Multiple Solid Bodies
---------------------

This section demonstrates how to set up a problem with two regions, each associated to a
separated solid body. Different element formulations are used for the solid bodies.

..  pyvista-plot::
    :context:

    import felupe as fem

    inner = fem.Rectangle(a=(-1, -1), b=(1, 1), n=(5, 5)).triangulate()
    
    lower = fem.Rectangle(a=(-3, -3), b=(3, -1), n=(13, 5))
    upper = fem.Rectangle(a=(-3, 1), b=(3, 3), n=(13, 5))
    left = fem.Rectangle(a=(-3, -1), b=(-1, 1), n=(5, 5))
    right = fem.Rectangle(a=(1, -1), b=(3, 1), n=(5, 5))
    
    outer = fem.MeshContainer([lower, upper, left, right], merge=True).stack()
    
    container = fem.MeshContainer([inner, outer], merge=True)


A top-level (vertex) field, which contains all the unknowns, is required for the
definition of the boundary conditions as well as for the evaluation of the job.

..  note::
    Ensure to init the mesh container with ``merge=True``, otherwise the points-array of
    the container will be empty.
    
..  pyvista-plot::
    :context:
    :force_static:

    container = fem.MeshContainer([inner, outer], merge=True)
    field = fem.Field.from_mesh_container(container).as_container()
    
    field.plot(plotter=container.plot(), point_size=15, color="red").show()

The sub-meshes are available in the global mesh container, on which the sub-fields are
created.

..  pyvista-plot::
    :context:

    regions = [
        fem.RegionTriangle(container.meshes[0]),
        fem.RegionQuad(container.meshes[1]),
    ]
    fields = [
        fem.FieldContainer([fem.FieldPlaneStrain(regions[0], dim=2)]),
        fem.FieldContainer([fem.FieldPlaneStrain(regions[1], dim=2)]),
    ]
    
The displacement boundaries are created on the top-level field.

..  pyvista-plot::
    :context:

    boundaries = dict(
        fixed=fem.Boundary(field[0], fx=field.region.mesh.x.min()),
        move=fem.Boundary(field[0], fx=field.region.mesh.x.max()),
    )


The rubber is associated to a Neo-Hookean material formulation whereas the steel is
modeled by a linear elastic material formulation. Due to the large rotation, its
large-strain formulation is required. For each material a solid body is created.

..  pyvista-plot::
    :context:

    # two material model formulations
    linear_elastic = fem.LinearElasticLargeStrain(E=100, nu=0.3)
    neo_hooke = fem.NeoHooke(mu=1, bulk=1)
    
    # the solid bodies
    fiber = fem.SolidBody(umat=linear_elastic, field=fields[0])
    matrix = fem.SolidBody(umat=neo_hooke, field=fields[1])


A step is created and further added to a job. The global field must be passed as the
``x0`` argument during the evaluation of the job. Internally, all field values are
linked automatically, i.e. they share their ``values`` array.

..  pyvista-plot::
    :context:
    :force_static:

    # prepare a step with substeps
    move = fem.math.linsteps([0, 3], num=10)
    step = fem.Step(
        items=[matrix, fiber],
        ramp={boundaries["move"]: move}, 
        boundaries=boundaries,
    )
    
    # take care of the x0-argument
    job = fem.Job(steps=[step])
    job.evaluate(x0=field)

    fields[1].plot(
        "Principal Values of Logarithmic Strain", 
        show_undeformed=False, 
        plotter=fields[0].plot(
            "Principal Values of Logarithmic Strain", show_undeformed=False
        ),
    ).show()