# What Is Nonlinear Geometry In FEA? And When Should You Use It?

FEA models come in all shapes and sizes. While sometimes we’re trying to find the stresses in a stiff, steel structure, others we might be looking at the behavior of a thin membrane or the buckling of a slender column.

You may have heard the term ‘nonlinear geometry’ before, but perhaps are not really sure what it means. This post is aimed at providing a summary of how linear and nonlinear geometry works within FEA, and then some examples and recommendations regarding when you might need to use these settings in your own simulations.

## Linear Geometry

Before we get started with the differentiation between linear and nonlinear geometry, let’s take a short refresher on the way finite element analysis deals with calculating displacement of nodes - the stiffness matrix.

We all remember the equation, *{F} = [K]{u}*, where *F* is the nodal force vector, *K* is the stiffness matrix and *u* is the nodal displacement vector. Well in a typical (linear) FEA model, this stiffness matrix, *K*, is defined at the beginning and it is assumed not to change throughout the entire analysis. That assumption is fine – as long as the change in shape of the things that we’re modeling has no (or minimal) effect on the stiffness of the system during the analysis. This is what we might term ‘small-strain assumptions’.

This might seem concerning to those exposed to the concept for the first time here, because we’re calculating displacements – right? While that is true, in most engineering problems, deformations are so small that the deviation from the initial geometry is essentially imperceptible. The potential errors that are associated with the small-strain assumptions are not significant enough to warrant any extra effort to eradicate.

It’s also worth noting here that all of our old-fashioned hand calculations make use of linear assumptions! That is an important point to remember whenever we’re comparing hand calculations to FEA results.

## Nonlinear geometry

But how about occasions where we cannot make small-strain assumptions? What do we need to do during our analysis to ensure that we capture the effects of shape change on stiffness? Well, it might seem like a somewhat brute force approach, but what we must do is redefine the stiffness matrix after each increment of the analysis. That way the subsequent increment is beginning its calculations with respect to the updated stiffness matrix, rather than the one that was defined at the start of the analysis. As you can imagine, that can become quite computationally expensive, but it is absolutely necessary for a whole myriad of different simulations. Here, we’ve chosen a few of the classics that really drive the point home:

### Bending of Beams

At Fidelis, we’re Abaqus enthusiasts, and so what better place to start than the Abaqus manual. We’ve all calculated the stress and deflection in a cantilever beam. It’s like a rite of passage for any mechanically minded engineer. But remember, those equations make use of linear or small-strain assumptions. If the deflection at the tip is of the beam small, then the FEA analysis of this problem can be considered geometrically linear (how small? Check out the recommendations in the next section). However, if the tip deflects too much, both the stiffness of the structure and the way the load is applied to it has changed significantly, meaning nonlinear geometry is required to produce acceptably accurate results. As the beam deflects, the load applied can be resolved into a component perpendicular to the beam and one along it’s axis. That tension component in the beam would not be observed at all in a linear solution.

### Stretching of Beams

Next, let’s take two beams that are constrained in almost the same way - but not quite. The right end of the top beam is allowed to translate horizontally, while the right end of the bottom beam is not. This might seem like an insignificant difference, and it is if we’re making linear assumptions – both beams will deform in an identical fashion when subjected to the point load.

However, if we were to include the effects of geometric nonlinearity in this model, it becomes quickly apparent that these are not identical load cases. The bottom beam is actually increasing in length (or trying to), and that induces a significant amount of tension. As the tensile force increases, its impact on the transverse displacement at the center of the beam will also increase, causing the results between the two beams to diverge as seen in the schematic below.

### Membranes

In much the same way that the beam in the above example will be affected by the tension induced by geometric nonlinearity, membranes exhibit the same behavior. Imagine the skin of a trampoline. If we were to analyze that using linear assumptions, it would simply bend and we wouldn’t be doing much jumping. In reality, however, as our weight depresses the trampoline, elastic tensile stress (rather than bending) builds up in the thin skin (and the springs) and we are propelled back into the air as it is recovered.

This is illustrated perfectly here, as the figure below shows. On the left (1) we see the correct result for the load, P, when nonlinear geometry is considered in the simulation and on the right (2), the excessive deformation that is predicted when it is not.

## When To Use Nonlinear Geometry

As with much of FEA, there is no hard and fast rule as to when you need to take nonlinear geometry into account. There are, however, a handful of recommendations that we can make, which are reasonably well observed by experienced simulation practitioners:

**Rule 1: Deflection in a beam of more than half the beam’s thickness will tend to require nonlinear geometry****Rule 2: If the deformation anywhere in the model is greater than 1/20th of the assemblies largest dimension, then nonlinear geometry should be considered****Rule 3: If strains are more than 5%, nonlinear geometry is likely required**

But be careful:

It can take significantly longer to solve problems using nonlinear geometry because of the time taken to update the stiffness matrix after every increment

If you want to compare to traditional hand calculations, they are based on linear theory. Hence correlation between hand calculation and nonlinear geometry in the FEA will tend to diverge as deformation increases beyond a certain point

To be safe, it's always a good idea to run some sensitivity studies with nonlinear geometry switched off and switched on. This will allow you to ascertain how important it is to the particular study that you're running. Sanity checks like this will allow you to present results with confidence.

## Final thoughts

If you ever found yourself wondering what nonlinear geometry was and when it might be important, hopefully this post has given you at least some insight. As with all FEA, the results are based on the assumptions that you make when defining the problem - and the more assumptions that you are aware that you’re making, the greater the likelihood that your results will be accurate *enough* to meet your needs.

If you need help with nonlinear simulation, or any other aspect of CAE for that matter, **get in touch with us at Fidelis** and learn how we can revolutionize your design!