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 2 of a 3-part series on common mistakes made in simulation, and how to avoid them. Part 1 can be read here.
3. Incorrect Use of Symmetry
Symmetry can be a powerful way to speed up your analysis, but there are a couple common traps new and even experienced users may fall into.
Symmetry Fixtures
SOLIDWORKS Simulation has a built in Symmetry fixture that makes it easy to enforce a symmetry condition on your model. It even allows viewing symmetric results so you can visualize the results on the full model. To set up a symmetry fixture requires cutting your model in advance and simply applying the symmetry condition to all faces cut by the symmetry plane.
That’s the important part. Unfortunately the built-in graphics preview appears to show the whole part mirrored even if you only select a single face cut by that symmetry plane.
Symmetry fixture as applied to one face (left) and correctly applied to all cut faces (right).
Improper or incomplete application of the symmetry fixture can cause strange responses that are sometimes difficult to catch, so I highly recommend applying the symmetry as the very first step in your simulation setup process so you don’t forget,
Scale Down Forces Proportionally
Any forces or mass loadings applied to faces that are split by the symmetry plane also need to be reduced proportionally (half for half symmetry, quarter for quarter symmetry). Pressure loads are applied over an area, so these won’t need adjusting. If your results are off by a factor of two or four from what you expect, check that the forces were not reduced by the same factor.
2D Simplification
A less common but still prevalent issue concerns the 2D Simplification available in SOLIDWORKS Simulation Professional which allows analyzing a slice of the model. When setting this up, pay attention to the Section Depth specified in the study creation. For plane stress and plane strain simplification, any forces applied (or extracted via result forces) can be thought of as lineal, or force per length of section depth. I recommend setting the section depth to a unit value such as 1 inch or 1 mm to make the mental math easier.
4. Per Face vs Total Force Application
Another category of improper force application can happen when applying force loadings in SOLIDWORKS Simulation. There is a pesky radio button that allows you to select whether the force is applied per face or as a total. With the Per Item selection, the total force would be multiplied by however many faces are selected. If you had five faces selected, you might inadvertently apply five times too much force.
“Per Item” vs “Total” force application.
The “Total” method, as one might expect, distributes the force by the surface area of the selected faces. With that approach the total force is always the same number specified by the user.
5. Units. Units. Units.
Whenever working with engineering calculations, there’s plenty of places to go wrong when it comes to units. Some of the most common tripping points in SOLIDWORKS Simulation specifically are during material definition, any time dealing with pressures (Pascals vs MPa), and torque.
Most common SOLIDWORKS Simulation unit errors.
In the IPS unit system, torque defaults to lbf-inch. This applies to both torque loadings and bolt pre-load, so take care to check whether you need lbf-ft or lbf-inch.
Always keep an eye out for results that seem off by some specific multiplier. Some multipliers I keep in my head: Pascals and megapascals are 1000x apart, lbf-ft rather than lbf-in would be off by a factor of twelve, lbf instead of Newtons would be off by a factor of 4.4.
Remember that perfect integer differences (2x or 4x off) could be due to improperly applied symmetry conditions, or the Per Item vs Total force selection previously detailed.
6. Too Much Bonded Contact
Another way SOLIDWORKS Simulation makes FEA setup easy is by its global contact conditions. Mates and other relations in a SOLIDWORKS assembly are completely irrelevant to the simulation, so all the interactions between components must be defined in the FEA.
The default “global bonded” condition will bond any initially touching faces (within a small user-defined tolerance). Parts that were mated as coincident in the assembly then will be automatically glued together in the simulation. This is great for getting an analysis up and running quickly, but may also contribute added stiffness to the model that can artificially impact the results.
This is especially noticeable in vibration analysis, such as frequency studies or linear dynamics. The example presented below shows a column attached to a baseplate and the first vibration mode calculated for three different bonding scenarios.
Various bonded contact approaches for a column.
The default “global bonded” condition essentially fuses the column to the baseplate over its entire contacting surface area. Compared to studies where the column was bonded at just some or all edges, there’s quite a noticeable spread in the resonant frequency predicted.
It’s best to put consideration into the way components are bonded and make sure it reflects the real-world conditions. For example, if the structure is only welded at a couple edges then it should be bonded as such as in the simulation, or employ other virtual connectors when appropriate.
To investigate the contacts in your model, I highly recommend using the built-in Interaction Viewer which is what produced the contact comparison images above. I rely on Interaction Viewer early on and throughout the process of simulation setup for assemblies.
Sheet metal parts are especially prone to over-bonding, as they are by their nature quite thin, and are often times only connected via small rivets, spot welds or edge welds. Bonding large regions of sheet metal parts together will dramatically and artificially increase their stiffness, affecting both vibrational and stress/displacement results.
7. Using the Wrong Mesh Elements
Shell Mesh
For geometries featuring sheet metal and other thin-walled parts such as thin wall tubing or composites such as fiberglass, including circuit boards, it can be practically impossible to achieve a good level of mesh refinement using the default solid mesh type. For these geometries, it’s almost always best to take advantage of shell elements which better represent the part as an infinitely thin surface and assigns the thickness as a parameter.
Aside from drastically speeding the solve time and enhancing solution accuracy, this also allows for quick iteration of wall thicknesses within the study without having to update the underlying geometry.
For sheet metal specifically, it shouldn’t require any extra setup definition in the simulation. Parts created with the built-in SOLIDWORKS Sheet Metal tools automatically convert to a shell mesh definition in SOLIDWORKS Simulation. For imported geometries or parts modeled with regular SOLIDWORKS features, the conversion process would be manual by either Defining Shell by Selected Faces or extracting a surface body in SOLIDWORKS.
Shell mesh definitions.
For extremely complex models that feature hundreds of sheet metal bodies, or bodies that have dense features such as perforations, the automatic conversion of sheet metal parts to bodies can become a bottleneck as the program can get hung up during mesh creation. For these cases, I often recommend enabling the option to “Treat all bodies as solids” and use the manual techniques outlined above to convert the sheet metal parts back to shells. Though this process is manual, it almost completely eliminates getting hung up during the automatic shell extraction.
Linear (Draft) Mesh
Draft quality mesh is a dangerous feature. The linear tetrahedral and triangle elements are known to underpredict both stiffness and stress, even with fairly high levels of refinement. It can be very useful to use the Draft Quality option while initially setting up your study to confirm that the loads and fixtures as well as the overall response appears as you expect, but once you are ready to interpret stresses and displacements you should switch to the High Quality (second order or parabolic) mesh definition.
Newer versions of SOLIDWORKS Simulation support mixing draft and high quality elements, so clever uses of draft quality mesh can be acceptable for specific cases when you’re confident it won’t affect the overall load path and the draft quality region is away from the area of interest.
Stay tuned for Part 3 of this series.
Part 1 can be read here: Top Setup Mistakes in SOLIDWORKS Simulation, Part 1.