In *powder compaction*, a metal powder enters a die and is compacted through applied pressure. This high pressure comes from a punching tool inside the die cavity (often at the bottom surface). The powder is ejected from the cavity once it has been compacted and molded into a certain shape.

*Through powder compaction, metal powders are transformed into solid components. Image by Alchemist-hp — Own work. Licensed under CC BY-SA 3.0 DE, via Wikimedia Commons.*

With production rates averaging between 15 to 30 parts per minute, the powder compaction process enables manufacturers to quickly design strong components. Another benefit of this process is that it saves costs, as the component doesn’t need much additional work.

From a simulation standpoint, we need to perform a highly nonlinear structural analysis on powder compaction that accounts for:

- Contact between moving parts
- The elastoplastic constitutive law applied to the metal powder
- Geometric nonlinearity resulting from large displacements

As we demonstrate here, COMSOL Multiphysics® version 5.3 is ideal for handling such analyses.

For our example, let’s consider the fabrication of a cup-shaped component via powder compaction. The model geometry includes the workpiece (metal powder in this case) and the die. Note that the punch tool is not part of the model setup. We instead apply a prescribed displacement in the normal direction to the upper and lower faces of the powder in order to compact it. Because of the axial symmetry of the model, we can reduce its size to a 2D model, thus reducing the computational time of the simulation.

*The model geometry for a powder compaction analysis.*

The latest version of COMSOL Multiphysics includes five new porous plasticity models that cover various porosity values.

- Shima-Oyane
- Gurson
- Gurson-Tvergaard-Needleman
- Fleck-Kuhn-McMeeking
- FKM-GTN

These models are important for simulating powder compaction, as they allow us to accurately represent the porosity of the workpiece and produce reliable results. In this case, we combine the Fleck-Kuhn-McMeeking and Gurson-Tvergaard-Needleman models to describe an aluminum metal powder. Note that the die’s material properties assume it to be rigid.

In addition to the *Prescribed Displacement* boundary condition mentioned above, we also set the inner and outer dies as fixed domains.

From our simulation results, we can assess various properties of the metal powder at the end of compaction. To start, let’s look at the volumetric plastic strain. The strain at the center of the fillet appears to be minimal, while the strain near the ends is high. At the corner points of the workpiece, the strain is around 12% — likely the result of friction against the die.

*The volumetric plastic strain of the workpiece as the compaction process ends.*

During compaction, the porosity of the aluminum powder decreases, while the density and strength of the component increases. Based on the geometry and loading used in this scenario, we can expect that the changes to the porosity will be nonuniform.

The plot below shows the current void volume fraction contours of the powder; i.e., the porosity of the powder. Compared to the middle and top portions of the workpiece, the metal powder in the thin lower portion is more compact. Near the central area of the fillet, the powder is less compact because of material sliding on the rounded corner. The following animation illustrates how the volume fraction evolves over time.

*The current void volume fraction as the compaction process ends.*

*Changes in the volume fraction over time.*

Lastly, let’s consider the von Mises stress in the workpiece. The results indicate that the stress is greater in the areas where more compaction occurs.

*The von Mises stress within the workpiece.*

When simulating powder compaction, it is important to access the appropriate plasticity model that is preferably predefined in your analysis tool and available for direct use. To meet your modeling needs, COMSOL Multiphysics® version 5.3 brings you five new models that cover a wide range of porosity values.

For a helpful introduction to using these porous plasticity models, try out the example from today’s blog post.

]]>

Arteries are blood vessels that carry oxygenated blood from the heart throughout the body. They are layered structures consisting of intima, with media and adventitia (also called externa) on the outside layers. The media and adventitia are the layers that are primarily responsible for mechanical behavior in healthy arteries.

Both of these layers are made up of collagenous soft tissues that exhibit noticeable strain stiffening behavior. Each layer has anisotropic properties because of families of collagen fibers. This means that these fiber-reinforced structures allow the blood vessels to experience large strains.

*An artery wall’s structure. Image by BruceBlaus — Own work. Licensed by CC BY 3.0, via Wikimedia Commons.*

A reliable constitutive model for arterial wall mechanics is essential to investigate changes in the arterial system due to age and disease, and for designing prostheses, among other uses (Ref. 3). The Holzapfel-Gasser-Ogden (HGO) constitutive model (Ref. 2) captures the anisotropic mechanical response described above, which has also been observed in lab experiments on excised arteries. Typical experiments in the lab measure the response of arterial sections subject to combined axial stretch and internal blood pressure, and numerical examples try to match this data to better understand its mechanics.

As Bower points out in Applied Mechanics of Solids: “*Finite strain viscoelasticity is not as well developed as finite strain plasticity, and a number of different formulations exist.*” In COMSOL Multiphysics version 5.2a, we have implemented the Holzapfel model for large-strain viscoelasticity (Ref. 1, Ref. 3), which is well suited to combine with any of the predefined hyperelastic material models available in the COMSOL software.

The author proposes a generalized Maxwell model based on the splitting of the strain energy density into volumetric and isochoric contributions

W(C,\Gamma_m) = W_{vol}(J) + W_{iso}(\bar{C}) + \sum_{m} \Psi_m(\bar{C},\Gamma_m)

Here, stands for the right Cauchy-Green deformation tensor and stands for its isochoric counterpart. The free energy associated to the nonequilibrium state, , is a function of the isochoric right Cauchy-Green tensor and internal strain-like variables (Ref. 1, Ref. 3).

The strain energy in the pure-elastic branch is normally denoted with the superscript to denote the long-term equilibrium (as ).

Then, Holzapfel derives the expression for the second Piola-Kirchoff stress in the hyperelastic and viscoelastic branches

S = 2\frac{\partial W}{\partial C} = S_{vol}^\infty + S_{iso}^\infty + 2\sum_m \frac{\partial \Psi_m}{\partial C}

and also defines the auxiliary stress tensors from thermodynamic considerations

Q_m =2 \frac{\partial \Psi_m(\bar{C},\Gamma_m)}{\partial C} =-2 \frac{\partial \Psi_m(\bar{C},\Gamma_m)}{\partial \Gamma_m}

The total second Piola-Kirchoff stress (hyperelastic and viscoelastic branches) is then given by

S = 2\frac{\partial W}{\partial C} = S_{vol}^\infty + S_{iso}^\infty + \sum_m Q_m

*A schematic representation of the second Piola-Kirchoff stress for a generalized Maxwell model in large-strain viscoelasticity.*

The evolution of the stresses in the viscoelastic branches is given by solving the rate equations

\dot{Q}_m+\frac{1}{\tau_m}Q_m = \dot{S}_{iso,m}

where is the relaxation time of the branch and is the corresponding second Piola-Kirchoff stress tensor.

Holzapfel also assumes that there should be an isochoric strain energy density associated to the spring on each branch, , so

S_{iso, m} = 2\frac{\partial W_{iso,m}}{\partial C}

The main assumption in the Holzapfel formalism is that the isochoric strain energy per branch depends on the isochoric strain energy of the main hyperelastic branch

W_{iso, m}= \beta_\alpha W_{iso}^\infty(\bar{C})

Here, the dimensionless coefficients are called *strain energy factors*.

The second Piola-Kirchoff stress per branch then becomes

S_{iso, m} = 2\frac{\partial W_{iso,m}}{\partial C} = \beta_mS_{iso}^\infty

and the rate to solve becomes

\dot{Q}_m+\frac{1}{\tau_m}Q_m = \beta_m \dot{S}_{iso}^\infty

The generalized Maxwell viscoelastic model in version 5.2a of COMSOL Multiphysics is available for all of the hyperelastic materials, and it also contains the same options for modeling thermal effects as implemented for linear viscoelasticity.

*With the User defined option, you can neglect thermal effects, use the predefined William-Landel-Ferry or Arrhenius shift functions, or define your own shift function.*

Let’s take a look at how large-strain viscoelasticity can be applied to biomechanics modeling.

To model the behavior of arterial walls after sudden changes in axial stress, we need to use a hyperviscoelastic material model, which goes beyond the HGO material model.

Take a look at the Arterial Wall Mechanics tutorial model for more details on how to set up an anisotropic hyperelastic material.

To start, let’s add viscoelastic behavior to this particular material model. As described in Ref. 3, a generalized Maxwell model of five branches added to the HGO model is suitable to model relaxation times ranging from 1 ms to 10 seconds. This model is suitable for quantitatively representing the viscoelastic response of circumferential segments of arteries (Ref. 3). To do so, we right-click on the *Hyperelastic material* node and add a *Viscoelasticity* node (we can also combine this with thermal expansion or other effects).

By default, we get a generalized Maxwell model with one branch. However, we can also use the standard linear solid (SLS) model or the Kelvin-Voigt viscoelastic model.

Then, we add the five branches with the corresponding energy factors and relaxation times as described in (Ref. 3). We are able to retrieve (and also save) such parameters from a text file.

After refurbishing the HGO hyperelastic material with five viscoelastic branches, we can simulate what happens in an artery section when subject to a constant axial strain for four minutes.

*The stresses in the viscoelastic branches. Note the different relaxation times for the stresses in the five branches of the generalized Maxwell viscoelastic material.*

The axial stress relaxes to the steady state for times longer than the highest relaxation time. The ability to model large-strain viscoelasticity in COMSOL Multiphysics enables us to easily investigate and understand different biomedical materials and applications.

- Try it yourself: Download the Arterial Wall Viscoelasticity tutorial model and related information
- See how linear viscoelasticity can be used to reduce vibrations in structural dampers

- G. Holzapfel, Nonlinear Solid Mechanics: A Continuum Approach for Engineering,
*John Wiley & Sons*, 2000. - G. Holzapfel, T. Gasser, and R. Ogden, “A New Constitutive Framework for Arterial Wall Mechanics and a Comparative Study of Material Models,”
*J. Elasticity*, vol. 61, pp. 1–48, 2000. - G. Holzapfel, T. Gasser, and M. Stadler, “A Structural Model for the Viscoelastic Behavior of Arterial Walls: Continuum Formulation and Finite Element Analysis”,
*European Journal of Mechanics A/Solid*, vol.21, pp. 441–463, 2002.

Squeeze-off is a procedure used for gas pipeline maintenance and repair. The process involves compressing a pipe to completely stop the flow of gas with a squeeze-off mechanism. Squeeze-off must be performed slowly to avoid damaging the pipes.

*A diagram (background) and photo (inset) of a general pipe squeeze-off procedure.*

The American Society for Testing and Materials (ASTM) has set standards for the squeeze-off procedure for gas pipelines. The location of the squeeze-off tool from the nearest pipe fitting must be either three lengths of the pipe diameter long or about 30 cm (twelve inches) long, whichever distance is greater.

This creates problems in the pipeline maintenance industry, as most average consumer pipes have a diameter of about 6 cm (2.375 inches). Although three lengths of this common pipe diameter is about 18 cm (seven inches), the standards say that the squeeze-off distance must be whichever length is greater, meaning that the squeeze-off tool would still have to be placed about 30 cm away from the pipe fitting. This can lead to digging into main roads and detours, causing costly and inefficient maintenance procedures.

These ASTM standards prompted researchers at GTI, sponsored by OTD, to investigate a question: Is the 30-centimeter distance for squeeze-off locations really necessary for smaller pipes, or can the standards be updated to allow smaller pipes to use the three-pipe-length diameter?

The team at GTI, Oren Lever and Ernest Lever, researched their question by implementing a fully parametric, time-dependent model of a polyethylene (PE) pipeline with a squeeze-off and fitting. They used both the Structural Mechanics and Nonlinear Structural Materials modules in COMSOL Multiphysics to define the numerical and mechanical properties of two sets of structural contacts: internal pipe-to-pipe contact and external pipe-to-squeeze-off contact.

The simulation enabled the researchers to analyze large deformations in the pipe at each of the different stages of the squeeze-off process, which include:

- Pressurization of the pipe
- Squeeze-off
- Hold
- Release
- Relaxation

*A simulation of the five steps of the squeeze-off process.*

*The total displacement of the pipe when it is fully squeezed off.*

The team also meshed the pipe under the squeeze bars of the squeeze-off mechanism to analyze the very large deformations that occur when the pipe is fully squeezed off and the gas flow is completely shut down. With the meshing capabilities of the COMSOL software, this process could be easily scaled to different pipe sizes besides the common 6-centimeter-diameter pipe.

The polyethylene material that makes up the pipe in question exhibits unique properties and behaviors, which the researchers needed to capture by way of a customized viscoelastic-plastic constitutive model. For this, they turned to Veryst Engineering, a COMSOL Certified Consultant, for assistance with implementing the chosen material model into their COMSOL Multiphysics simulation.

First, the team at Veryst chose the experimental material tests that were needed to calibrate the material model typically used for polyethylene, a thermoplastic. Then, they fit the parameters of this material model to the stress-strain response of the polyethylene material. Finally, they implemented a set of ordinary differential equations (ODEs) needed to use the customized material model in the simulation.

For the material tests, GTI used a medium-density polyethylene (MDPE) pipe material. They tested it in tension and compression at different temperatures; strains; and strain rates, especially at high levels of strain (such as when the pipe is completely shut off). They also performed loading and unloading tests on the chosen material.

*Tensile response of the MDPE material from experimental data and custom material model implemented by Veryst Engineering.*

They then used their own MCalibration optimization tool to find actual values of material parameters that fit the experimental data, ensuring that the custom material model was a very good fit for GTI’s simulation.

Through their research, GTI found that for smaller pipe diameters, such as those smaller than about 9 cm (3.5 inches), the closer squeeze-off distance of three pipe diameters would not cause strains that went beyond the current strain limits accepted in the pipeline industry.

To further validate their results, the researchers used accelerated lifetime testing. They found that under their updated standard squeeze-off distance, pipes would have an 80-year lifetime at an average operation temperature of 20ºC. This is actually the current industry-accepted standard life expectancy for these pipes.

*Results from the accelerated lifetime testing for the polyethylene pipe.*

With their question answered through simulation and testing, GTI is now helping to revamp standard gas pipeline maintenance procedures to be more efficient and cost effective, without sacrificing the most important element: safety.

- Read the full story about GTI and gas pipeline maintenance on page 18 of
*COMSOL News*2016 - Browse the COMSOL Blog for more information on simulation applications involving nonlinear structural materials
- Explore the latest functionality and tools for nonlinear structural mechanics modeling in COMSOL Multiphysics® version 5.2a

To begin, let’s take a look at a common geometrical configuration for a pressure vessel.

Pressure vessels are made in different shapes and dimensions. Cylindrical shapes are a common choice due to the trade off between manufacturing cost and performance.

Typically, cylindrical pressure vessels are made out of a cylinder capped by two heads. Different shapes for the heads are available, with the torispherical head often selected. Torispherical heads are composed of a crown, a toroidal shape knuckle, and a straight flange.

The two most common torispherical heads in use are the *Klöpper head* and the *Korboggen head*. What differentiates these two heads is the geometric relationships that are used to design the crown and the knuckle dimensions. In a Klöpper head, and . In a Korboggen head, and . Here, is the radius of the cylindrical part of the vessel, is the crown radius, and is the knuckle radius.

*Geometrical dimensions of a cylindrical pressure vessel with a torispherical head.*

Now that we’ve got our geometry set up, let’s briefly discuss some important elements when it comes to material plasticity and how it affects the design of pressure vessels.

Rolled metal sheets are commonly used in the manufacturing of pressure vessels. Most designs are such that a material operates within the elastic limit, as is the case when moderately large stresses act in them. The material then exhibits a deformation that is proportional to the load. Further, the shape returns to the original configuration once the force is removed. However, if the force exceeds a limiting value known as the *yield limit*, the body does not return to its original shape, even when the loading is completely removed. It instead remains partly deformed.

In such a case, we say that the body has undergone plastic deformation. For a pressure vessel made of rolled steel, this yield stress can be of the order of 500 MPa. Due to the high internal pressure, parts of the vessel in the vicinity of the transition at the knuckle may exceed the elastic limit and operate in plastic conditions.

In this example, a rather sophisticated plasticity model is incorporated into the mix: *Hill’s orthotropic plasticity*. For rolled steel plates, the yield limit in different directions is not the same due to the rolling process. Such behavior can be captured using Hill’s orthotropic plasticity model. The Nonlinear Structural Materials Module in COMSOL Multiphysics is the internal backbone for the elastoplastic analyses of pressure vessels. Now, with the Application Builder, we can make such physics available in an easy-to-use app that can be accessed by a wide range of users.

When building a simulation app, your task as the designer is to identify the important parameters that influence the outcome of the simulation. Once these are determined, the flexibility and functionality of the Application Builder enables you to create a simplified user interface (UI) that includes only those selected parameters. End-users can then easily run simulation tests and interpret the results without having to understand how the underlying physics are actually implemented within COMSOL Multiphysics.

Knowing that we are going to perform plasticity analyses on a pressure vessel, the question becomes this: Which parameters are relevant for selection as user inputs? The options to vary the geometry and material properties are obvious candidates. Another desirable feature is the ability to modify the operating conditions; for instance, the operating pressure inside the vessel and allowable yield fraction values based on safety considerations. Such parameters are included as inputs in our app and can be entered through the customized UI.

*The UI of the Stress Analysis of a Pressure Vessel app.*

After computation, the quantities of interest can be displayed in predefined plots:

- Von Mises effective stress
- Plastic strains
- Yielded region
- Yielded volume fraction as a function of the internal pressure

The Stress Analysis of a Pressure Vessel app is just one example of how the Application Builder can be used to encapsulate complex simulation studies within a user-friendly layout. Suppose, for instance, that you want to meet a certain safety condition for a given operating pressure inside the vessel. With an app, it is easy to alter the geometry and material properties to identify the right combination that works within the safety limits. Users are able to modify the parameters in the UI without having to understand the working principles of COMSOL Multiphysics.

With apps, as we’ve highlighted here, performing repeated computations with varying parameter settings is faster and easier than ever before. Start building apps today and experience how they can optimize your own design workflow.

- Download the demo app presented today: Stress Analysis of a Pressure Vessel
- Watch this video to learn how to build and run simulation apps
- Looking to get hands-on experience creating apps? Consider attending one of our free workshops

The human body, as we know, is a complex machine comprised of individual systems that work together. Soft tissue plays an important role in helping these systems thrive, connecting and supporting other structures and organs within the body. This type of tissue is comprised of collagen, elastin, and ground substance. While the ground substance helps keep the tissue hydrated, the elastin and collagen fibers determine the tissue’s mechanical behavior.

When the soft tissue undergoes deformation, the elastin fibers cause the tissue to stiffen, storing the majority of the strain energy. The collagen fibers, meanwhile, are comparatively inextensible and loose. These fibers increase the tissue’s stiffness when pulled tight, limiting the degree of deformation and protecting the tissue from injury. Because each of these collagen fiber families tend to have preferred directions, soft tissues possess anisotropic properties.

Consider arterial wall mechanics, for instance. Arteries are blood vessels comprised of three layers: the *intima*, the *media*, and the *adventitia*. The two outer layers — the media and the adventitia — are primarily responsible for the mechanics behind healthy arteries and are both made up of collagenous soft tissues. The collagen fibers give each layer anisotropic properties and allow the blood vessels to sustain rather large elastic deformations.

*The anatomy of an artery. Image by Maksim, via Wikimedia Commons.*

An important step in understanding and describing the mechanical behavior of arteries is designing a model that accurately reflects their anisotropic nonlinear properties. Let’s take a look at such an example from our Application Gallery.

In our Arterial Wall Mechanics tutorial model, the model geometry is designed to represent part of a rabbit’s carotid artery. To model the media and adventitia, we use a layered cylindrical tube, which is reduced to a 10° sector.

*A model of a carotid artery section. Here, the length (L) is 2.5 mm, the inner radius (R _{i}) is 0.71 mm, and the outer radius (R_{o}) is 1.1 mm. The media thickness is 0.26 mm and the adventitia thickness is 0.13 mm.*

The boundary conditions used in this example are meant to replicate typical experiments measuring arteries’ responses to a combination of axial stretch and internal blood pressure. With the use of roller boundary conditions, the bottom section of the artery is able to freely expand in the radial direction. Meanwhile, prescribed displacements in the axial direction address the impact of axial stretching on the top surface. Lastly, a pressure boundary load applies internal pressure on the inner surface.

Here, we consider axial stretching within the range of 1.5 to 1.9 and internal pressures within the range of 0 and 160 mmHg. Stretch refers to the ratio between the current length and the original length. Within such ranges, the mechanical response is highly nonlinear and produces large elastic deformations — a behavior that can be described mathematically by the theory of hyperelasticity.

To accurately account for the arteries’ mechanical response, we can implement the Holzapfel-Gasser-Ogden (HGO) material model in COMSOL Multiphysics. This nearly incompressible anisotropic hyperelastic material model is based on the article “A New Constitutive Framework for Arterial Wall Mechanics and a Comparative Study of Material Models”, by G. Holzapfel, T. Gasser, and R. Ogden. The HGO model describes the mechanical behavior of the elastic ground substance and the collagen fiber network within the artery, accounting for the deformation and volumetric strain energy density in each fiber family.

To begin, we can first identify the static response of the artery to the applied boundary conditions. The figure below illustrates the fiber layout for the different fiber families. Red represents the media and blue represents the adventitia. The angles between the different fiber families vary.

*Fiber layout prior to deformation.*

Let’s now evaluate radial stress distribution through the thickness of the arterial wall. Here, we apply an axial stretch of 1.9 and an internal pressure of 160 mmHg.

*Radial stress distribution.*

Lastly, we can compare the internal blood pressure against the expansion of the inner radius. The analysis covers three different axial stretches within our initial range. Our results show good agreement with the findings from the article, which are illustrated by circles in the plot below.

*Comparing internal pressure with inner radius expansion.*

- Try it yourself: Download the Arterial Wall Mechanics tutorial model

Geometric nonlinearity may not even be explicitly introduced in a fundamental course on structural mechanics. In fact, geometric linearity is often tacitly assumed. In a geometrically linear setting, the equations of equilibrium are formulated in the undeformed state and are not updated with the deformation. This may sound a bit alarming at first, since computing deformations is what structural mechanics is all about.

However, in most engineering problems, the deformations are so small that the deviation from the original geometry is not perceptible. The small error introduced by ignoring the deformations does not warrant the added mathematical complexity generated by a more sophisticated theory. This is why a vast majority of analyses are made with an assumption of geometric linearity.

There are a number of cases where the deformation cannot be ignored, and not all of these cases comprise deformations that you would intuitively think of as being large.

The most important effects on the mathematics when you include geometric nonlinearity in COMSOL Multiphysics are:

- A distinction is made between the
*Spatial*and the*Material*frame. The spatial coordinates of a certain point () differ from the material coordinates of the same point () by the the displacement vector (), so that . It will thus matter whether you use uppercase or lowercase coordinate names in expressions. - The strains are represented by the Green-Lagrange strain tensor instead of the engineering strains.
- The stresses are represented by the Second Piola-Kirchoff stress tensor.
- Pressure loads take the deformation into account. Normals to boundaries are updated and area changes caused by stretching are taken into account.

You can read more about different stress and strain tensors in this previous blog post, but a small digression into the strain measures is needed. To this end, let us look at the difference between linear and the full nonlinear strain by considering some components of the strain tensor.

The *X*-direction Green-Lagrange normal strain can be written as

\epsilon_X = \frac{\partial u}{\partial X} + \frac{1}{2}(\frac{\partial u}{\partial X})^2 + \frac{1}{2}(\frac{\partial v}{\partial X})^2 + \frac{1}{2}(\frac{\partial w}{\partial X})^2

If the quadratic terms are omitted, the familiar engineering strain is retrieved:

\epsilon_X = \frac{\partial u}{\partial X}

Similarly, for a shear strain, the Green-Lagrange strain component is

\epsilon_{XY} = \frac{1}{2}(\frac{\partial u}{\partial Y} + \frac{\partial v}{\partial X} + \frac{\partial u}{\partial X} \frac{\partial u}{\partial Y} + \frac{\partial v}{\partial X} \frac{\partial v}{\partial Y} + \frac{\partial w}{\partial X} \frac{\partial w}{\partial Y} )

Again, the engineering strain is obtained by ignoring the nonlinear terms:

\epsilon_{XY} = \frac{1}{2}(\frac{\partial u}{\partial Y} + \frac{\partial v}{\partial X})

When a structure rotates significantly, the engineering strains used in basic theory will no longer give a useful representation. Rigid body rotations will cause nonzero components of the engineering strain tensor. This will, through the constitutive law, cause stresses that for physical reasons should not appear in a rigid body. Another way of viewing this is that any useful strain tensor must be able to reflect the fact that there is no stretching or change of relative angles in a rigid body motion.

Consider a 2D body rotating rigidly in the *xy*-plane around the origin. A simple linear plane stress model in which a rectangular steel plate is rotated 10° is shown below.

*Effective stress in a rectangular steel plate at a 10° rotation with no geometric nonlinearity.*

The result is an effective stress of 572 MPa, which is above the yield limit for the most common steel qualities. To see why this happened, let’s study the analytical solution:

A point originally placed at (X,Y) will then have moved to a new location (x,y), given by

\begin{matrix}

x = X \cos(\phi)-Y \sin(\phi) \\

y = X \sin(\phi) + Y \cos(\phi)

\end{matrix}

x = X \cos(\phi)-Y \sin(\phi) \\

y = X \sin(\phi) + Y \cos(\phi)

\end{matrix}

This means that the displacements (u,v) are

\begin{matrix}

u = x-X = X (\cos(\phi)-1)-Y \sin(\phi) \\

v = y-Y = X \sin(\phi) + Y (\cos(\phi)-1)

\end{matrix}

u = x-X = X (\cos(\phi)-1)-Y \sin(\phi) \\

v = y-Y = X \sin(\phi) + Y (\cos(\phi)-1)

\end{matrix}

The engineering strains will then be

\begin{array}{l}

\epsilon_X = \frac{\partial u}{\partial X} = \cos(\phi)-1 \\

\epsilon_Y = \frac{\partial v}{\partial Y} = \cos(\phi)-1 \\

\epsilon_{XY} = \frac{1}{2}(\frac{\partial u}{\partial Y}+\frac{\partial v}{\partial X}) = -\sin(\phi)+ \sin(\phi) = 0

\end{array}

\epsilon_X = \frac{\partial u}{\partial X} = \cos(\phi)-1 \\

\epsilon_Y = \frac{\partial v}{\partial Y} = \cos(\phi)-1 \\

\epsilon_{XY} = \frac{1}{2}(\frac{\partial u}{\partial Y}+\frac{\partial v}{\partial X}) = -\sin(\phi)+ \sin(\phi) = 0

\end{array}

For a rigid body rotation, all strains should be zero, but clearly two of these strain components are not. A metal will often yield at a strain that is of the order of 0.001. A fictitious strain of this size will already occur at a rotation of 2.5°. To keep the strain lower than 0.0001, there must not be rigid rotations larger than 0.8°. This means that even at angles where you often would expect a “small angle approximation” to be sufficient, the geometrically nonlinear approach must be used.

Using the same rigid body rotation as above, but using Green-Lagrange strains instead, gives

\epsilon_X = \frac{\partial u}{\partial X} + \frac{1}{2}(\frac{\partial u}{\partial X})^2 + \frac{1}{2}(\frac{\partial v}{\partial X})^2 = \cos(\phi)-1 + \frac{1}{2}(\cos(\phi)-1)^2+ \frac{1}{2}(\sin(\phi))^2 = 0

Now this strain tensor component is zero for any value of the rotation. This property can be shown for the whole Green-Lagrange strain tensor and also for arbitrary rotations.

By using a geometrically nonlinear formulation, you can avoid having these kinds of stress artifacts. This is confirmed by solving the same problem with geometric nonlinearity enabled. The stress levels are now pure numerical noise; 12 orders of magnitude lower than the yield limit.

*Effective stress at a 10° rotation while using geometric nonlinearity.*

Consider the two beams in the sketch below:

*Beams with different end conditions.*

At the right end, the upper beam is free to translate horizontally, while the lower beam is not. In a linear theory, these two end conditions are equivalent if the beam is subjected to a vertical load. There is no coupling between axial and bending action. However, in a geometrically nonlinear analysis, the different end conditions will lead to quite different results:

- When the end is free to move axially, the vertical displacement of the beam is almost the same as in the geometrically linear case.
- When the axial displacement is constrained, the vertical displacement will be smaller than in the linear case and have a strong nonlinear dependence on the load.

As the beam deflects, its center line will be stretched if the end cannot move inwards. This will introduce a significant axial force that will make the beam act similar to a wire in tension — the higher the tensile force, the more it will resist a transverse force.

*Midpoint deflection of a beam with a square cross section of 0.05 x 0.05. The red line indicates the load where the deflection in the linear analysis is 0.025 (half the height of the beam).*

The same ideas also apply to plates and shells. If the boundary conditions are such that deflection will cause in-plane tension, then the plate will become significantly stiffer with increasing deflection.

There is a rule of thumb saying that if the deflection of the beam or plate in a linear analysis exceeds half of its thickness, then geometrically nonlinear effects should be considered. This is indicated by the red line in the figure above.

As seen in the previous example, the stiffness of a structure can sometimes change significantly due to geometrically nonlinear effects. This is sometimes referred to as *stress stiffening*. The term is somewhat misleading, since it is also possible that the stiffness could decrease. If we were to add a compressive axial load to the beam above, its transverse stiffness would actually decrease.

Stress stiffening is important in, for example, rotating systems where the centrifugal forces can introduce significant tensile stresses. This causes the eigenfrequencies of the system to increase with the RPM.

*Campbell diagram showing how the natural frequencies of a rotating blade change with speed of rotation.*

Often, the loads that cause the prestress are not the same as the one for which you actually perform the analysis. So there may be two distinct load systems that must be analyzed separately.

In COMSOL Multiphysics, there are two predefined study types specifically intended for the analysis of prestressed systems:

- Prestressed Analysis, Eigenfrequency
- Prestressed Analysis, Frequency Domain

*Study types intended for the analysis of prestressed structures.*

These study types consist of two study steps in which step one is used for computing the prestress state. That study can be linear or nonlinear. The second study step is linear in itself, but includes the nonlinear terms caused by the geometric nonlinearity when setting up the stiffness matrix.

If you are interested in examples in which stress stiffening is important, please check out:

*Buckling*, or the loss of stability when the load reaches a certain critical value, is caused by geometrically nonlinear effects. In COMSOL Multiphysics, there is a specific study type called Linear Buckling for computing the first order approximation to the critical load.

*The Linear Buckling study type.*

In the linear buckling study, an approximate buckling load is obtained by solving an eigenvalue problem.

As an alternative, you can trace the full nonlinear response up to the point of collapse, and even past it. In this case, you must increase the load in smaller steps. This approach is significantly more computationally expensive, but more accurate.

*Load-deflection history with a buckling collapse at point A.
*

You can read more about buckling in this previous blog post.

Geometric nonlinearity is a property of the Study step. For those study types for which it is relevant, a check box is available in the settings for the study.

*Settings for a stationary study.*

Sometimes this check box is preselected and you cannot change it. This happens when you include certain physics nodes in the model tree that cannot be used in a linear context, such as:

- Hyperelastic material
- Large strain plasticity
- Contact

Note that most nonlinear material models, such as nonlinear elasticity or creep, do not assume geometric nonlinearity.

Geometrically nonlinear problems are often strongly nonlinear, and you need to consider that when supplying settings for the solver.

Think of the beam with the fixed end mentioned above. When solving the nonlinear problem, the solution after the first iteration will be the same as the solution to the linear problem so that all points on the beam move only vertically under a transverse load.

After the first iteration, there will thus be a significant axial elongation of the beam. Such an elongation is related to an axial force. As there is no net axial force (there is no external load in that direction), this force will end up as a residual for the next iteration. This unbalanced force may be larger than the applied load. To the nonlinear solver, this looks like a very nasty problem and the solver will often introduce damping.

Fortunately, these problems are often more well behaved than the numerics would indicate. You can then speed up the solution significantly by using a more aggressive iteration scheme than the default.

*Settings for the Fully Coupled solver.*

Using the Constant Newton scheme instead of the automatic adaptive scheme will cause the solver to make larger updates. The damping factor can be set to 1 (no damping) or possibly 0.9.

A problem where geometrical nonlinearity is the only source of nonlinearity will, in most cases, possess a unique solution for a certain load level. In this sense, it is possible to analyze the problem using a stationary analysis with a single load only. For convergence reasons, it is sometimes better to gradually increase the load using the parametric continuation solver.

An example of how the solver can be set up for a severely nonlinear problem is shown in our Pinched Hemispherical Shell tutorial model.

As we have shown above, there are several cases in which geometric nonlinearities must be considered when solving structural mechanics problems. So why don’t we always include this effect in our models to be on the safe side?

- Even if the nonlinear effect is very small, invoking the nonlinear solver will give you a significantly longer solution time. This is not an issue for small models, but when you are working with several million degrees of freedom, a reduction of the solution time by a factor of two really matters.
- Sometimes you want to be able to compare to an analytical solution, and such solutions are often based on linear theory.
- You may need to follow a standard or analysis procedure where it is assumed that a linear approach is used.
- In a geometrically nonlinear problem, it is necessary to use the actual load. If you just want to do a conceptual study of a structural response, the solution may not converge if the estimated load was too large.

Piezoelectric valves are common in medical and laboratory applications because they offer many advantages, such as energy efficiency, durability, and fast response times. To open and close the valve featured in this tutorial, there is a hyperelastic material with a piezoelectric actuator sitting on top of it. When a voltage is applied to the stacked piezoelectric actuator, it deforms in a way that either pushes the hyperelastic material against the opening of the valve to seal it or moves it away from the valve to open it.

*Valve, piezoelectric actuator, and seal.*

Stacked piezoelectric actuators consist of two actuators stacked on top of each other. Each of the two actuators is made up of alternating layers of piezoelectric material, PZT, and very thin metal conducting layers between them. Every second metal layer is grounded, while every other layer receives an applied voltage. Similarly, the stacked PZT layers have alternating polarization directions.

*Close-ups of the actuator and seal with alternating layers of PZT and metal highlighted. The top images show the PZT layers of alternating polarization directions. The bottom images show the metal substrate with an applied voltage to every other layer and the others set to a ground.*

The bimorph actuator under consideration can be thought of as two stacked actuators placed one on top of the other. For a positive applied voltage, the upper and lower actuators are designed to expand laterally and contract laterally, respectively. This results in a bending of the structure (in this case, a disc), such that the center of the disc arches downwards. This forces the hyperelastic seal into contact with the valve seat — closing the valve. In the surface plot below, the stress is indicated by the color scale.

*The von Mises stresses in a piezoelectric valve with a bimorph disc actuator.*

The Piezoelectric Valve tutorial model, a new addition to the Application Gallery with COMSOL Multiphysics 5.1, demonstrates how to model a stacked piezoelectric bimorph disc actuator in a pneumatic valve. The MEMS Module and Nonlinear Structural Materials Module are used for this simulation.

The valve model consists of a multilayer stacked piezoelectric actuator, which in itself is a complex structure of stacked layers and electrodes. The model also includes a stainless steel substrate and a seal of hyperelastic material over the through hole of the valve.

For the simulation, we apply 50 volts to the layers. The contact pressure is determined here at the two contact pressure points of the seal. We can see that deformation of the disc is greatest at the center, which compresses the hyperelastic seal against the valve’s opening and closes the valve.

*Left: The strain at the two contact surfaces of the valve’s seal. Here, we can see that the deformation of the disc is greatest at the center, which closes the valve. Right: The contact pressure at the two surface points of the valve’s seal.*

Modeling a piezoelectric valve allows us to analyze the operation of the stacked piezoelectric actuator and evaluate the stress and strain in the seal and the surrounding materials. The analysis could be extended to estimate the performance of the seal with different pressure differentials applied across the valve in the closed state.

- Tutorial Download: Piezoelectric Valve

One of the most common effects associated with an earthquake is shaking. Depending on the size and magnitude of the seismic waves, this shaking can result in various levels of destruction. In the case of buildings, such waves can produce instability or, in more extreme cases, cause structures to collapse.

Seismic control is an important consideration in the design of buildings. This is particularly relevant to taller structures, which pose a greater risk to human life during earthquakes. Such control can be achieved through various techniques, one of which includes a passive control approach where an external energy source isn’t required.

A *base isolation system* is an example of such a passive control method. As indicated by its name, a base isolation system isolates a structure’s base from its foundation with the use of a bearing. The bearing, which acts as an isolator, deflects and absorbs seismic waves, helping to protect the structure from the force of the vibrations.

*Fixed base and isolated base systems. Image by R. Sugumar, C.S. Kumar, and T.K. Datta*.

Base isolation systems are valued for their simplistic construction and installation as well as their ability to be installed in existing buildings. Such systems can be used effectively in tall structures featuring multiple levels and in buildings with up to 20 stories.

Using the Nonlinear Structural Materials Module in COMSOL Multiphysics, a team of researchers from India set out to investigate the efficiency of a base isolation system as well as how to optimize its performance. They presented their findings from the study at the COMSOL Conference 2014 Bangalore.

In the analysis, a laminated rubber bearing (LRB) was used as the isolator. Consisting of steel shims between rubber layers, the LRB uses its flexibility to deflect seismic waves and, through plastic deformation, absorbs the energy from the vibrations. Additionally, its lead core assists in further dissipating the energy. Here, the steel component of the LRB was treated as an elastoplastic material, the rubber as a hyperelastic material, and the lead as an elastic perfectly plastic model.

*A schematic depicting the cross section of the LRB. Image by R. Sugumar, C.S. Kumar, and T.K. Datta*.

For the structure, the research team chose a two-story, single-bay frame comprised of mild steel (i.e., low-carbon steel). In this study, two frames were analyzed: one bare frame and one frame with a base isolation system.

An eigenmode analysis was performed for the structures, and their damping properties were determined based on the first two eigenfrequencies and assuming damping ratios of 0.02. These damping properties were incorporated then into a transient analysis. The force exerted on the structures was derived from a pre-recorded earthquake time history, as illustrated in the plot below.

*Pre-recorded earthquake acceleration. Image by R. Sugumar, C.S. Kumar, and T.K. Datta*.

The responses of the bare frame and the base isolation system frame to the applied earthquake acceleration were then compared. The results showed that the presence of the isolator reduced the frame’s response to the vibrations, highlighting the effectiveness of this approach in providing structures with seismic control. Furthermore, researchers noted that modifying the material properties and the dimensions of the isolator could further enhance the LRB’s ability to control vibrations.

*Comparing the response of the bare frame (uncontrolled) and the frame with the base isolation system (controlled). Image by R. Sugumar, C.S. Kumar, and T.K. Datta*.

From this research, we can observe the effective nature of base isolation systems using laminated rubber bearings as a means of seismic control for structures. Simulation can help address how different parameters impact the performance of the isolator and advance its ability to stabilize vibrations within buildings. The analyses performed here can also be applied to other types of bearings, emphasizing the extensive capabilities and applications of the nonlinear material models and simulations available in the COMSOL Multiphysics FEA software.

- Access the presentation, poster, and abstract: “Seismic Control of a Structure Using Laminated Rubber Bearings“

A vehicle’s dashboard provides valuable information for a driver, from indicating the speed of the car to gauging its fuel levels. What’s as important as the instruments themselves is the manner in which they are installed. In many cases, fasteners known as snap hooks are used in the design of a car’s control panel, ensuring that the different components are securely fixed.

When inserting a snap hook into its slot, an important consideration is the force that needs to be applied to insert the hook into the slot as well as the force that is required to remove it. With COMSOL Multiphysics FEA software, you can study these forces and the resulting stresses and strains in the hook.

In the Snap Hook model, we leverage the snap hook’s symmetry to analyze only half of its original geometry in an effort to decrease the size of the model. The snap hook is assumed to be composed of an elastoplastic material featuring isotropic hardening and a constant tangent hardening modulus. Meanwhile, the lock is assumed to be rigid when compared to the hook, with the space behind the lock representing the slot into which the hook should lock.

*Model geometry.*

Several boundary conditions are applied to the model, as shown in the schematic below. For boundaries in the symmetry plane, a symmetry boundary condition is used. A fixed boundary condition is implemented for the face of the lock, where it is attached to the remainder of the geometry of the locking mechanism (not modeled here). Lastly, a prescribed boundary condition is applied where the face of the hook meets the rest of the geometry.

*The applied boundary conditions.*

Before insertion into the slot, we first measure the effective stress levels in the hook. As indicated in the following plot, the maximum effective stress levels occur at parameter step 0.84. This parameter represents the point right before the hook enters the slot. Note that when passing over the edge, the hook is bent upwards. The elastic forces will tend to press the hook into the slot before it “fits.” If holding the hook, you would be pushing up until this point; however, here the hook would actually be pulled away from your hand.

*The hook’s effective stress levels prior to entering the slot.*

The next graph depicts the degree of force needed to insert and remove the fastener as a function of the parameter step. When the parameter value varies from 0 to 1, the hook is moved inwards at a constant rate to eventually sit in the slot. Then, between the parameter values 1 and 2, the hook is pulled back out of the slot.

At the parameter value 0.2, the hook first comes into contact with the fixed locking mechanism. The force rises steeply, while the hook tip is forced upwards. In reality, the hook would snap into place after reaching the peak force of around 2.5 N at the parameter value 0.23. Since we control the displacement in the simulation, we can follow the force throughout the entire process. Between the parameter values 0.7 and 0.9, the hook slides down on the back side. The change in the sign of the force indicates that the hook is actually pulled into the slot by a combination of the geometry and the elastic forces.

When trying to pull the hook back out of the slot (at parameter values greater than 1), we must apply a load that is three times higher — about 7.5 N — to remove the hook from the slot (at a parameter value of about 1.12). This is a desirable feature of a hook designed for a locking mechanism.

*Force required for the insertion and removal of the snap hook. The first positive peak in the graph can be attributed to the elastic forces pushing the hook into the slot before it “fits.” Following retraction, the hook hits a steep surface, which results in the second positive peak in the graph. After passing the corner (represented by parameter 1.2), the hook is pressed out by itself, or a negative force.*

Upon its removal from the slot, the hook is shown to have a volume in which there are plastic strains, as illustrated in the plot below. Thus, we can conclude that after inserting the hook into the slot, it is permanently deformed.

*The hook’s effective plastic strain following its removal from the slot.*

In this blog post, we have explored the role of simulation in addressing the forces behind the insertion and removal of a snap hook into a slot. By analyzing such forces, you can enhance the design of snap hooks to ensure that they provide continuous security while also being able to remove them without causing damage to the fastener. This is particularly relevant within the automotive industry in cases where certain parts of a vehicle’s control panel need to be repaired or replaced.

- Model download: Snap Hook
- Related blog post: Why All These Stresses and Strains?

The nonlinear stress-strain behavior in solids was already described 100 years ago by Paul Ludwik in his *Elemente der Technologischen Mechanik*. In that treatise, Ludwik described the nonlinear relation between shear stress and shear strain observed in torsion tests with what is nowadays called *Ludwik’s Law*:

(1)

\tau = \tau_0 + k\gamma^{1/n}

For , the stress-strain curve is linear; for , the curve is a parabola; and for , the curve represents a perfectly plastic material. Ludwik just described the behavior (*Fließkurve*) of what we now call a *pseudoplastic material*.

In version 5.0 of the COMSOL Multiphysics simulation software, beside Ludwik’s power-law, the Nonlinear Structural Materials Module includes different material models within the family of nonlinear elasticity:

- Ramberg-Osgood
- Power Law
- Uniaxial Data
- Bilinear Elastic
- User Defined

In the Geomechanics Module, we have now included material models intended to represent nonlinear deformations in soils:

- Hyperbolic Law
- Hardin-Drnevich
- Duncan-Chang
- Duncan-Selig

The main difference between a nonlinear elastic material and an elastoplastic material (either in metal or soil plasticity) is the reversibility of the deformations. While a nonlinear elastic solid would return to its original shape after a load-unload cycle, an elastoplastic solid would suffer from permanent deformations, and the stress-strain curve would present hysteretic behavior and ratcheting.

Let’s open the Elastoplastic Analysis of a Plate with a Center Hole model, available in the Nonlinear Structural Materials Model Library as *elastoplastic_plate*, and modify it to solve for one load-unload cycle. Let’s also add one of the new material models included in version 5.0, the *Uniaxial data* model, and use the stress_strain_curve already defined in the model.

Here’s a screenshot of what those selections look like:

In our example, the stress_strain_curve represents the bilinear response of the axial stress as a function of axial strain, which can be recovered from Ludwik’s law when .

We can compare the stress distribution after laterally loading the plate to a maximum value. The results are pretty much the same, but the main difference is observed after a full load-unload cycle.

*Top: Elastoplastic material. Bottom: Uniaxial data model.*

Let’s pick the point where we observed the highest stress and plot the *x*-direction stress component versus the corresponding strain. The green curve shows a nonlinear, yet elastic, relation between stress and strain (the stress path goes from ). The blue curve portraits a hysteresis loop observed in elastoplastic materials with isotropic hardening (the stress path goes from ).

With the Uniaxial data model, you can also define your own stress-strain curve obtained from experimental data, even if it is not symmetric in both tension and compression.

- P. Ludwik.
*Elemente der Technologischen Mechanik* - “Hypoelasticity“, Chapter 3.3 of
*Applied Mechanics of Solids* - Download the Elastoplastic Analysis of a Plate with a Center Hole model

The piezoelectric modeling interface seeks to:

- Make the modeling workflow more
- Transparent
- Flexible

- Enable you to debug the models more easily

This will allow you to successfully simulate piezoelectric devices as well as easily extend the simulation by coupling it with any other physics.

You may already be familiar with the three different modules that can be used for simulating piezoelectric materials:

Each of these modules gives you a predefined *Piezoelectric Devices* interface that you can use for modeling systems that include both piezoelectric and other structural materials. The Acoustics Module offers two predefined interfaces, namely the *Acoustic-Piezoelectric Interaction, Frequency Domain* interface and the *Acoustic-Piezoelectric Interaction, Transient* interface. These two allow you to model how piezoelectric acoustic transducers interact with the fluid media surrounding them.

*The *Piezoelectric Devices* interface is available in the list of structural mechanics physics interfaces.*

*The *Acoustic-Piezoelectric Interaction, Frequency Domain *and the* Acoustic-Piezoelectric Interaction, Transient* interfaces are available in the list of acoustics physics interfaces.*

These predefined multiphysics interfaces couple the relevant physics governing equations via constitutive laws or boundary conditions. Thus, they offer a good starting point for setting up more complex multiphysics problems involving piezoelectric materials. The new piezoelectric interfaces in COMSOL Multiphysics version 5.0 provide a transparent workflow to visualize the constituent physics interfaces. There is also a separate Multiphysics node that lists how the constituent physics interfaces are connected to each other.

Let’s find out how these multiphysics interfaces are structured.

Upon selecting the *Piezoelectric Devices* multiphysics interface, you see the constituent physics: *Solid Mechanics* and *Electrostatics*. You also see the *Piezoelectric Effect* branch listed under the Multiphysics node, which controls the connection between *Solid Mechanics* and *Electrostatics*.

*Part of the model tree showing the physics interfaces and multiphysics couplings that appear upon selecting the* Piezoelectric Devices *interface.*

By default, all modeling domains are assumed to be made of piezoelectric material. If that is not the case, you can deselect the non-piezo structural domains from the branch *Solid Mechanics > Piezoelectric Material*. These domains then get automatically assigned to the *Solid Mechanics > Linear Elastic Material* branch. This process ensures that all parts of the geometry are marked as either piezoelectric or non-piezo structural materials and that nothing is accidentally left undefined.

If you are working with other material models that are available with the Nonlinear Structural Materials Module, such as hyperelasticity, you can add that as a branch under *Solid Mechanics* and assign the relevant parts of your modeling geometry to this branch. The Solid Mechanics node gives us full flexibility to set up a model that involves not only piezoelectric material but also linear and nonlinear structural materials. The best part is that if these materials are geometrically touching each other, the COMSOL software will automatically take care of displacement compatibility across them.

If some parts of the model are not solid at all, like an air gap, you can deselect them in the Solid Mechanics node.

From the Solid Mechanics node, you will also assign any sort of mechanical loads and constraints to the model.

The Electrostatics node allows you to group together all the information related to electrical inputs to the model. This would include, for example, any electrical boundary conditions such as voltage and charge sources. By default, any geometric domain that has been assigned to the *Solid Mechanics > Piezoelectric Material* branch also gets assigned to the *Electrostatics > Charge Conservation, Piezoelectric* branch. If you have any other dielectric materials in the model that are not piezoelectric, you could assign them to the *Electrostatics > Charge Conservation* branch.

The *Multiphysics > Piezoelectric Effect* branch ensures that the structural and electrostatics equations are solved in a coupled fashion within the domains that are assigned to the *Solid Mechanics > Piezoelectric Material* (and also the *Electrostatics > Charge Conservation, Piezoelectric*) branch.

The multiphysics coupling is implemented using the well-known coupled constitutive law for piezoelectric materials. Note that the *Electrostatics > Charge Conservation, Piezoelectric* branch is mainly used as a placeholder for assigning geometric domains that belong to the piezoelectric material model. This helps the *Multiphysics > Piezoelectric Effect* branch understand whether a domain assigned to the *Electrostatics* interface is piezoelectric or not.

Note: For an example of working with the

Piezoelectric Devicesinterface, check out the tutorial on modeling a Piezoelectric Shear Actuated Beam.

It is also possible to add effects of damping or other material losses in dynamic simulations. You can do so by adding one or more of the following subnodes under the *Solid Mechanics > Piezoelectric Material* branch:

*Damping and losses that can be added to a piezoelectric material.*

Subnode Name | When to Use the Subnode |
---|---|

Mechanical Damping | Allows you to add purely structural damping. Choose between using Loss Factor (in frequency domain) or Rayleigh damping (for both frequency and time domains) models. |

Coupling Loss | Allows you to add electromechanical coupling loss. Choose between using Loss Factor (for frequency domain) or Rayleigh damping (for both frequency and time domains) models. |

Dielectric Loss | Allows you to add dielectric or polarization loss. Choose between using Loss Factor (for frequency domain) and Dispersion (for both frequency and time domains) models. |

Conduction Loss (Time-Harmonic) | Allows you to add electrical energy dissipation due to electrical resistance in a harmonically vibrating piezoelectric material (for frequency domain only). |

Note: For an example of adding damping to piezoelectric models, check out the tutorial on modeling a Thin Film BAW Composite Resonator.

Additional damping also takes place due to the interaction between a piezoelectric device and its surroundings. This can be modeled in greater details using the Acoustic-Piezoelectric Interaction interfaces.

Upon selecting one of the Acoustic-Piezoelectric Interaction interfaces, you see the constituent physics: *Pressure Acoustics*, *Solid Mechanics* and *Electrostatics*. You also see the *Acoustic-Structure Boundary* and *Piezoelectric Effect* branches listed under the Multiphysics node.

*Part of the model tree showing the physics interfaces and multiphysics couplings that appear when selecting the *Acoustic-Piezoelectric Interaction, Frequency Domain* and the* Acoustic-Piezoelectric Interaction, Transient* interfaces.*

By default, all modeling domains are assigned to the *Pressure Acoustics* interface as well as the *Solid Mechanics > Piezoelectric Material* and* Electrostatics > Charge Conservation, Piezoelectric* branches. Note that the *Pressure Acoustics* interface is designed to simulate acoustic waves propagating in fluid media.

Since COMSOL Multiphysics cannot know a *priori* which parts of the modeling geometry belong to the fluid domain and which ones are solids, you are expected to provide that information by deselecting the solid domains from the *Pressure Acoustics, Frequency Domain* (or *Pressure Acoustics, Transient*) branch and deselecting the fluid domains from the *Solid Mechanics* and *Electrostatics* branches.

Once you do that, the boundaries at the interface between the solid and fluid domains are detected and assigned to the *Multiphysics > Acoustic-Structure Boundary* branch. This branch controls the coupling between the *Pressure Acoustics* and *Solid Mechanics* physics interfaces. It does so by considering the acoustic pressure of the fluid to be acting as a mechanical load on the solid surfaces, while the component of the acceleration vector that is normal (perpendicular) to the same surfaces acts as a sound source that produces pressure waves in the fluid.

Note: For an example of Acoustic-Piezoelectric Interaction, check out the tutorial on modeling a Tonpilz Transducer.

The transparency in the workflow as discussed above also paves the way for adding more physics and creating your own multiphysics couplings.

For example, let’s say there is some heat source within your piezoelectric device that produces nonuniform temperature distribution within the device. In order to model this, you can add another physics interface called *Heat Transfer in Solids* in the model tree and prescribe appropriate heat sources and sinks to find out the temperature profile. You could then add a *Thermal Expansion* branch under the Multiphysics node to compute additional strains in different parts of the device as a result of the temperature variation.

The *Multiphysics > Thermal Expansion* branch couples the *Heat Transfer in Solids* and the *Solid Mechanics* interfaces. It might also be possible that the piezoelectric material properties have a temperature dependency. You could represent these properties as functions of temperature and let the *Multiphysics > Temperature Coupling* branch pass on the information related to temperature distribution in the modeling geometry to the *Solid Mechanics* or even the *Electrostatics* branches, thereby producing additional multiphysics couplings.

*Part of the model tree showing the physics interfaces and multiphysics couplings that you can use to combine piezoelectric modeling with thermal expansion and temperature-dependent material properties.*

Similar to adding more physics and multiphysics couplings, it is also possible to disable one or more multiphysics couplings — or even any of the physics interfaces shown in the model tree. This could be immensely helpful for debugging large and complex models.

*The model tree on the left shows a scenario where the Piezoelectric Effect multiphysics coupling is disabled. The model tree on the right shows a scenario where the* Electrostatics* physics interface is disabled.*

For example, you can disable the *Multiphysics > Piezoelectric Effect* branch and solve for the *Solid Mechanics* and *Electrostatics* physics interfaces in an uncoupled sense. You could also solve a model by disabling either the *Solid Mechanics* or the *Electrostatics* interface.

Running such case studies could help in evaluating how the device would respond to certain inputs if there were no piezoelectric material in place. This approach could also be used to evaluate equivalent structural stiffness or equivalent capacitance of the piezoelectric material.

You could also start by adding only one of the constituent physics, say *Solid Mechanics*, and after performing some initial structural analysis, go ahead and add the *Electrostatics* physics interface to the model tree once you are ready to add the effect of a piezoelectric material.

In that case, when you add the *Electrostatics* physics on top of the existing *Solid Mechanics* physics in the model tree, the COMSOL software will automatically add the Multiphysics node. From there, you can manually add the *Piezoelectric Effect* branch. Note that if you take this approach of adding the constituent physics interfaces and multiphysics effect manually, you would also have to manually add the piezoelectric modeling domains to the *Solid Mechanics > Piezoelectric Material*, the *Electrostatics > Charge Conservation, Piezoelectric*, and the *Multiphysics > Piezoelectric Effect* branches.

In a similar fashion, you can continue to add more physics interfaces and multiphysics couplings to your model based on your needs.

To learn more about modeling piezoelectric devices in the COMSOL software environment, you are encouraged to refer to these resources:

- Piezoelectric Features Overview
- Acoustics Module User’s Guide
- MEMS Module User’s Guide
- Structural Mechanics Module User’s Guide