Plate with a Hole#

Plane stress structural linear analysis.

  • create and mesh a plate with a hole

  • define a solid body with a linear-elastic plane stress material

  • create an external pressure load

  • export and plot stress results

A plate with length \(2L\), height \(2h\) and a hole with radius \(r\) is subjected to a uniaxial tension \(p=-100\) MPa. What is being looked for is the von Mises stress distribution and the concentration of normal stress \(\sigma_{11}\) over the hole.


Let’s create a meshed plate with a hole out of quad cells with the help of pygmsh (install with pip install pygmsh). Only a quarter model of the plate is considered. A boolean difference between a rectangle and a disk results in a plate with a hole. This plate is meshed with triangles. A so-called re-combination of the surface mesh gives a mesh with quad cells.

import felupe as fem
import pygmsh

h = 1.0
L = 2.0
r = 0.3

with pygmsh.occ.Geometry() as geom:

    geom.characteristic_length_min = 0.02
    geom.characteristic_length_max = 0.02

    rectangle = geom.add_rectangle([0, 0, 0], L, h)
    disk = geom.add_disk([0, 0, 0], r)

    plate = geom.boolean_difference(rectangle, disk)

    mesh = geom.generate_mesh()

The points and cells of the above mesh are used to initiate a FElupe mesh.

mesh = fem.Mesh(
    points=mesh.points[:, :2],

A numeric quad-region created on the mesh in combination with a vector-valued displacement field represents the plate. The Boundary conditions for the symmetry planes are generated on the displacement field.

region = fem.RegionQuad(mesh)
displacement = fem.Field(region, dim=2)
field = fem.FieldContainer([displacement])

boundaries = fem.dof.symmetry(displacement)

The material behavior is defined through a built-in isotropic linear-elastic material formulation for plane stress problems. A solid body applies the linear-elastic material formulation on the displacement field.

umat = fem.LinearElasticPlaneStress(E=210000, nu=0.3)
solid = fem.SolidBody(umat, field)

The external uniaxial tension is applied by a pressure load on the right end at \(x=L\). Therefore, a boundary region in combination with a field has to be created at \(x=L\).

region_boundary = fem.RegionQuadBoundary(mesh, mask=mesh.points[:, 0] == L)
field_boundary = fem.FieldContainer([fem.Field(region_boundary, dim=2)])

load = fem.SolidBodyPressure(field_boundary, pressure=-100)

The equivalent stress von Mises, projected to mesh points, will be added to the result file. For the two-dimensional case it is calculated by:

\[\sigma_{vM} = \sqrt{\sigma_{11}^2 + \sigma_{22}^2 + 3 \ \sigma_{12}^2 + \sigma_{11} \ \sigma_{22}}\]
import numpy as np

def von_mises(substep):
    "Von Mises Stress projected to mesh points."

    stress = solid.evaluate.gradient(substep.x)[0]

    vonmises = np.sqrt(
        stress[0, 0] ** 2 + stress[1, 1] ** 2 + 3 * stress[0, 1] ** 2 +
        stress[0, 0] * stress[1, 1]

    return fem.project(vonmises, region)

The simulation model is now ready to be solved. The results are saved within a XDMF-file, where additional point-data is passed to the point_data argument.

step = fem.Step(items=[solid, load], boundaries=boundaries)
job = fem.Job(steps=[step])
job.evaluate(filename="result.xdmf", point_data={"von Mises Stress": von_mises})

The normal stress distribution over the hole at \(x=0\) is plotted with matplotlib.

import matplotlib.pyplot as plt

left = mesh.points[:, 0] == 0

plt.plot([0], region)[:, 0][left],
    mesh.points[:, 1][left] / h,

plt.xlabel(r"$\sigma_{11}(x=0, y)$ in MPa $\longrightarrow$")
plt.ylabel(r"$y/h$ $\longrightarrow$")