To begin, I would like to highlight several changes in the Linear Elastic Material model of the *Membrane* interface.

First off, the previous version of the interface always assumed geometric nonlinearity. The new version listens to the “Include geometric nonlinearity” setting in the study step settings in the same way as the *Solid Mechanics* interface. The geometric linear version of the membrane can be used when it is acting as cladding on a solid surface. If the membrane is used by itself and not as a cladding, a tensile prestress is, as before, necessary in order to avoid singularity. This is because a membrane without stress or with a compressive stress has no transverse stiffness. To include the prestress effect, you must enable geometric nonlinearity for the study step.

Another update is that linear elastic materials can now also be orthotropic or anisotropic. This affects the settings of the Damping subnode as well, where non-isotropic loss factors are now allowed.

You may also notice that we have added a Hygroscopic Swelling feature as a subnode to the Linear Elastic Material node. (We described the hygroscopic swelling effect in a previous blog post. Check that out to learn more about the effect.)

All of you who use the Nonlinear Structural Materials Module may now use the *Membrane* interface to model thin hyperelastic structures by adding a Hyperelastic Material node. In order to illustrate the Hyperelastic Material model using the *Membrane* interface, we have recreated the Model Library example Inflation of a Spherical Rubber Balloon.

Tip: You can download the new version of the model in the Model Gallery by logging into your COMSOL Access account.

The *Membrane* interface works on the plane stress assumption, and it is assumed that there is no variation across the thickness of the balloon. Also, it requires a prestress to solve the model due to the absence of bending stiffness in the membrane. For this purpose, a separate study has been created before the inflation of the balloon is carried out in further studies. Results from this analysis are used as initial values for the rest of the inflation analyses. Aside from these two changes, the model is similar to the previous Solid Mechanics version.

The advantage of the Membrane version is that it is more computationally efficient. Why is that? Because the *Membrane* interface is on one geometric entity lower than the *Solid Mechanics* interface. The results obtained from the *Membrane* interface are in agreement with the analytical results. The plot below shows the inflation pressure as a function of circumferential stretch for different hyperelastic material models compared to the analytical expression for the Ogden model.

As the internal pressure increases, the balloon starts to inflate and its thickness decreases. Since the pressure is uniform over the surface, the thickness is the same along the cross section for any given inflation pressure. The next plot compares the variation of deformed thickness with applied stretch to the balloon obtained from the *Membrane* interface and the *Solid Mechanics* interface. We see that the thinning of the balloon is accurately captured by the *Membrane* interface.

We have added four new feature nodes to the *Membrane* interface.

They are as follows:

*Prescribed Velocity*— Available at the domain and boundary level*Prescribed Acceleration*— Available at the domain and boundary level*Symmetry*and*Antisymmetry*— Both available at the boundary levels

In addition to the specific improvements I just went over, we have made a few general changes to the structural mechanics interfaces that affect the *Membrane* interface. You will notice that the menus have been restructured for a number of structural mechanics interfaces.

The following interfaces now have restructured menus:

*Solid Mechanics**Shell**Plate**Membrane**Beam**Truss*

You can see a screenshot of the menu structure for the *2D Axisymmetric Membrane* interface below:

As for the Spring Foundation features, we have generalized these so that you can enter the “spring force versus displacement” and the “damping force versus velocity” relations in matrix form, rather than by component.

For 2D Axisymmetric cases, there is a new load type called “Point Load (on Axis)”. With this option, it is now possible to apply loads on a point on a symmetry axis.

For 2D Axisymmetric cases, a Point Load is actually a line load (N/m) since a point represents a ring in axisymmetry. To follow better naming conventions, such a load is now called “Ring Load” in both the *Solid Mechanics* interface and the *Membrane* interface.

Models that were made with COMSOL Multiphysics version 4.4 or earlier still use the old *Membrane* interface and new functionality is not available. To utilize the new functionality for old models, we suggest that you add a new *Membrane* interface and copy all the nodes from the previous interface to the new one.

As always, do not hesitate to contact us if you have any questions.

]]>

Residual stresses are self-equilibrating stresses that remain after performing the unloading of an elastic-plastic structure. During the manufacturing process of a mechanical part, residual stresses will be introduced. These will influence the part’s fatigue, failure, and even corrosion behaviors.

Indeed, uncontrolled residual stresses may cause a structure to fail prematurely. Although residual stresses may alter the performance, or even lead to the failure of manufactured products, some applications actually rely on them. For instance, brittle materials, such as glass in smartphone screens, are often manufactured so that compressive residual stresses are induced on the surface to avoid crack-tip propagation.

For these reasons, residual stresses play an important role in mechanical projects as a whole. Only through qualitative and quantitative analysis of these stresses is it possible to determine the most suitable machining processes for a given application. These types of analyses also help you discover the optimal amount of material to be used for their reliability or the most suitable shape that needs to be designed, in order to avoid malfunctions and failures.

Let’s consider the following slender beam with a rectangular cross section, depth a, and width b. The beam is fixed at the left-hand side and a bending moment is applied on the free end.

Based on the beam theory, it turns out that the bending moment is constant in this case and the stress can be written as:

(1)

\sigma_x=\frac{M_\mathrm{b}}{I_z}y

where I_z is the moment of inertia about the *z*-axis.

As M_\mathrm{b} increases, the beam first behaves in an elastic manner, but after reaching its yield moment, M_y, it begins to take on plastic behavior. This leads to an elastic-plastic cross section. Once the plastic zone has propagated through the entire cross section, the ultimate bending moment, M_\mathrm{ult}, that the beam can carry is determined. Here, it is assumed that the beam will collapse at such a moment and that it has a perfectly plastic behavior.

The outer fibers of the beam will reach the yield point first, while the core fibers remain elastic. Thus, the previous equation applied to the outer fibers of the beam provides the first yielding moment:

(2)

M_y=\frac{\sigma_\mathrm{yield} I_z}{b/2}=\frac{\sigma_\mathrm{yield} ab^3/12}{b/2}=\frac{ab^2\sigma_\mathrm{yield}}{6}

where \sigma_\mathrm{yield} is the yield stress.

Under an elastic-plastic moment, M_\mathrm{ep} < M_\mathrm{ult}, the plastic zone propagates through the thickness by a distance of h_\mathrm{p} at each side of the beam, as shown below.

*Plastic zone penetration in a rectangular cross-section beam.*

The total moment can be divided into an elastic part, M_e, and a plastic part, M_p, such that:

(3)

M_\mathrm{ep}=M_\mathrm{e}+M_\mathrm{p}=\frac{2\sigma_\mathrm{yield}I_\mathrm{e}}{b-2h_\mathrm{p}}+\sigma_\mathrm{yield}ah_\mathrm{p}(b-h_\mathrm{p})

where I_\mathrm{e}=\frac{a(b-2h_\mathrm{p})^3}{12} is the elastic core moment of inertia along the *z*-axis.

Combining the last two expressions, we get the following:

(4)

M_\mathrm{ep}=\frac{ab^2\sigma_\mathrm{yield}}{6}\left[1+\frac{2h_p}{b}\left(1-\frac{h_p}{b}\right)\right]

When an elastic-perfectly plastic beam is unloading from M_\mathrm{ep}, a state of residual stress, \sigma_r, remains in the beam cross section. The beam attempts to recover its initial shape following recovery of elastic bending stress, \sigma_\mathrm{e}. Here, it is assumed that purely elastic unloading occurs after being loaded at M_\mathrm{ep}, corresponding to a state of elastic-plastic stress, \sigma. The residual stresses can be computed from the difference between the elastic-plastic stress and the purely elastic stress — i.e., the stress you would have if plastic behavior was not involved.

(5)

The elastic bending theory gives the recovered elastic stress as:

(6)

\sigma_\mathrm{e}=\frac{M_\mathrm{tot}y}{I_z}=\frac{2\sigma_\mathrm{yield}}{b}\left[1+\frac{2h_\mathrm{p}}{b}\left(1-\frac{h_\mathrm{p}}{b}\right)\right]y

Assuming a perfectly plastic behavior, the stress \sigma in the plastic zone (in other terms, \frac{b}{2}-h_\mathrm{p} \le |y| \le \frac{b}{2}) remains constant and equal to \sigma_\mathrm{yield}. Therefore, according to the Equation (5), the residual stresses can be written as:

(7)

\sigma_\mathrm{r}=\sigma_\mathrm{yield}-\frac{2\sigma_\mathrm{yield}}{b}\left[1+\frac{2h_\mathrm{p}}{b}\left(1-\frac{h_\mathrm{p}}{b}\right)\right]y

In the elastic zone (in other terms, 0 \le |y| \le \frac{b}{2}-h_\mathrm{p}), the beam theory provides the applied stress as:

(8)

\sigma_\mathrm{e}=\frac{M_\mathrm{e}y}{I_\mathrm{e}}=\frac{2y\sigma_\mathrm{yield}}{b-2h_\mathrm{p}}

Therefore, the residual stress is then deduced as:

(9)

\sigma_\mathrm{r}=\sigma_\mathrm{yield}\left[\frac{2}{b-2h_\mathrm{p}}-\frac{2}{b}\left[1+\frac{2h_\mathrm{p}}{b}\left(1-\frac{h_\mathrm{p}}{b}\right)\right]\right]y

Note that after the external moment has been removed, the beam will still have some permanent displacement due to plastic deformation, but it will also have recovered some of the displacement that was present at the peak load. This *springback* effect is important when you want to achieve a controlled plastic deformation.

When modeling the beam in 2D, we could choose a *plane stress* assumption taking Poisson’s ratio, \nu=0, to match with the 1D beam theory, which does not account for the Poisson effect. In COMSOL Multiphysics, you can model 2D plane stress by selecting a 2D space dimension and choosing the *Solid Mechanics* interface.

Here, we will show how to use the *Solid Mechanics* interface in 2D to compute the residual stresses in the beam cross section.

*A snapshot of the 2D beam model using the* Solid Mechanics *interface.*

According to the snapshot above, we define variables to evaluate the theoretical residual stresses we worked out in the section above. Those values will be used to compare the computed results with the theoretical ones.

The applied bending moment is ramped progressively. A Plasticity node is added to account for the uniaxial plastic behavior that may occur through the beam thickness. Plastic flow begins once \sigma_x reaches the critical value \sigma_\mathrm{yield}. Any fiber that has reached this value will remain at a constant state of stress during loading.

In the graph below, you can see the stress distribution along the *Y*-axis of the cross section. The applied bending moment has been computed from Equation (4) for a plastic zone with depth h_\mathrm{p}=\frac{b}{4}=0.01 \ \mathrm{m}. According to the blue curve, COMSOL Multiphysics results match perfectly with this value. The red curve represents the residual stresses after one loading-unloading cycle. It is worth noting that the residual stresses obtained may also be found by subtracting the elastic curve (green) from the elastic-perfectly plastic curve (blue).

*Stress value after elastic-plastic loading, elastic loading, and unloading.*

Equations (7) and (9) have been defined as variables and compared to the solution computed in COMSOL Multiphysics. As shown in the previous screenshot, you can create a “switch” using the if() operator, so that the two expressions representing the analytical residual stresses are gathered together in one expression. The next graph shows both analytical and computed residual stresses after two loading-unloading cycles.

*Analytical vs. computed residual stresses.*

COMSOL Multiphysics enables you to model the hysteresis cycle of a given material. In the case of perfectly plastic behavior, as depicted below, the second load cycle already provides a stable stress-strain response that is representative of each consecutive load cycle. For instance, you can use these load cycles to carry out a fatigue analysis.

*Hysteresis behavior after three loading-unloading cycles.*

Last but not least, let’s find out how strain-hardening behavior influences residual stresses and loading-unloading cycles. So far, we have been dealing with a perfectly plastic material. The yield stress remains constant, no matter the number of cycles or whether a tensile or a compressive is applied. Equation (5) is only valid as long as reverse yielding does not occur. Since reverse plastic deformation during unloading has a negative effect on the performance, it is quite important to figure out under which condition reverse yielding is likely to occur.

A ductile material that is subjected to an increasing stress in one direction (in tension, for instance) and then unloaded, will behave differently when loaded in the reverse direction. It is found that the *compressive* yield stress is now lower than that measured in *tension*. This is called the *Bauschinger effect*. Similarly, an initial compression provides a lowered tensile yield stress. The figure below displays this effect over two stress cycles:

*Hysteresis behavior with kinematic strain hardening.*

Now, let’s move on to a more sophisticated mechanical process in which residual stresses are of great importance: the sheet metal forming process.

Die forming is a widespread sheet metal forming manufacturing process. The workpiece, usually a metal sheet, is permanently reshaped around a die through plastic deformation by forming and drawing processes. A blankholder applies pressure to the blank, leading the metal sheet to flow against the die.

In order to avoid cracks, tears, wrinkles, and too much thinning and stretching, you can turn to simulations. They can also be useful to estimate and overcome the *springback phenomenon*. This refers to how the workpiece will attempt to recover its initial shape once the forming process is done and the forming tools are removed. Springback can lead the formed blank to reach an unexpected state of warping. To cope with this effect, the sheet can be over-bent. Thus, the die, punch, and blankholder must be manufactured not only to match the actual shape of the object, but also to allow for springback.

In this study, the sheet is made of aluminum. A Hillâ€™s orthotropic elastoplastic material model with isotropic hardening is used to characterize the plastic deformation. It has been observed that metal sheets in deep drawing process no longer behave isotropically. There tends to be less plastic deformation through the thickness. Therefore, in die forming and deep drawing of sheets, we need a kind of anisotropy where the sheet is isotropic in-plane and has an increased strength in the perpendicular direction, called *transverse isotropy*.

Below, we have illustrated the forming tools that are used in the process.

*Forming tools: The die is shown in red, punch in blue, blankholder in pink, and the blank in gray.*

As mentioned above, simulations can allow for handling several tasks that need to be taken into account whenever such a mechanical process is worked out. For instance, optimization of the corner radius of both the die and the punch can be carried out properly to prevent tearing of the metal sheet. It may also be useful to carry out simulations in order to get the clearance that is needed between the punch and the die, to avoid shearing or cutting of the metal blank.

One of the most challenging aspects is to figure out how much of the metal sheet should be over-bent. When the sheet has been formed, the residual stresses cause the material to spring back towards its initial position, so the sheet must be over-bent to achieve the desired bend angle. Therefore, you have to properly model residual stresses as not to over- or underestimate the springback phenomenon.

The two animations below show the sheet metal forming as well as the springback of the metal blank.

*Representation in the* RZ*-plane of the spingback phenomena.*

*Simulation of sheet metal forming.*

When subjecting the structure to other mechanical loads, the superposition of the residual stresses can reduce the reliability of the structure or even cause irreversible damages. Therefore, the residual stresses must be released as much as possible or be managed so that the structure can withstand the external loads that may be applied. The plot below shows the Hill effective residual stresses that remain around the bend regions after the deep-drawn cup process.

Today, we studied residual stresses in structural mechanics. We introduced a conventional definition, which was first applied to a bending beam example. We simulated this bending example using COMSOL Multiphysics and compared our results to the analytical solution from the beam theory. Then, we explored the importance of the residual stresses in a sheet metal forming example. We saw that any mechanical process induces residual stresses and particular care must be given to release them properly or, at least, be certain that they will not cause any damage.

Learn more about the related products:

]]>