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 is part 3 of a 3-part series on common mistakes made in simulation, and how to avoid them. Part 1 is here and Part 2 is here.
8. Not Performing Mesh Refinement
Given how frequently the topic comes up in FEA literature and as an early topic in training courses, you may be surprised to find “mesh refinement” so far down the list of top FEA mistakes. I placed it here because SOLIDWORKS Simulation has fairly robust default mesh settings that, in general, tend to deliver solutions that are in the right ballpark for the overall response of the structure. If your intent is just to compare general design trends, the default settings are often adequate.
The other reason it is placed so far down this list is that I frequently see users going too far in the opposite direction – creating analyses on relatively simple parts or creating models with millions of elements (and dealing with excruciatingly long solve times) out of concern that their solution needs to be accurate.
Meshing or the discretization of the model, and mesh size are certainly important parts of any numerical simulation. Care must be taken to conduct meshing in a reasonable manner and only once the fundamentals of the simulation setup (loads, fixtures, contacts, load path and overall response) have been proven accurate.
Thankfully, there are tools within SOLIDWORKS Simulation to help you determine where mesh refinement is required and an appropriate mesh size.
Adaptive Mesh Refinement
You can, of course, manually refine the mesh by adjusting the mesh settings globally or placing mesh controls. If you aren’t sure where to start, enabling adaptive mesh refinement by editing the study properties will allow SOLIDWORKS Simulation to refine the mesh for you.
Adaptive refinement solver options.
The h-adaptive method works by reducing the element size in regions with high errors, while the p-adaptive works by raising the order of the elements. I tend to recommend h-adaptive for most applications as it is the most intuitive and will allow the user to see where the additional refinement was placed.
Von Mises stress before and after adaptive refinement.
For the example above, observe the stress pattern on the part before refinement. Even without the underlying mesh displayed, the “splotchy” contours are a great visual indicator that the mesh is inadequate. Post-refinement, the contours are smooth and continuous.
Though smooth and continuous contours don’t prove much on their own and should not replace a mesh-convergence exercise, it’s great to train yourself to look out for the red flag of “splotchiness” as a warning that stress results may be underpredicted unless further mesh refinement is performed.
Note that the adaptive mesh refinement listed above is only available with certain limitations: they don’t work for “mixed mesh” studies and are only available in linear static and drop test study types.
Energy Norm Error (ERR) Plots
Wouldn’t it be great if there was some way SOLIDWORKS could tell us in a plot where additional mesh refinement is needed? Well, there is. And it relies on the same type of logic that the adaptive refinement above utilized.
Creating or editing a stress plot allows changing its component to “ERR: Energy Norm Error” which will create a plot that allows visualizing the magnitude of any stress discontinuity between elements.
Inserting an ERR Plot.
Applied to our same example before and after the adaptive mesh refinement, it can be seen how the adaptive refinement focused on placing additional elements into the areas of highest energy norm error. To utilize the plot most effectively, I’d recommend setting the maximum value of the legend to a reasonable target and observing the red values as areas to refine.
Energy norm error before and after adaptive refinement.
Note that the “error” here is not necessarily proportional to the percent difference you’ll observe in stress results from performing the refinement. The help files state that, “If the mesh is fine enough such that two neighboring elements have perfectly continuous stress contours, the stress error at each node would be zero.”
It would be impractical to achieve near-zero energy norm error – reasonable targets I’ve seen for high accuracy results are to maintain < 5% energy norm error in the areas of interest and for first pass results I may use a value of 10-20% as a crude target.
I’d encourage you to still go through the process of performance mesh convergence studies, where the mesh is refined iteratively until the solution converges. Comparing the converged mesh refinement versus the corresponding energy norm error should be the best way to prove out the threshold that could be used as a guideline on your geometries.
9. Not Being Conscious of Assumptions
Understanding the assumptions of the simulation study are crucial and I think most users are aware of factors such as that a linear static study uses materials that must behave in an elastic manner, meaning it neglects any plastic deformation and can only be relied on to predict the onset of yielding.
But I run into many users who have not fully internalized the assumption that the entire system responds linearly, for example, that doubling the input load exactly doubles the displacements and stresses.
Linear response assumption.
For a typical linear static study with the small displacement assumption, the response will really be one-to-one correlated. The “factor of safety” calculation is also based on this linear relationship – it informs us that if we apply a 100 lbf load and have a factor of safety of four, a 400 lbf load will put the material at its limit.
If you have reason to believe your structure or system may behave in a nonlinear manner, then these physics should be incorporated. Geometrically nonlinear problems may involve large displacements or membrane stiffness effects and can be captured by enabling the large displacement option within a linear static study or creating a dedicated nonlinear study. As soon as non-linear factors come into play, the linear response relationship is no longer guaranteed and behavior may deviate drastically. The same goes for incorporating nonlinear material models.
Another major assumption common to any static study is that the loads should be applied gradually. This is because inertial effects are not represented in these study types. If your loading is actually a shock loading applied over a very short time period, you need to either build in additional safety factor (if there is a known dynamic amplification factor for your application) or perform an appropriate dynamic study.
Linear dynamics studies allow definition of f(t) curves for shock loadings and other effects and will calculate any amplification of the response as an output but still rely on small displacement assumptions and a linear system response. Nonlinear dynamic studies allow removal of both major assumptions and can capture events incorporating both large displacements/nonlinear response and inertial effects — but at the cost of computational expense.
10. Improper Treatment of Singularities
Singularities can be a pesky issue for anyone performing finite element analysis. They may often occur at geometry features such as sharp re-entrant corners or near fixtures (like the “fixed geometry” example previously detailed) or rigid connectors.
A singularity is a mathematical artifact that, rather than converging with subsequent rounds of mesh refinement, actually diverges. As the mesh is refined, the stress results at the singularity will approach infinity.
SOLIDWORKS Simulation has tools like the Stress Hot Spot Diagnostics that can help a user identify if a high stress region is due to a singularity or due to valid stresses in the region. Valid stresses may be relied on for Factor of Safety and failure prediction, while singular stresses would require special treatment.
Stress hot spot diagnostics for singularity detection.
An increasingly disturbing trend I see among users is to “ignore” singular stresses all together – writing off the high stresses as irrelevant. This practice may be acceptable when it’s known that the real-world stresses are low in that region but as a general habit it is a serious issue, as any part with a sharp notch may have significant real-world stress concentrations that can lead to failure or fatigue damage.
One common method to eliminate a singularity in a stress analysis would be to apply a radius (even a very small one) to the area in question for a sharp re-entrant corner. Alternatively, performing a nonlinear analysis with an elastic-plastic material model should allow the material to yield locally in the singularity region and redistribute stresses accordingly. Refining the mesh in the region of the singularity will “confine” the singularity to a smaller and smaller region, allowing interpretation of converged stresses a couple of elements away. For certain applications like pressure vessels, stress linearization may be performed.
If the singularity is from a load, fixture or connector, there may be alternate setup approaches that alleviate it. For example, with bolts, pins and remote loads, the “distributed” connection type in SOLIDWORKS Simulation helps mitigate any localized singularities that may occur with a “rigid” connection.
If none of these approaches to addressing the singularity are possible due to time constraints or other factors, I would at least suggest a shift in mindset to treat a singular region as a “potential area of concern” rather than writing it off altogether. It’s also very useful when dealing with singularities to scale the stress plot to your design stress limit, rather than rely on the automatically calculated maximums. And recall that, though the numerical artifact of singularities impacts derived values such as stress in the local area, it should not affect the convergence of displacements or reaction forces or stresses that are distant from the singularity region.
11. Not Doing a Sanity Check
It’s a great idea to do some form of sanity check for any simulation result. This can take the form of a comparison to test data for similar products or hand calculations.
Built-in Verification Problems & Benchmarks
If you’re not sure where to start to validate a finite element analysis, I’d encourage working through the built-in validation examples and NAFEMS benchmarks. These are accessible under the help menu (question mark icon in newer version of SOLIDWORKS) under Help > SOLIDWORKS Simulation > Validation > Verification Problems.
Built-in verification problems.
These verification problems include a pre-defined model with simulation study and associated comparisons against the analytical solution. NAFEMS is an industry body dedicated to engineering, modeling, analysis and simulation and publishes benchmarks that allow direct comparison between various FEA and CFD packages, Also, by reviewing the NAFEMS benchmarks, you can compare the accuracy of SOLIDWORKS Simulation to other leading simulation tools.
Extract Reaction Forces
Reaction forces can be extracted by right clicking the Results folder and choosing to Extract Result Force to measure the reaction forces at the fixtures of the structure and compare against a free body diagram. When extracting these, it’s crucial to make the same geometry selection as the fixture. For example, if the fixture was defined on a set of faces, choose those same faces for the reaction force. Selecting some partial entity (such as an edge belonging to a face) will result in only a partial reaction force displayed.
Extracting reaction forces.
Note that the statics calculations for an FBD generally assume rigid bodies, so some differences may be expected due to the elasticity in the FEA model.
Analytical Calculation Assumptions
While comparing against hand calculations can be very useful to make sure your result is in the right “ballpark,” do take care to consider the assumptions associated with any hand calculations.
Some examples to consider:
- Reaction force from a statics calculation/free body diagram relies on rigid body assumptions while FEA incorporates elasticity.
- Stress concentration factors for a hole in a plate that assumes an infinitely thin, infinitely large plate while the FEA model has a finite thickness and span.
- Euler beam bending calculations are assumed to be valid only for long slender beams and only under small deformations.
These differences in assumptions can lead to variance between the analytical solution predicted and the finite element analysis results that could range from mild to severe. Understanding the assumptions of the analytical calculations will help you determine how much deviation would be expected.
Summary & Conclusion
Hopefully this series of articles has helped you understand the current state of finite element analysis (FEA) tools such as SOLIDWORKS Simulation, and provided tips for setting up an analysis, whether simple or complex, and how to avoid common traps that can impact the validity of results.
It’s hard to go wrong with your simulation setup if you pick a reasonable level of simplification for your model, avoid going overboard with the “fixed geometry” fixture on large faces or spans, put consideration into the contact interactions in your assembly, are conscious of the assumptions of your analysis and do a sanity check by extracting reaction forces and/or comparing results against analytical calculations.
Lastly, if you aren’t sure if you should make a certain assumption, use a certain approach or just how to proceed in general – I’d suggest either combing for research papers (Google Scholar is a valuable tool) of similar analyses conducted in the past, or reaching out to your colleagues or software vendor for further assistance.
Part 1 of this series can be read here: Top Setup Mistakes in SOLIDWORKS Simulation, Part 1.
Part 2 can be read here: Top Setup Mistakes in SOLIDWORKS Simulation, Part 2.