What is the meaning of distortion in region outside of stressed geometry using FEA?

Question

In FEA simulation of simple beams (3D solid and shell/plate), I have taken a simple geometry:

• A long beam in the y direction
• a concentrated load applied on the plane of symmetry

• There is a pin or roller joint at some point between the symmetry plane and end of the beam:

                        load
  a       b            c↓
  ======================⌇  y-symmetry
          ▲              
  free    pin
  

In this system, when we solve with the typical beam equation, we assume that the angle of deflection is small. In that case, we see a slight axial distortion between the pin and free end because the total deflection is very small.

However, when we solve this with 3D FEA elements, I would expect the length of the beam from a-b to be conserved. In my understanding, I expect the the shear and moment on elements beyond the joint to be zero. However, in practice I have seen beams with finite-thickness-shell elements and 1 and 2 element thick solid plate (cannot go thicker because of software limitations) meshes result in extreme axial distortions of this region when the load is large.

Is the mesh distortion here unphysical? What is the cause of this behavior? What are some ways to reduce or eliminate this behavior?

Should I simply not include this region in a simulation? If so, what are some guidelines or considerations for deciding what regions to expect such behavior in order to eliminate/reduce it?

Answer 1

Concentrated forces and constraints are per se unphysical: have you never seen a force acting on a true geometrical point? And a point-wise roller?

Whenever you use beam theory (whether Euler-Bernoulli or Timoschenko) you should ask yourself about its hypothesis and how the theory maps to real world beams. The same holds true for Continuum Mechanics and shell theories.

This said in beam theory all internal forces are vanishing in $ab$ which is subject only to rigid body motion, as outlined by Bill in his answer. Please note that under the small deflection assumption this means linear transversal displacement. (Of course this is not a true rigid body motion if finite displacement are assumed: is this the origin of your supposed axial deformation?)

For 3D continuum elements, concentrated loads and constraints can be modelled as nodal forces or constraints. Note however that, in continuum mechanics, solutions are singular under concentrated forces (e.g. Kelvin solution). This means that near the nodal loads and constraints great element distortion and no point-wise convergence is to be expected. Furthermore, due to numerical problems like hourglassing, a catastrophic breakdown of the solution can occur even far away from the concentrated load.

From the engineering point of view, beam models and concentrated forces are OK, provided you understand what they really mean. According to de Saint Venant principle, you can assume that far away from a loaded region, only the load resultant influences the solution, and not the actual load distribution.

If you experience stresses and deformations in $ab$ I would tentatively suppose that

1. the beam is not slender enough to apply the de Saint Venant principle, or

2. numerical problems (like hourglassing for reduced integration elements) are affecting your results.

Answer 2

In this system, when we solve with the typical beam equation,

Let's first consider the results from the beam equation-- whether you solve it analytically or by FEA. Beam theory says that the axial deformation is zero along the beam centerline (neutral axis)-- both to the left and the right of the pin. At locations away from the centerline (e.g. the outer fibers of the beam), you can easily calculate the axial deformation from the first derivative of the transverse deformation.

As you observe, there is no bending moment or shear force to the left of the pin. The transverse deformation there is basically a rigid-body rotation due to the rotation of the beam cross section at the pin. This deformation is something you would certainly see in an experiment.

The situation is slightly more complex in 3D and depends on how you model the pin in your FEA model. In the vicinity of the pin, there will be a 3D stress state; for example, there will be stresses to the left of the pin. At locations away from the pin and as you make the beam more slender, the solution will agree more closely with beam theory.