Linear Elasticity

Standard isotropic linear elasticity (src/models/LinearElasticity.jl).

Two constructors are provided:

Hooke – 3D isotropic linear elasticity, parameterized by E and ν.
Hooke2D – 2D isotropic linear elasticity, with a plane_stress::Bool keyword. By default it builds a plane strain stiffness; pass plane_stress=true for the analytical plane stress matrix.

Mathematical formulation

The 3D Hooke model uses the fourth-order isotropic Lamé stiffness $C_{ijkl} = \lambda\delta_{ij}\delta_{kl} + \mu\left[\delta_{ik}\delta_{jl} + \delta_{il}\delta_{jk}\right]$, where $C_{ijkl}$ maps strain to stress, $\delta_{ij}$ is the Kronecker delta, and the indices $i,j,k,l$ run over the spatial dimensions. The Lamé parameters are $\lambda = E\nu / \left[\left[1+\nu\right]\left[1-2\nu\right]\right]$ and $\mu = E / \left[2\left[1+\nu\right]\right]$. Hooke2D uses the same Lamé form for plane strain and an analytical Voigt matrix for plane stress.

Implementation details

Hooke and Hooke2D are stateless, i.e., create_state returns NoState(). The stress given by σ = C : ε, using the constant material tangent C. The generic small-strain element routine accumulates (ε(δu_i) : C : ε(δu_j)) * α_dΩ at each quadrature point. Here, ε(δu_i) is the symmetric strain associated with basis function displacement δu_i, and α_dΩ is the quadrature weight including the alpha scaling and the independent volume measure. Hooke and Hooke2D implement the material-interface method is_linear with true, so the assembler preassembles K_linear once during create_assembler; subsequent stiffness_matrix calls only handle nonlinear cells and add K_linear * u to the residual.

Constructor

Hooke(E, ν)                       # 3D isotropic linear elasticity
Hooke2D(E, ν; plane_stress=false) # 2D plane strain
Hooke2D(E, ν; plane_stress=true)  # 2D plane stress

Hooke2D analytical plane stress

When Hooke2D is constructed with plane_stress=true, the stiffness matrix is built in Voigt form as

\[C^{\mathrm{ps}} = \frac{E}{1-\nu^2} \begin{pmatrix} 1 & \nu & 0 \\ \nu & 1 & 0 \\ 0 & 0 & \left[1-\nu\right]/2 \end{pmatrix}\]

and converted to a SymmetricTensor{4,2} via fromvoigt. Otherwise the plane strain stiffness is the standard Lamé form as

\[C^{\mathrm{pe}}_{ijkl} = \lambda\,\delta_{ij}\delta_{kl} + \mu\, \left[\delta_{ik}\delta_{jl} + \delta_{il}\delta_{jk}\right]\]

with $\lambda = E\nu / \left[\left[1+\nu\right]\left[1-2\nu\right]\right]$ and $\mu = E / \left[2\left[1+\nu\right]\right]$.

Hooke2D vs PlaneStrain(Hooke) / PlaneStress(Hooke)

Hooke2D is a direct analytical 2D form, while PlaneStrain(Hooke) / PlaneStress(Hooke) are the wrappers that take a 3D Hooke and reduce it to a 2D problem through 2D-to-3D embedding and, for plane stress, local Newton iteration plus static condensation (see Wrappers). For a linear elastic material the two approaches are mathematically equivalent: both use the same infinitesimal-strain stiffness, so the in-plane stresses agree to within numerical round-off (rtol ≈ 10⁻¹⁰) at any displacement level. The regression test in test/test_dimensionality_wrappers.jl verifies this on a single-element uniaxial load case.

Prefer `Hooke2D` for production 2D linear elasticity

The generic wrappers always run through the nonlinear wrapper path: PlaneStrain(Hooke(...)) and PlaneStress(Hooke(...)) are treated as nonlinear by the assembler, even though the wrapped material is linear. This way, there's no preassembly into K_linear; the PlaneStrain / PlaneStress element routine is evaluated on every Newton iteration, and PlaneStress also solves the local out-of-plane condition. For linear 2D analyses, use Hooke2D directly unless you specifically want to exercise the generic wrapper contract.

Provenance

The 3D Hooke element routine and related documentation are adapted from the Ferrite.jl linear elasticity tutorial [1]. The upstream copyright/license notice is retained in the repository LICENSE. Hooke2D is a package-local model with analytical plane strain and plane stress moduli.

References

[1] Ferrite.jl documentation. Linear elasticity tutorial. https://ferrite-fem.github.io/Ferrite.jl/stable/tutorials/linear_elasticity/