Correctly setting boundary condition for periodic linear elasticity problem

Question

From an old, wise engineering book Peterson's Stress Concentration Factors (http://eu.wiley.com/WileyCDA/WileyTitle/productCd-0470048247.html page 324) I've got the following problem:

There is 2D infinite periodic structure with round holes of radius r with tension applied to it. The relation of maximum stress in the body to the applied one should follow nice 1/x like curve, see the picture. While I'm trying to reproduce this example by numerical simulations, I'm getting that max stress is almost independent of hole size.

I use displacement based weak formulation for elasticity with periodic boundary conditions remaping top to bottom and left to right, with exception of corners (0,0), (0,1), (1,0), (1,1). For problem to be well-posed I've fixed displacement vector in one point (0,0) to be equal (0,0). Am I right? Is fixing one point enough? I still can rotate the unit square though. Do I need to fix an additional point?

The tension is applied via Neumann boundary conditions with tension applied in the following way. First, I define vector $g = (1.0, 0)$ and then I create right hand side for the weak form of equation: $$ \int C\varepsilon(u):\varepsilon(v)dx = \int_{left border} (-g,v)ds + \int_{right border} (g,v)ds, $$ where the differential operator $\varepsilon$ is the symmetric part of the gradient and $v$ is a test function obeying periodic boundary conditions. This is the place I'm most doubted about applying tension correctly. Is it correct? Is my problem well-posed?

p.s. I'm solving it with Fenics and code can be found here https://fenicsproject.org/qa/13464/verifying-elasticity-benchmark-structure-boundary-conditions

Answer 1

Here is a description of a small FE model that might approximate the case of an infinite number of holes in an infinite plate.

Create a model of a single repeating element with $1/4$ of a hole centered at $x=0, y=0$. Along the boundaries at $x=0$ and $y=0$ apply classical symmetry boundary conditions.

On the two remaining edges, apply constraints on the displacements simply to keep the edges straight and parallel to either the x-axis or y-axis, as appropriate. In other words, all nodes along the boundary $x=l/2$ would have the same $u$ displacement and all nodes along the boundary $y=l/2$ would have the same $v$ displacement. This type of boundary condition is often referred to as an MPC (multi-point constraint) (e.g. NASTRAN, ABAQUS).

Either or both of these edges would also have an applied stress loading normal to the edge of $\sigma_1$ or $\sigma_2$.

The idea is that the straight-edge constraints would enforce compatibility with the adjoining cells but not restrict the motion unnecessarily.

Answer 2

As a first approach, you could do as @BillGreene suggests, that is increase the size of your model, increasing the number of cells each time. I guess that around 10 cells in each direction you should have a value that won't change much for further increasing.

Another option is to constrain the displacements at opposite sides of the cell, for example, in the horizontal direction, you would have

$$u(\text{left}, y) = u(\text{right}, y) + g(y)\, ,$$

a common choice is to have $g(y) = u_0$, constant.

If you combine both approaches, you would have better results, I guess.