To satisfy basic design criteria or make conservative estimations about the ultimate strength of a given structure, it’s common practice to do some basic hand calculations or Finite Element Analysis (FEA).
However, what if you wanted to know:
- That your design is strong and optimized?
- That the product has extra endurance when the applied load exceeds the design limit?
- What’s going to happen under the ultimate load?
In this post you will gain insights into the main areas of FEA, including:
An overview of the three FEA types – static linear, static nonlinear and explicit
Results achieved by static linear, static nonlinear and explicit FEA
Benefits and limitations of static linear, static nonlinear and explicit FEA
A practical discussion about application of static linear, static nonlinear and explicit FEA
The limitations of traditional stress testing
Standard methods of stress hand calculations work fine for a number of basic designs. They help to minimize risks of failure while working under the design load. However, how would the structure work in extreme situations that are not explicitly anticipated by the design?
What if you don’t want to guess, but know precisely when and how your design will collapse?
A traditional way to answer this question would be to build several prototypes and individually stress test them. But we all know that prototyping and physical testing is expensive, thus we need to avoid it as much as possible.
FEA provides unique advantages for today’s designers & engineers
An alternative to conventional stress testing is FEA, which offers a unique way to understand your design and simulate stress testing for real world situations. Using Autodesk Inventor Nastran software, we virtually test our product and expose it to numerous stress testing scenarios.
In the following example I will show you how to use:
- Static linear analysis to determine maximum design load
- Static nonlinear to find out the moment before the product breaks
- Explicit analysis to confirm the maximum load and demonstrate failure mode
This example is based on a hypothetical tow bar model which is an assembly of components welded together.
Material: steel AISI 1006 with following mechanical properties:
- Tensile Strength, Ultimate – 330MPa (47.9ksi)
- Tensile Strength, Yield – 285MPa (41.3ksi)
- Elongation at Break – 20%
- Modulus of Elasticity – 206GPa (29,900ksi)
- Poisson’s Ratio – 0.29
As you can see, the tow bar is made of relatively thin rectangular tubes. Therefore, shell elements work best for this type of analysis.
To demonstrate the difference between shell and solid elements, I have conducted a number of experiments – read Shell vs Solid Elements: Are They Similar?
Disclaimer: The model is built for the demonstration purpose only, with no intent to confirm that the design meets any industry standards. Also, detailed weld analysis is not in scope for this article.
This is a great tool to get a quick answer to the common question “Is my design strong enough?”
Because the finite element model works only for small deformations and does not simulate material plasticity, the results are relevant only if stress does not exceed material Yield value.
Therefore, using static linear analysis it is easy to determine the maximum load before plastic deformations appear. This will give a very rough understanding of the failure mode.
As a starting point, I applied 5kN (1,124 lbf) and found that there is a small spot at the corner of the safety chain ring where von Mises stress exceeds the Yield. However, the chain ring modelled uses shell elements. These elements have virtual thickness that defines their stiffness, but their actual thickness is zero.
As a result, the chain ring acts like a knife and provides an unrealistic stress concentrator at a corner. In real life, the same load is distributed across a wider area due to material thickness and welds. So, it is reasonable to ignore results directly in the hot-spot and measure stress at a distance = ½ material thickness.
The maximum stress (½ material thickness away from the stress concentrator) is 240MPa. This gives a safety factor equal to 1.18 which is Yield Stress / Maximum Stress. In other words, the margin of safety is 0.18 or 18%.
What can we tell based on the static linear analysis above?
- Taking a conservative approach, 5kN appears to be the maximum design load to stay under the Yield limit for the chosen material.
- Average maximum stress (away from the hot spot) in the tube is around 150MPa. This is much lower than material Yield value.
- It is not possible to correctly predict the ultimate load that the design can withstand using static linear analysis.
In practice it is common to ensure that a product won’t immediately collapse if the applied load significantly exceeds the design limit – for example, in the case of a road accident.
Static nonlinear analysis helps to confirm this, taking us to the next level of modelling by determining the ultimate load that should be applied to break the structure.
In the chosen example the material elongation at break is 20%. This means that we can expect quite significant plastic deformations before the tow bar breaks.
In Autodesk Inventor Nastran there is a material model which works well for most ductile materials like steel – Elasto-Plastic (Bi-Linear).
Applying Enforced Motion
Instead of guessing the ultimate load, I applied Enforced Motion and calculated the reaction force. The primary benefit of this approach is that it minimizes challenges with nonlinear analysis convergence.
Enforced motion is the same approach as used by the stress test machine, where the structure is deformed by X mm to find out its reaction force and material strain. In this model I literally pulled the tow bar by 100mm to see what the result would be.
To better understand the model behavior and prepare accurate Strain-Displacement and Force-Displacement charts I set the result save interval to 1% of the load. So, it gave me loading history with 100 result sets (see video recording).
In addition to the examination of stress plots, I extracted Strain-Displacement and Force-Displacement data from Autodesk Inventor Nastran’s plot tool. Usually, it’s quick and simple to use Inventor Nastran’s built-in graphs for strain and force. But sometimes I prefer to export result values and create charts in MS Excel.
Discovering breaking point
In order to determine a moment when the material starts to break, I extracted Maximum Effective Strain Plastic data from 4 points around the chain ring corner. Then using a MAX function in Excel I created a summary chart and determined a load step when it reaches the material elongation limit (0.2).
As a result we see that the material limit was reached at 45mm displacement. Then using a Force-Displacement chart we can find that the Reaction force at the same moment is approximately 18kN.
Static nonlinear analysis shows that the tow bar breaks at much higher than the design load (18kN vs 5kN). This is a significant insight into design strength that is possible due to allowed large plastic deformations.
Using static nonlinear analysis, we successfully identified a moment when material failure starts to occur. However, it still doesn’t give us an answer to the question: what is the failure mode? Explicit analysis is a way to identify failure mode.
Often explicit analysis is associated with fast dynamic simulations such as impact analysis – for example, car collision. But it is a good alternative to typical static nonlinear analysis that simulates complex contact problems, large deformations, or structural collapse.
Adding element deletion criteria
Explicit analysis also uses large deformations and nonlinear material properties. But in addition to that it is possible to add element deletion criteria. In other words, explicit analysis allows us to switch elements off once they reach ultimate elongation.
By using explicit analysis, it is possible to:
- Identify failure mode. In the tow bar model we can see that a crack – which leads to the structural collapse – begins from the corner of the safety chain plate.
- Identify the maximum load the design can withstand. This process is similar to the one used for static nonlinear analysis – using loading history we can see when force reaches the maximum.
Comparing Reaction Force charts
It is possible for us to see that the explicit and static nonlinear analyses provide nearly identical results. Explicit analysis shows that structural collapse begins at around 55mm displacement, keeping the maximum load at the same 18kN mark.
Factoring in solution time
Finally, another thing to consider is solution time. For example, on my 3.5 GHz, 6-core i7 comparable size, explicit and nonlinear models with contacts and large deformations on average take the same time to solve.
However, using a powerful CPU with a higher number of cores it could take much less time to solve explicit then nonlinear, because not all stages of the nonlinear analysis are highly parallel.
As we have seen from the above examples and explanations, the application of FEA in your own practice provides significant benefits. It’s no longer necessary to guess design strength, run expensive and time-consuming crash tests or use conservative empirical methods of hand calculations.
Knowing and applying FEA types and their basic principles can help engineers working in any field to make confident decisions about their designs.
Autodesk Inventor Nastran is an intuitive and powerful software that helps users find answers to different engineering questions. Being a part of the Product Design Collection, it allows you to quickly optimise your design and achieve reliable results
The next steps in your FEA journey
- Would you like to learn practical FEA and start confidently using it in your everyday work?
- Are you looking for a highly accessible and practical FEA course where you can build finite element models from scratch?
- Do you want to learn a range of FEA tricks and time-saving tools for your own designs?
Please get in touch
I would love to hear more about your current design challenges and help you understand how FEA could benefit your work. Feel free to contact me – firstname.lastname@example.org