Guidelines for NONLINEAR ANALYSES

Ramesh Ramalingam
Cosmos
Los Angeles, Calif.

The maximum stress from a nonlinear analysis using CosmosDesignStar (same loading and boundary conditions used in the static-linear analysis) is about 11,600 psi.

The electrical clip is restrained at the circular handle and loaded with 0.5 N on the small exposed tip at the lower right. Linear analysis shows a maximum stress of over 16,000 psi, which exceeds the material's yield strength of 8,000 psi. Stress beyond yield is one indicator that better answers will come from a nonlinear analysis.

Most engineering problems contain nonlinear effects. Take a paper clip, for example. Push on one end hard enough and the clip changes and maintains the new shape. In other words, the paper clip has a permanent deformation — a nonlinear behavior.

A swimming pool's diving board offers another illustration. With no one on the board, it's horizontal. But when a person stands on its end, the board dips to an angle depending on the person's weight. This drastic change in the shape results in a change in the stiffness of the diving board and hence requires a geometric nonlinear analysis.

In another example, a vessel subjected to high pressure undergoes a drastic change of shape, requiring a geometric nonlinear analysis similar to the diving-board example. However, the pressure load in this case always acts normal to the walls of the pressure vessel. For that reason, it's important to take into account the change in the direction of the pressure load as the walls change shape.

Realistic analysis of this scenario requires a geometric nonlinear analysis with nonconservative or follower loading. Linear analysis of this scenario assumes that the stiffness of the pressure vessel and the direction of the pressure on the walls are based on the initial shape of the pressure vessel, which is not the final shape.

In FEA programs equipped to handle real-world conditions, such as Cosmos-DesignStar, loading comes from adding forces in small increments, such as onetenth of a pressure value at a time, and then updating the stiffness of the model at each step.

Linear-static analysis, on the other hand, assumes that induced displacements are small, changes in structural stiffness caused by loading are negligible, and the magnitude and direction of the load do not change while the structure deforms. Linear analysis also assumes a linear relationship between loads and the induced response. For example if you double the load, the response of the model (displacements, strains, and stresses), also doubles. This simplified assumption works in many cases, but some problems require nonlinear analysis.

In general, these cases include:

Geometric nonlinearities. These come from a model with large displacements or rotations, large strain, or a combination of those, such as in metalforming processes.
Material nonlinearities. Rubber and elastics are nonlinear materials. The nonlinearities often occur when the material's stress-strain relation depends on the load history (as in plasticity problems), long load durations (as in creep analysis), and when temperature can influence the outcome (as in thermoplasticity).
Contact nonlinearities. These occur when a structure's boundary conditions change because of the applied loads, such as in gear-tooth contacts and threaded connections.

Many engineers shy away from nonlinear analysis because they believe it is hard to use, expensive, and ties up computers for long periods. This was true at one time but is less so now thanks to faster processors and advances in FEA software.

A brief word on material models

In the same way that users must select a material before setting a solver to run, nonlinear analysis occasionally calls for selecting a material model. This consists of a series of algorithms that describe how the material behaves under stress and temperature. For nonlinear analysis,the table presents a few material models and description of where they work best.

Other material models are also available — but it is important to note that these models still represent an idealized behavior of real material conditions. When obtaining material properties, make sure to check the testing temperature and strain rate of the material data with that of the operating conditions of the model.

A demonstration of an analysis for a simple electrical connector shows the simplicity and capability of modern nonlinear software.

The thin electric connector must be sturdy enough not to deflect and touch adjacent parts. An initial linear-static analysis examines deflection and stresses. Conduct a nonlinear analysis if the deflection seems large or stresses exceed the material's yield strength. Then we can also find the residual stresses in the part when it undergoes one cycle of loading and unloading.

Linear stress analysis of this model with a 0.5-N load produces a maximum von Mises stress of 16,174 psi, which exceeds the material's 8,000-psi yield strength. This indicates that the problem calls for a nonlinear approach to account for material behavior beyond yield. A check of the displacement relative to the model size, however, shows the displacement is relatively small, about 2%.

Note that linear analyses generate conservative stress values which could lead to an overdesign. These results indicate that the solver assumed higher stiffness, and therefore produced higher stress.

Users of modern software don't have to start from scratch to conduct a useful nonlinear analysis. In fact, they only need to drag and drop the loads, constraints, mesh, and material from the linear study to a nonlinear one. For a nonlinear study of this model, the user selects the von Mises plasticity-material model and supplies a value for the tangent modulus — available from material handbooks. The user then defines a time curve and associates it with the loads to apply in small steps. In this case, after reaching the maximum loads they are decreased to zero in small steps to determine residual stress and permanent deformation.

Nonlinear analysis of this model produces a von Mises stress of 11,617 psi for maximum load of 0.5 N and a residual von Mises stress of 4,618 psi. The software also shows a permanent deformation less than 0.003 in. at the tip of the connector.

WHERE THE DIFFERENT MATERIAL MODELS WORK WELL
MATERIAL CLASSIFICATION	MODEL	COMMENTS
Elastoplastic	von Mises or Tresca	These models work for most metals and plastics that will be loaded beyond their elastic range. For metals that undergo work hardening, select the isotropic or kinematic hardening condition in the software.
Elastoplastic	Drucker-Prager	This model works for soils and granular materials.
Hyperelastic	Mooney-Rivlin and Ogden	Use these to model incompressible elastomers such as rubber.
Hyperelastic	Blatz-Ko	This model works for compressible polyurethane foam rubbers.
Viscoelastic	Generalized Maxwell	This model works for hard rubber or glass.