Nonlinear Analysis in SOLIDWORKS Simulation
This article presents three use cases for nonlinear static analysis in SOLIDWORKS Simulation Premium through examples. Tips for getting started and sourcing material data are also included.
Example 1: Loadings Past Yield Stress
Loadings past the yield strength of a material may be the stereotypical application that comes to mind for nonlinear analysis. In certain industries and testing standards, it is acceptable for a part to undergo permanent deformations under overload conditions so long as the part continues to function and avoids catastrophic failure.
Consider the case of an alloy steel arm subject to a proof load of two tons representing an overload scenario.
Figure 1: Alloy steel arm mesh and loading.
Linear material models (the only option in a SOLIDWORKS Simulation Static analysis) only have a single stiffness parameter: elastic modulus, which represents the slope of the stress-strain curve within the linear region. Nonlinear study types available in SOLIDWORKS Simulation Premium can utilize plasticity material models, which contain extra information to describe post-yield changes in stiffness.
Figure 2: Example stress-strain curve (left), bilinear approximation (right).
Ideally, a stress-strain curve obtained from tensile test of the material would be input for most accurate plasticity model definition.
Alternatively, a parameter called tangent modulus can be added to approximate the slope of the stress-strain curve post-yield. Together with the elastic modulus and yield strength, this creates a bilinear material model as visible in Figure 2 above.
Figure 3: Linear material model (top) vs plasticity-Von Mises model (bottom).
Two simulation results from studies with identical setup and plot scales are visible in Figure 3 above. The top result utilizes a linear material model for alloy steel, and the bottom with a plasticity model driven by stress-strain curve. The linear material model predicts stresses approaching the ultimate strength of the material. The nonlinear material model shows substantially reduced peak stress values—only slightly above yield strength. How is such a difference possible?
As the material begins to enter the plastic region, its stiffness rapidly drops. This leads to a redistribution of stresses to surrounding material.
Strain plots in nonlinear studies are a valuable tool and allow displaying elastic or plastic strain. Plastic strain plots are useful to visualize regions of the model which have undergone permanent deformation, as seen in Figure 4 below.
Figure 4: Plastic strain plot.
These yielded regions have produced a redistribution of the locally high stresses around these fillets.
For these reasons, linear material models are generally an inaccurate predictor of stresses above yield. The only conclusion that can be drawn from stresses above yield in a linear static study is often that “yielding is likely to occur”—the values reported over yield must not be relied upon without first investigating a plasticity model in a nonlinear study.
It’s worth noting that finite element models in nonlinear studies will show distorted shapes but never damage like ruptures, cracks or tears. Predicting that kind of damage with SOLIDWORKS Simulation requires careful engineering determinations based on approaches such as comparing relevant stresses to the ultimate strength of material or observing strains.
If desirable, applied loads can be removed at the end of a nonlinear study to output residual stresses and deformations in an unloaded state.
Example 2: Snap Fit Connector
Design of snap fit connectors or clips are another great potential application for nonlinear analysis. In this example, a snap fit connector is pushed into the corresponding boss, and then pulled back out.
Quarter symmetry is employed to speed up solution time and provide a convenient cross-sectional view. Parameters of interest may include peak stresses in the snap fit connector and the insertion and pull-out forces required (if the clip is removable).
Figure 5: Nonlinear static stress results for a snap fit connector.
These studies are impractical in a linear static analysis due to changing contact conditions, and the desire to extract values over multiple load steps. As the linear static study solves in a single load application “step,” it is impossible to extract any time history.
Nonlinear static analyses (despite the name “static”) increment loadings using a parameter called time. However, dynamic effects such as inertia and damping are not taken into account in a nonlinear static analysis—such effects are incorporated in a nonlinear dynamics analysis if deemed necessary. Time in a nonlinear static analysis is sometimes referred to as pseudo-time to help reinforce this distinction.
This time parameter allows sequencing loadings that are not highly dynamic in nature and observing behavior at various steps. It is also the underlying mechanism that accounts for being able to solve large displacements, plastic deformation and other effects by incrementing load application and re-solving the stiffness matrix at each time step.
The loading in this example is a prescribed displacement on the top face of the male component, as visible in figure 6 below.
Figure 6: Prescribed displacement with corresponding time curve.
The loading is sequenced by ramping up the desired displacement amount from t = 0 to t = 0.5 seconds. From t = 0.5 seconds to t = 1, the displacement is reversed to pull back to its starting position. If desired, multiple loads/displacements may be varied or turned on and off during a study to represent different effects.
The default end time for a nonlinear static analysis is 1 second, but can be adjusted through the solver properties, as seen in figure 7 below.
Figure 7: Nonlinear static study properties.
Solution convergence is sometimes a concern for the implicit nonlinear solvers used in SOLIDWORKS Simulation Premium.
Time curves for loads and displacements must feature non-vertical slope in all areas to prevent solution convergence problems. It’s also necessary to provide a small enough time increment for the solution to converge.
The default “Automatic (autostepping)” option accomplishes this quite well by automatically reducing time step size when solution convergence issues are detected.
In this example, the time steps automatically reduce during the contact interactions between the two bodies. The mesh and contact pairs are defined as below:
Figure 8: Mesh and contact set definition.
Peak stresses are easily extracted by plotting relevant parameters such as Von Mises stress at various time steps or activating an envelope plot which will plot the maximum values across all steps. If stresses are in the elastic region then it’s not inherently necessary to use a nonlinear material model for these types of problems.
Another parameter of interest is the insertion and pull-out forces required. As force was not specified as an input to this analysis it is a variable being solved for that can be extracted.
This is accomplished by right clicking the Results folder and choosing Plot Result Force, then Reaction Force on the face defined as a fixture. This can then be plotted over the solution, as seen in the figure below.
Figure 9: Reaction force extraction.
Any graph plot can be exported as a .CSV through the File, Save As submenu for easier interpretation in an external plotting tool. In the figure below, the force in the Z direction was isolated on a plot in Microsoft Excel:
Figure 10: Reaction force in Z direction vs. time.
Note that the number of data points on the plot is controlled by the time steps in the nonlinear analysis. More data points may be desirable for plotting purposes, even if additional time steps aren’t necessary for solver convergence.
In these situations it’s recommended to reduce the “Max” time step size in the automatic time step parameters. For instance, setting the max time step to .02 would ensure the result features, at minimum, 50 data points—potentially more if the time step size needs to autostep down in any given area for convergence.
Example 3: Elastomers and Hyperelastic Materials
Elastomers such as rubber, TPE or EPDM are another common focus area for nonlinear analysis, utilizing a hyperelastic material model.
The Mooney-Rivlin model is the perhaps the most widely used in the area of hyperelastic material finite element analysis. It accepts inputs of either Mooney-Rivlin constants, or up to three material curves obtained through physical testing: simple tension, planar tension/pure shear, and biaxial tension.
A properly defined Mooney-Rivlin material model may allow examination of elongations of up to 300% or more. A common application for analysis of this type is gasket and O-ring design. In this example, a syringe plunger is presented modeled with a rubber-like material, as pictured in the figure below.
Figure 11: Cross section of syringe 3D Model.
The desired movement is to insert the plunger into the syringe barrel body. Parameters of interest here would include the insertion force required, the geometry of the seal that is generated and the contact pressure associated with the sealed surfaces.
Study setup for this example is similar to the Snap Fit Connector example in that a prescribed displacement is used to insert the plunger, and locally defined no penetration contact was employed. A Mooney-Rivlin material model was assigned to the black plunger body, and a linear elastic material model was used for the barrel body.
A key difference in this case is the use of 2D Simplification to analyze an axisymmetric slice of the model. This has many benefits in terms of solution time for a given mesh density, but also tends to have a much more favorable outcome in terms of solution convergence for the types of complex contact conditions that will occur once the hyperelastic material starts deforming.
Results at various timesteps are presented in Figure 12 below.
Figure 12: Results of 2D-simplified analysis with hyperelastic material model.
To get a sense of the sealing performance of the plunger to barrel interface, a Contact Pressure stress plot is created as visualized in Figure 13 below.
Figure 13: Contact Pressure stress plot with vector display.
The contact pressure values reported are used to make determinations about the amount of fluid pressure that can be resisted.
Sourcing Material Data
The more advanced material models provided in nonlinear study types are great, but they aren’t much use if a reliable source of material data can’t be established.
For the greatest accuracy, material model definitions should come from a material as close as possible to production parts. Ideally, material tests would be performed on a material sample from each lot of parts to derive the curves necessary.
There are some materials built into the default SOLIDWORKS Material library that feature more advanced material definitions. Any Material that says (SS) next to it includes a stress-strain curve that can be used with plasticity models.
Figure 14: Available material models in SOLIDWORKS Simulation Premium Nonlinear analysis.
Note in the figure above the text on the bottom of the material library window to “Click here” to access more materials. Through this link, SOLIDWORKS Simulation Professional or Premium customers on active subscription will have access to an additional material web portal called Matereality.
Matereality has many material definitions for fatigue, stress-strain curves and hyperelastic material models, as well as providing sources, references or certificates for material samples.
The raw test curves can be extracted from Matereality if desired, or each material can be conveniently downloaded as a SOLIDWORKS material.
Figure 15: Stress-strain curve for 7075-T6 aluminum from Matereality.
This makes Matereality a convenient fallback source for material models when they aren’t otherwise readily available.
Beyond SOLIDWORKS Simulation Premium
There are limits to what SOLIDWORKS Simulation Premium Nonlinear is capable of. Highly nonlinear systems with complex contact behavior or very large strains may be technically possible to solve but could require more simplification than desired or need frequent adjustments to time step size and mesh density.
Other offerings such as SIMULIA Abaqus employ state of the art nonlinear solvers particularly useful for resolving these difficulties. Some of the applications of Abaqus for nonlinear analysis include vehicle crash testing, buckling problems with many self-contacting faces (such as an imploding pressure vessel or a crumpling soda can) and drop tests for consumer product design.
Summary & Resources
This article presented a variety of use cases through three examples of nonlinear analysis.
There are many additional applications of nonlinear analysis in SOLIDWORKS Simulation Premium, including but not limited to nonlinear buckling studies, creep analysis, viscoelastic material model for foams and Nitinol (a nickel titanium alloy) shape-memory alloy material model.
Aside from these more exotic applications, it is also useful as a step-up from linear static analysis when complex contact conditions or large deformations arise.
Interested in trying out nonlinear FEA? There are a variety of built-in tutorials accessible from the pull-down menus. With the SOLIDWORKS Simulation add-in loaded, choose Help, SOLIDWORKS Simulation, Tutorials and click SOLIDWORKS Simulation Premium for a variety of step-by-step tutorials for various applications.
Figure 16: SOLIDWORKS Simulation Premium Tutorials.
Training courses should also be available locally from a SOLIDWORKS Value Added Reseller (VAR), or online.
SOLIDWORKS Simulation is also capable of copying a static study into a nonlinear study:
Figure 17: Copy static study into nonlinear study.
This means an existing static study can be used to quickly generate the basis of a nonlinear analysis. Once the static study is copied over, nonlinear-specific features such as the various material models can be applied to relevant components and forces can be modified with load curves to produce a functional nonlinear study.