Submodeling with Plasticity

Submodeling is a powerful technique for computing accurate local results in large structures. The basic idea is that a small detailed model is analyzed, driven by boundary conditions that are given by the results from a global model.

In this example, it is shown how you can incorporate nonlinearities in a submodel. The source of the nonlinearity is plasticity, but the same approach can be used also for other cases. The only important thing is the fundamental assumption that the properties of the submodel are such that its stiffness does not differ significantly from what is computed from the same volume of material in the global model.

If the material would have an explicit time dependency, as would be the case for creep, then the submodel would have to be analyzed in time domain.

The global model can be either considered as linear or be analyzed under the same nonlinear conditions as the submodel. A nonlinear analysis would provide somewhat better boundary conditions for the submodel, but may be computationally too expensive for a large structure.

This example is an extension of the model Submodeling Analysis of a Shaft in the COMSOL Multiphysics Application Library, where the general submodeling technique is discussed in more detail.

Model Definition

The geometry consists of a shaft with a sudden change in diameter. At the location of the diameter change, there is a fillet with a small radius where stress concentrations will appear. There is also a central hole through the shaft. The geometry and mesh are shown in Figure 1.

The shaft is fixed at the thick end. On the thin end, a tensile force of 2500 N and a shear force of 900 N are applied.

The material is steel, with Young’s modulus 200 GPa and Poisson’s ratio 0.3.

The yield stress is 350 MPa, and a linear hardening with tangent modulus 1.045 GPa is assumed.

Figure 1: The full model.

As submodel, a region around the fillet at the side giving the highest stress is chosen.

The geometry and mesh of the submodel are shown in Figure 2.

Figure 2: The submodel.

Results and Discussion

In the original linear model, the computed maximum von Mises stress is 466 MPa. This is well above the yield limit of 350 MPa. A plot of the stress contour for the yield limit, Figure 3, shows that the yield stress is exceeded only in a smaller region in the fillet. This indicates that it can be possible to apply the submodeling technique to determine the stress and strain state accurately. Since only a small volume of the material will yield, the stiffness of the component should not be affected too much.

Figure 3: Stress distribution in the linear analysis. The contour shows the yield limit.

In Figure 4, the stress distribution after the full nonlinear analysis is shown. The peak stress is now 351 MPa. There is only a small amount of hardening. In the same figure, the actual size of the plastic region is shown, together with the previous estimate from the nonlinear analysis.

Figure 4: Von Mises equivalent stress at full load in the elastoplastic analysis. The yellow contour shows where the yield stress was exceeded in the elastic analysis while the cyan contour shows the same limit in the elastoplastic analysis.

In Figure 5, the equivalent plastic strain field is shown. As can be seen, the plastic zone does not penetrate very deep from the surface of the fillet. This also serves as a verification of the assumption that the introduction of the elastoplastic material model should not affect the overall stiffness significantly.

The maximum plastic strain is about 0.08 %.

It should be noted that even with mesh in the submodel, the plasticity is essentially confined to the outermost layer of elements.

Figure 5: Equivalent plastic strain in the submodel.

As another verification of the validity of the approach is to evaluate the reaction force in the Y-direction for the cut in the thin part of the shaft for all steps in the auxiliary sweep. When normalized by the applied shear load, the value should ideally be constant, and equal to 1. In Figure 6, the result is shown. In the linear regime, the value is 0.990. This can be interpreted as that the submodel actually is 1.0% more compliant than the global model. At full load, the normalized reaction force has decreased to 0.983. The force applied to the submodel is thus about 1.7% too small, which is probably still acceptable.

Figure 6: The normalized cut reaction force as function of the load multiplier.

Notes About the COMSOL Implementation

When a study that either contains an auxiliary sweep, or is time dependent, references results from a previous study, it is important that correct values can be retrieved. This means that the same parameter must be used in both studies.

In time domain, the built-in time parameter (t) is used. In an auxiliary sweep, you must select the same parameter to represent the loading in both studies. The parameter values that are used can however differ. When values are not matching, the results from the previous study are interpolated. Thus, it is a minimum requirement that the range of the loading parameter in the previous study is at least as large as in the one referencing it.

In this example, the first (full model) study is linear. Still, in order for results to be interpolated, a formal auxiliary sweep with two parameter values is required.

In the settings for the second study step, you need to make the appropriate settings under :

•