElement(disp, ue). Using this syntax re-allocation of ue is avoided. If this optimisation is irrelevant for you problem (or if you are using the Python interface), please use the same function, but starting with a capital:

ue = vector.AsElement(disp);


Note that this allows the one-liner

Eps = elem.SymGradN_vector(vector.AElement(disp));


Compute stress and tangent¶

    mat.tangent(Eps, Sig, C);


The stress and stiffness tensors are now computed for each integration point (completely independently) using the external material model.

Note

Sig and C are the output variables that were preallocated in the main.

Assemble system¶

    // internal force
vector.assembleNode(fe, fint);

// stiffness matrix
K.assemble(Ke);


The stress stored per integration point (Sig) is now converted to nodal internal force vectors stored per element (fe). Using vector this ‘elemvec’ representation is then converted of a ‘nodevec’ representation in fint. Likewise, the stiffness tensor stored for integration point (C) are converted to system matrices stored per element (‘elemmat’) and finally assembled to the global stiffness matrix.

Warning

Please note that downsizing (fe fint and Ke K) can be done in two ways, and that “assemble…” is the right function here as it adds entries that occur more than once. In contrast “as…” would not result in what we want here.

Note

Once more, fe, fint, and Ke are output variables. Less efficient, but shorter, is:

// internal force

// stiffness matrix


Solve¶

    // set fixed displacements
xt::view(disp, xt::keep(nodesRgt), 0) = +0.1;
xt::view(disp, xt::keep(nodesTop), 1) = -0.1;
xt::view(disp, xt::keep(nodesLft), 0) = 0.0;
xt::view(disp, xt::keep(nodesBot), 1) = 0.0;

// residual
xt::noalias(fres) = fext - fint;

// solve
Solver.solve(K, fres, disp);


We now prescribe the displacement of the Prescribed degrees-of-freedom directly in the nodal displacements disp and compute the residual force. This is follows by partitioning and solving, all done internally in the MatrixPartitioned class.

Post-process¶

Strain and stress¶

    vector.asElement(disp, ue);
mat.stress(Eps, Sig);


The strain and stress per integration point are recomputed for post-processing.

Residual force¶

    // internal force
vector.assembleNode(fe, fint);

// apply reaction force
vector.copy_p(fint, fext);

// residual
xt::noalias(fres) = fext - fint;

// print residual
std::cout << xt::sum(xt::abs(fres))[0] / xt::sum(xt::abs(fext))[0] << std::endl;


We convince ourselves that the solution is indeed in mechanical equilibrium.

Store & plot¶

    // average stress per node
xt::xtensor<double, 4> dV = elem.AsTensor<2>(elem.dV());
xt::xtensor<double, 3> SigAv = xt::average(Sig, dV, {1});

// write output
H5Easy::File file("output.h5", H5Easy::File::Overwrite);
H5Easy::dump(file, "/coor", coor);
H5Easy::dump(file, "/conn", conn);
H5Easy::dump(file, "/disp", disp);
H5Easy::dump(file, "/Sig", SigAv);


Finally we store some fields for plotting using plot.py.

Manual partitioning¶

To verify how partitioning and solving is done internally using the MatrixPartitioned class, the same example is provided where partitioning is done manually: