In my time using finite element analysis software like SOLIDWORKS Simulation and SIMULIA Abaqus/CAE, I’ve seen many of the same mistakes being repeated by users at various skill levels. This article will outline some of the most common traps and basic steps to avoid them. It will focus primarily on SOLIDWORKS Simulation but should also apply to other finite element analysis software.

CAD/FEA integration makes it easy to apply some loadings and generate displacement, stresses and strains — as well as get results with a reasonable level of accuracy — as long as you avoid these common pitfalls.

## 1. Model is Overly Complex

Much of my time assisting engineers with their FEA setup is spent trying to convince them to reduce the complexity of their FEA models. Rapid advances in consumer hardware (notably the increased RAM capacity and number of CPU cores) have made it possible to analyze problems with tens of millions of elements on consumer hardware — but that doesn’t mean you should.

All too often users reach out to us for help when they have already been struggling painfully for too long on an extraordinarily complex model. It’s worth thinking long and hard upfront to develop a plan for the analysis that defines regions of interest. Then the setup of the simulation can be tailored to focus on these areas, minimizing refinement in other regions or excluding parts that have no effect.

*Figure 1. Comparing various simulation setup approaches.*

Through careful consideration, it’s possible to reduce millions of degrees of freedom in a model by orders of magnitude. Similarly, the amount of contact interactions can often be reduced to only the most critical areas. Combined, these changes can reduce solve time from hours/days to just a few minutes.

If it’s unclear whether it’s safe to perform certain simplifications to a model, virtual A/B comparison tests or sensitivity analysis via a Design Study can reveal the impact of any additional assumptions or adjustments.

If you’ve gone through the exercise above and determined that your problem can’t be simplified any further and it’s still quite complex, you still don’t want to dive headfirst into the simulation setup.

Before setting up a complex FEA, you should make the most basic and crude model, minimizing the level of complexity, and then use this as a baseline to progressively add more detail to the analysis. Most often this means starting off by suppressing or excluding all but a handful of the most critical structural components, using only bonded contact interactions and applying a simple gravity load or other arbitrary loading to the study.

Once the response of the structure matches intuitive expectations under the simplified conditions, gradually start including more complexity such as bolted connections with contact and periodically run the analysis.

It’s much easier to diagnose a misstep this way, rather than trying to determine why an assembly analysis with hundreds of parts (that you spent days or weeks setting up) doesn’t work.

*Figure 2. Dedicated simulation model for gantry crane.*

On one extreme, it may be worth building a dedicated model just for simulation purposes. I find this especially useful for models featuring a large number of thin or sheet metal bodies that will be represented with shell elements. Using techniques like in-context assembly editing in SOLIDWORKS, you can ensure that a dedicated simulation model stays associatively linked to the original CAD source files.

For exploring techniques like these further, I’d recommend reading through the article Large Assembly Analysis with SOLIDWORKS Simulation.

## 2. Improper Fixtures

It’s probably no surprise for experienced users that improper constraints can lead to invalid results, but new users often don’t understand the ramifications of their fixture selection. While the SOLIDWORKS Simulation interface makes it easy to apply pre-defined fixtures (such as Fixed Geometry and Roller Slider) it can also obfuscate which degrees of freedom are being removed under the hood. Restraining more degrees of freedom compared to the real-world results in over-constraining the model, effectively increasing the stiffness of the part and artificially affecting the response.

### Fixed Geometry

The most egregious of all offending fixtures, Fixed Geometry, has been responsible for more wildly inaccurate simulations than I can count. Fixed geometry totally restrains the selected geometry from all translations and rotations. Consider that if a large flat face is selected, all the elements on that face will be unable to translate in the X, Y or Z directions or rotate about any axis.

By applying fixed geometry, the faces are defined as perfectly rigid regardless of the load and cannot deform. Think about that — no matter how extreme a loading is applied, these fixed faces will notdeform and in many cases, will have no detectable stress.

Users new to FEA have a hard time fully accepting this given how often we see fixed (AKA clamped) geometry or parts depicted. By far the most important takeaway from this series should be to avoid haphazardly applying fixed geometry constraints to large surfaces and spans. If nothing else, be conscious of the fixture selection and document the assumption.

The fixed geometry fixture can cause all sorts of problems even on the simplest examples. One problem is due to Poisson’s ratio. Even the simple case of a test specimen in axial tension may show artificially high stresses near the fixture. If you’re willing to ignore the stresses local at the fixture because your area of interest is sufficiently far enough away, then it’s not much of a problem. Still, there are better methods available.

*Figure 3. Fixed geometry vs roller/slider fixture for a bar under tension.*

An alternate fixture scheme, such as the Roller/Slider fixture, locks translation in the in-plane direction and doesn’t produce these kinds of artificial stresses. For the example above, the Roller/Slider fixture isn’t enough to fully constrain the model, however. While in theory it should fully balance the applied force, FEA solvers such as those in SOLIDWORKS Simulation sometimes complain when there are remaining degrees of freedom.

Even the slightest imbalance (due even to numerical noise in the solver) may cause the part to translate through space and yield artificially high displacements or a “model is unstable” warning.

Solver options such as enabling soft springs or inertial relief can counteract this. Or, clever usage of fixtures such as the Reference Geometry fixture in SOLIDWORKS Simulation to constrain a single vertex in the X direction and another vertex in the Y direction can remove the possibility for these rigid body movements.

Whatever way you choose to stabilize the model, it’s important to verify after the fact that these additional “helper” fixtures or stabilization methods such as soft springs/inertial relief are not carrying more than the expected (near zero) load.

### Roller Slider

We just discussed how the Roller/Slider fixture can be an improvement for restraining large surfaces, but it contains another common trap many users fall into: the Roller/Slider fixture locks all the translations through the plane and doesn’t allow the geometry to pull away no matter how much force is applied.

*Figure 4. Roller slider fixture preview tooltip – the source of much confusion.*

If you require a fixture that doesn’t allow the part surface to cross through some plane but will also still be allowed to separate, then you should instead look at the Virtual Wall contact condition. This allows specifying contact to some imaginary virtual wall defined by a plane and is suitable for cases such as a machine sitting on a floor or a simplified representation of a bolted joint using Foundation Bolt virtual connectors.

*Figure 5. Roller/slider fixture (left) vs virtual wall (right) with 100x deformation.*

In the example above, the response with a Roller/Slider fixture is compared against a setup with the Virtual Wall and virtual bolts. The deformation scale is amplified so the differences can be seen – note how the virtual wall solution allows the back of the bracket to deform, which yields very different patterns in both displacement and stress.

Generally, the Virtual Wall and other sliding contact conditions are not available in modal analysis such as buckling, frequency and linear dynamics so in these cases you would need to fall back to other fixture schemes.

*Stay tuned for the next article in this series on SOLIDWORKS Simulation.*