In Part 1 of this blog series, we discussed some of the considerations that you need to make when transforming your measured material data into a constitutive model. Hyperelastic materials were discussed in some detail. Today, we will have a look at how to use nonlinear elastic and elastoplastic materials, and show one way in which you can use your measured data directly in COMSOL Multiphysics.

Some materials already exhibit significant nonlinearity at small strains. Cast iron and some ceramics show this behavior, for example. However, when unloaded from a moderate strain, they follow the same stress-strain path back to the original state, so the response is elastic. This calls for a nonlinear elastic model.

In the previous blog post, we discussed hyperelastic materials, so why not just use one of these models to fit the measured stress-strain curve for, say, a nodular cast iron? The answer is that the hyperelastic material models are tailored for large strains. In elastomers, you may have elongations of several hundred percent of the original length, whereas the elastic range of metals and more brittle materials is usually less than 1%.

The very popular Mooney-Rivlin model will, for example, be essentially linear for small strains, and is therefore not useful in this context. In the Ogden model, the stress is computed as a sum of powers of the stretches. But for small strains, the stretch may have a range from 0.999 to 1.001 or so. In order to predict a significant nonlinearity, the exponent in the power law would have to be extremely high. A stable fitting of data to such an equation is not feasible. At the low strains present in a brittle material, the engineering strain would be a more natural representation of deformation. You can read more about different stress and strain measures in the blog entry “Why All These Stresses and Strains?”

To cope with this situation, COMSOL provides a set of nonlinear elastic models intended for small strains. These material models require the Nonlinear Structural Material Module or the Geomechanics Module and are available in the *Solid Mechanics* and *Membrane* interfaces. Let’s investigate how you can use these materials.

*Selecting a nonlinear elastic material model in COMSOL Multiphysics.*

In total, there are nine nonlinear elastic material models. Some of them have a simple mathematical form determined by a few parameters. One material model is especially useful when dealing with experimental stress-strain data: *Uniaxial data*. This model is explicitly intended for analyses based on measured data. Let’s have a look at the settings for this model:

*The settings for the Uniaxial data nonlinear elastic model.*

The main input is a function relating the uniaxial stress to the uniaxial strain. In this example, the measured data is given in terms of an interpolation function, called `stress_strain_curve`

, but it could also have been an analytical expression. An interpolation function can be entered explicitly as a number of data points or it can be read from a file. Here, the import is made directly from an Excel® file. This requires the LiveLink™ *for* Excel® add-on, but it is also possible to read the data from tabulated text files.

*Imported uniaxial stress-strain curve.*

The uniaxial curve does not, however, provide enough information to completely define a multiaxial constitutive law. One more assumption is needed, which is why you have to provide either a constant Poisson’s ratio or bulk modulus. For many materials, a constant Poisson’s ratio with a value between 0.2 and 0.3 will provide a good approximation. This is all that is needed to complete the material model.

If you study the stress-strain curve above, you will notice that it is different in tension and compression. In a multiaxial stress state, however, a certain point in the material may experience tension in one direction and compression in another. So which branch of the material curve should then be used? The material model is isotropic, so it has the same stiffness in all directions, but it is the volume change that is decisive. If the local volume change is negative, the compression branch is used.

An isotropic nonlinear elastic material is only admissible from the theoretical point of view if:

- The mean stress (“pressure”) or bulk modulus is a function only of the volumetric strain.
- The shear stress or shear modulus is a function only of the shear strains.

If these conditions are violated, you can devise a stress-strain cycle from which it is possible to extract energy, that is, a *perpetuum mobile*.

All of the built-in materials are designed so that these conditions are fulfilled. If you take a look at the settings for the Bilinear elastic material, you will have to input the bulk moduli for this in tension and compression — not the Young’s moduli as you might have anticipated.

Most structural analysts work with Young’s modulus and Poisson’s ratio as the primary parameters for elastic materials. But the requirements above unfortunately mean that if Young’s modulus has a dependence on the strain, then…

- The function describing this dependency can only have some very specific forms.
- Poisson’s ratio must also be a function of strain, which leads to a function that is very difficult to express.

So how was it possible to enter the Uniaxial data above with a constant Poisson’s ratio? The answer is that we created behind-the-scenes allowable functions for the bulk modulus and shear modulus. No reference is made to Young’s modulus, even though that is what you would intuitively derive in the graph.

That said, I have seen quite a number of successful models where an analyst has introduced strain dependencies in the Young’s moduli for isotropic or orthotropic materials in an elastic material model. For practical engineering use, this may work fine. We supply an example of how to define a stress-dependent Young’s modulus in the Modeling Stress-Dependent Elasticity tutorial. The important point for such an approach to be acceptable is that the structure should be subjected to a mainly proportional loading (in the sense that the directions of the principal strains do not rotate).

*Cantilever beam with different values of Young’s modulus in tension and compression. The beam is subjected to a bending moment at the free end. The upper plot shows von Mises stress; the lower plot shows the current value of Young’s modulus.*

When you set out to model nonlinear elasticity by either using the built-in models or by your own expressions, it is important to keep a clear distinction between a *tangent stiffness* and a *secant stiffness*. A nonlinear elastic model is often expressed similarly to the linear model, but with a stress or strain dependence in the elastic constant (which is no longer a constant!). Assume that the shear stress \tau is related to the shear strain \gamma through

\tau = G_S(\gamma) \cdot \gamma

The shear modulus G_S(\gamma) is then a secant shear modulus. When the total strain is multiplied by the secant modulus, the result is the total stress. The tangent shear modulus G_T(\gamma), on the other hand, is the stiffness experienced for a small change in strain, as illustrated by the figure below.

Mathematically, the relation between the two moduli is

G_T(\gamma) = \frac{d \tau}{d \gamma} = G_S(\gamma) + \frac{d G_S(\gamma)}{d \gamma} \gamma

Your measured data will usually have the form

\tau = f(\gamma)

This means that the secant stiffness actually is

G_S(\gamma) = \frac{f(\gamma)}{\gamma}

When converting a stress-strain curve into secant form using this expression, special attention must be given to the possible zero-divide at zero strain.

Also, you may sometimes encounter the statement that a certain material has been fitted to a power law with a certain exponent *n*. This may either mean that

\tau = C \gamma^n

or that

G_s = C \gamma^n

The Power law model in COMSOL Multiphysics uses the former, more common definition, where the strain exponent *n* relates to the slope of the stress-strain curve in a semi-log plot.

A pure tension experiment cannot determine whether a certain measured nonlinearity is caused by plasticity or not. The unloading curve must also be investigated. This is illustrated by the animation below, taken from the previous blog post.

The use of a nonlinear elastic model to simulate plasticity has been explored in a previous blog post.

In addition to using the Uniaxial data model, the Ramberg-Osgood nonlinear elastic material model is specifically intended for use as a simple replacement for a full elastoplastic model. Using a nonlinear elastic material is significantly cheaper in terms of computer resources, but what are the limitations of such an approach?

- Obviously, only a continuous increase in the loading is allowed.
- If there are several external loads acting, for example a pressure load together with thermal expansion, these are usually not proportional to each other. This may cause the local stresses to be non-proportional.
- The three-dimensional response will usually not be the same, even if the uniaxial stress-strain curve is identical for a nonlinear elastic model and a full elastoplastic model. In metal plasticity, like a von Mises flow rule, plastic deformation preserves the volume. This will not be the case in a corresponding nonlinear elastic model.

When deciding upon a suitable material model, you must take into account the accuracy of the whole analysis. In engineering, we are often working with incomplete information, and there will be uncertainties in the loads, in the homogeneity of the materials, and in the actual dimensions of the structure. You will also introduce approximations by the selection of boundary conditions. It is the weakest link in the chain that determines the quality of the results, and that may well not be the exact mathematical foundation of the material model.

In the previous blog post, I stated that “it is not a good idea to just enter a simple stress-strain curve as input.”

So why did I change my mind today? The answer is that when working with the Uniaxial data model, it is the actual measurements that are used. For all hyperelastic models, and most of the other nonlinear elastic models, the measured data must be fitted to a mathematical model with a small number of parameters. It is this fitting that cannot safely be done without human supervision.

]]>We often get requests of the type “I would like to just enter my measured stress-strain curve directly into COMSOL Multiphysics”. In this new blog series, we will take a detailed look at how you can process and interpret material data from tests. We will also explain why it is not a good idea to just enter a simple stress-strain curve as input.

All material models are mathematical approximations of a true physical behavior. Material models can, however, not always be derived from physical principles, like mass conservation or equations of equilibrium. They are by nature phenomenological and based on measurements. The laws of physics will, however, enforce limits on the mathematical structure of material models and the possible values of material properties.

It is well known, even from everyday life, that different materials exhibit completely different behavior. A material can be very brittle, like glass, or very elastic, like rubber. Choosing a material model is not only determined by the material as such, but also by the operating conditions. If you immerse a piece of rubber into liquid nitrogen, it will become as brittle as glass — a popular educational experiment. Also, if you heat up glass, it will start to creep and show viscoelastic behavior.

When analyzing structural mechanics behavior in COMSOL Multiphysics, you can choose between about 50 built-in material models, many of them featuring several options for their settings. You can also set up and define your own material models, or combine several of the material models to, for example, describe a material exhibiting both creep and plasticity at the same time.

Some of the available classes of materials are:

- Linear elastic
- Hyperelastic
- Nonlinear elastic
- Plasticity
- Creep
- Concrete

Without going into details about how you should actually come to the correct decision about an appropriate material model, here are some questions you should ask yourself before you start modeling:

- How large are the stress and strain ranges?
- Will the loading speed be important?
- What is the operating temperature and will it be constant?
- Is there a predefined material model targeted specifically at my material, such as concrete or soil plasticity?
- Is the load constant, monotonously increasing, or cyclic?
- Is the stress state predominantly uniaxial or is it fully three-dimensional?

Based on these considerations, you can then make a choice of a suitable material model. Determining the correct parameters to use in this material model will then be more or less difficult.

On one end of the spectrum, there are common materials (such as steel at room temperature) where many engineers know the material data by heart (E = 210 GPa, *ν* = 0.3, *ρ* = 7850 kg/m^{3}) and where data is easily found in the literature or through a simple web search.

On the other end of the spectrum, finding the high temperature creep data for a cast iron to be used in an exhaust manifold can be a major project in itself. Many tests at different load levels and at different temperatures are required. A complete test program for this may take half a year and have a price tag of several hundred thousand dollars.

*Tensile testing equipment. “Inspekt desk 50kN IMGP8563″ by Smial. Original uploader was Smial at de.wikipedia — Transferred from de.wikipedia; transferred to Commons by User: Smial using CommonsHelper. (Original text: eigenes Foto). Licensed under CC BY-SA 2.0 de via Wikimedia Commons.*

Before starting your simulation with COMSOL Multiphysics, it is not enough to import the geometry of the specimen, select the material model, and apply the loads and other boundary conditions; you should also provide the parameters for the chosen material model in the operating stress-strain and temperature range. These parameters are typically obtained from one or more tests.

The most fundamental test is the *uniaxial tensile test*. This is also what most engineers in daily life refer to when they state that they have a “Stress-Strain curve.” If you look at the list of questions above, it is evident that even this seemingly simple test can leave many loose ends:

- A material may exhibit time dependence even at constant loads, giving creep or viscoelastic effects. Many tests, often at different temperature and stress levels, are needed to give reliable data.
- Material parameters obtained from an ordinary tensile test at low speed may not be representative of the material behavior at high strain rates. A crash analysis might show strain rates as high as 10 s
^{-1}, while conventional uniaxial testing machines can use strain rates as low as 10^{-3}s^{-1}. - Is the material isotropic or would tests in several directions be required?
- If you only have a tension test, what would happen in compression? With a single curve, you cannot really tell.
- A tensile test will supply stress versus strain in the tested direction, but it will not always contain data about the deformations in the transverse direction. Without that data, you have no information at all about the cross-coupling between the directions in the 3D case.
- When curve fitting experimental measurements, perhaps not all data should be given equal weight. It may so be that the response in a certain strain range has a larger impact on your simulation results.

Some materials, like concrete, have little or no capacity to carry loads in tension. Here, the *uniaxial compression test* is the most fundamental test. It has many properties in common with the tensile test.

Other materials, like steel and rubber, can also be tested in compression. It is actually a good idea to do so, as we will demonstrate later in this blog post.

When using only uniaxial testing (whether it is in tension, compression, or both), you can however not achieve the full picture of the properties of a given material. You will need to combine it with some other assumptions like isotropy or incompressibility. For many materials, such assumptions are well justified by experience, though.

We have illustrated how the range of a test will affect your conception of the material behavior in the animation below.

- If you just do the onloading part, it is not possible to discriminate between elastic and plastic behavior.
- By unloading, you can distinguish plastic from elastic behavior, but until the specimen is in a state of significant compression, it is not possible to determine whether an isotropic or a kinematic hardening model would give the best representation.

It is significantly more difficult to design testing equipment that can create a homogenous biaxial stress state. *Biaxial testing* is often used for materials that are available only in thin sheets, like fabrics, for instance. By controlling the ratio between the loads in two perpendicular directions, it is possible to extract much more information than from a uniaxial test.

For soils, which generally need to be confined, *triaxial compression* is a common test. Triaxial compression tests could in principle be applied to a block of any material, but the testing equipment is difficult to design. The low compressibility of most solid materials also makes triaxial testing less attractive, since the measured displacements will be small when the material is compressed in all directions.

The Triaxial Test model shows a finite element model of a triaxial compression test.

The *torsion test*, where a cylindrical test specimen is twisted, is a rather simple test that generates a non-uniaxial stress state. The stress state is, however, not homogenous through the rod. Therefore, some extra processing is needed to translate the moment versus angle results to stress-strain results.

In an upcoming blog post in this series, we will make an in-depth demonstration of how to fit measured data to a number of different hyperelastic material models. In the example here, we will assume that you have been able to fit your data to the tests. The raw data consists of two measurements: one in uniaxial tension and another in equibiaxial tension, as shown below.

The nominal stress (force divided by original area) is plotted against stretch (current length divided by original length).

*Measured stress-strain curves by Treloar.*

Since the data covers a wide range of stretches, the experimental results are clearly nonlinear. The simplest hyperelastic models with one or two parameters will probably not be sufficient to fit the experimental data. The Ogden model with three terms is a popular model for rubber, and it is the model we used here.

A least squares fit will give the results below when assigning equal weights to both data sets. As we can see in the graph, it is possible to fit both experiments very well with a single set of material parameters.

*Fitted material parameters using a three terms Ogden model.*

But what if the biaxial test had not been available? Fitting only the uniaxial data will give a different set of material parameters, which will of course fit that set of experimental data even more closely, but it would deviate from the biaxial results. This is shown below.

*Analytical results for uniaxial and biaxial tension when only the uniaxial data was used to fit the model parameters.*

Clearly, the prediction for a equibiaxial stress state will differ between the two sets of parameters. As we can see, the error in stress in the biaxial curve is more than 20% at some stretch levels.

What about other stress states? Two stress states that can be simulated in a simple finite element model are uniaxial compression and pure torsion. The uniaxial stress-strain curve over a wide range of stretches is shown below. The results on the tensile side are not as sensitive to the data set used for obtaining the material parameters as the compressive side is. This is not surprising as tensile data is used for parameter fitting in both cases, whereas neither of the experiments contain any information about the compressive behavior.

*Uniaxial response ranging from compression to tension. The scale on the *x*-axis is logarithmic.*

Note that operating conditions of rubber parts, such as seals, are often under predominantly compressive states. If the data sets used for parameter fitting contain only tension data, this may be a source of inaccuracy when modeling multiaxial stress states.

Finally, let’s have a look at a simulation where a circular bar is twisted. The same type of discrepancies between the results from two sets of material parameters as above can be seen below.

*Computed torque as function of the twist angle.*

Finally, it should be noted that many hyperelastic models are only conditionally stable. This means that even though the estimated material parameters are perfectly valid for a certain strain range, a unique and continuous stress-strain relation may not even exist for other strain combinations. We often come across such problems in support cases. This is unfortunately rather difficult to detect a *priori*, since it would require a full search of all possible strain combinations.

Measured data must be processed and analyzed before being used as input for simulations. For material models other than the simpler linear elastic model, it is a good idea to make small examples with a unit cube to assess the behavior under different loading states before using the material model in a large-scale simulation.

So the answer to the question: “I would like to just enter my measured stress-strain curve directly into COMSOL Multiphysics” is that such an approach is *not* recommended. That would make the software a black box where the user really must take a number of active decisions in order to obtain meaningful results.

Up next in our Structural Materials series: We will discuss nonlinear elasticity and plasticity.

]]>

With its notable display of historical artwork, the Louvre has become a central landmark in Paris, France. As the Louvre grew in popularity — eventually ranking as one of the world’s most visited museums — it became evident that the building’s original entrance could no longer handle the large number of guests admitted on a daily basis. The need for an entrance with a greater capacity prompted the construction of the Louvre Pyramid within the museum’s courtyard in 1989. This structure now serves as the main entrance to the building, descending visitors into a spacious lobby and then moving them up to the museum level.

*The Louvre Pyramid. (“Courtyard of the Louvre Museum, with the Pyramid” by Alvesgaspar — Own work. Licensed under Creative Commons Attribution Share-Alike 3.0, via Wikimedia Commons).*

In comparison to the Louvre’s classical architecture, the pyramid was based on a more modern design approach — the space frame. A *space frame* is a truss-like structure composed of interlocking struts that form a geometric pattern. Requiring few interior supports, these structures offer a lightweight and elegant solution in structural engineering. Additionally, due to their inherent rigidity, space frames are able to span large areas while maintaining a strong resistance.

The Louvre pyramid is just one example of a building based on a space frame design. Many other structures, such as the Eden Project in England and Globen in Sweden, have also used a space frame as the basis for their construction. With its common application in modern buildings, it is important to study how loads affect the stability of such structures.

In the new COMSOL Multiphysics version 5.0 model, Instability of a Space Arc Frame, we set up and analyze a space frame. In this benchmark model, the frame undergoes concentrated loading at various points, with a small lateral load implemented to break the structure’s symmetry. The description of the space frame and the applied loads are based on the example from “A Mixed Co-rotational 3D Beam Element for Arbitrarily Large Rotations” by Z.X. Li and L. Vu-Quoc.

*A schematic depicting the space frame’s geometry.*

As a constraint, all of the frame’s base points are pinned. Vertical concentrated loads P are applied to the top four corners of the space frame. Meanwhile, lateral loads of 0.001*P are applied to the frame’s two front corners. These lateral loads are designed to perturb the frame’s symmetry to implement a controlled instability. The figure below shows the final state of the deformed frame.

*Deformed space frame.*

Next, we can evaluate the relationship between the compressive load and the horizontal displacement on point A of the frame. Comparing the reference data with the simulation results, the plot below illustrates a strong agreement between the two findings.

*A plot relating load parameter P and displacement v. Here, the simulation results are compared with the reference data.*

Furthermore, this plot highlights an instability occurring at a parameter value of around 8.0, even though a deviation from linearity can be seen much earlier. In practice, an imperfect structure’s critical load is often far lower than that of the ideal structure, as was discussed in this previous blog post.

- Download the model: Instability of a Space Arc Frame

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 \tau and shear strain \gamma observed in torsion tests with what is nowadays called *Ludwik’s Law*:

(1)

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

For n=1, the stress-strain curve is linear; for n=2, the curve is a parabola; and for n=\infty, 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 n=1.

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 a\rightarrow b \rightarrow a \rightarrow c \rightarrow a). The blue curve portraits a hysteresis loop observed in elastoplastic materials with isotropic hardening (the stress path goes from a\rightarrow b \rightarrow d \rightarrow e ).

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

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.

]]>

First, let us have a look at the interfaces available in the Structural Mechanics Module. The following table lists the interfaces, their space dimension, geometric entity, and the type of structures they are intended for.

Interface | Space Dimension | Geometric Entity | Type of Structure |
---|---|---|---|

Solid Mechanics | 3D, 2D, 2D Axisymmetry | Domain | Any structure |

Shell | 3D | Boundary | Thin flat or curved structures with significant bending stiffness |

Plate | 2D | Domain | Thin flat structures with significant bending stiffness |

Membrane | 3D, 2D Axisymmetry | Boundary | Membranes without bending stiffness, usually prestressed |

Beam | 3D, 2D | Edge (3D), Boundary (2D) | Slender members with significant bending and torsional stiffness |

Truss | 3D, 2D | Edge (3D), Boundary (2D) | Slender members that can sustain only axial forces; cables |

Suppose we want to model a reading table using COMSOL Multiphysics.

For modeling such a table, we could use the *Solid Mechanics* interface and model the full 3D problem. This would, however, lead to a model with a very large number of small finite elements. It is more appropriate to model it as a combination of the *Beam* and *Shell* interfaces. In that case, we’d use the *Beam* interface for the legs of the table and the *Shell* interface for the tabletop surface.

The figure below, on the left, shows the solid geometry of the table. On the right, the geometry is, instead, created with the *Shell* and *Beam* interfaces. It consists of a 3D boundary for the top panel of the table, to be modeled with the *Shell* interface, and 3D edges for the legs of the table, to be modeled with the *Beam* interface.

*Left: Solid geometry of a reading table. Right: Geometry created with the* Shell *and* Beam *interfaces*.

More examples where a combination of structural interfaces can be used are:

- Structures that are thin in large regions but more three-dimensional at certain locations. A mixture of solids and shells can then significantly reduce the model size.
- Plates or shells having beams as stiffeners.
- Truss elements acting as reinforcement bars in a concrete structure.
- A thin layer of one material on top of another material. In this case, an idealization with shells or membranes covering the boundary of a solid can be useful.

How can we couple these interfaces in a model? Well, the answer is that in COMSOL Multiphysics, there are a number of possible ways to do this. Which method we choose mainly depends on the type of problem at hand. Next, we’ll have a look at these methods, one by one, and discuss the types of problems they can be used with.

In order to illustrate the built-in coupling features, let’s consider the Model Library example of a Pratt truss bridge (also available online in the Model Gallery), which is modeled using the *Shell* and *Beam* interfaces. The figure below shows the geometry of a Pratt truss bridge. Here, 3D edges, shown in black, are modeled using the *Beam* interface and 3D boundaries, shown in gray, are modeled using the *Shell* interface.

*Geometry of a Pratt truss bridge, modeled using the* Beam *and* Shell *interfaces*.

To couple the *Shell* and *Beam* interfaces in this model, we have utilized the built-in Beam-Shell coupling feature. Below, I have summarized the steps for using a Beam-Shell coupling:

- In the
*Beam*interface, use the Shell Connection nodes for the edges that are common to the*Shell*and*Beam*interfaces.

- In the
*Shell*interface, use Beam Connection nodes on the common edges. You can also define an offset in the connection in the settings window. This is done to account for the fact that, in real life, the supporting beams are located below the concrete roadway.

The following built-in couplings are available and can be used in a similar manner as described above:

- Shell Edge to Solid Boundary (3D)
- Shell Boundary to Solid Boundary (3D)
- Beam Point to Solid Boundary (2D)
- Beam Edge to Solid Boundary (2D)
- Beam Edge to Shell Edge (3D)
- Beam Point to Shell Boundary (3D)
- Beam Point to Shell Edge (3D)

Another way of coupling different physics interfaces is through a Prescribed Displacement node, where the displacement is forced to be the same as the displacement in another physics interface. An example of this coupling is the Model Library example of a concrete beam with reinforcement bars (also in the Model Gallery).

The figure below shows the geometry of the model. Here, the concrete (3D Domain, gray colored) is modeled using the *Solid Mechanics* interface, while the reinforced bars (3D Edges, black colored) are modeled using the *Truss* interface.

*Geometry of a concrete beam that’s reinforced with steel bars. It was modeled using the* Truss *and* Solid Mechanics *interfaces*.

In this model, individual rebars are modeled by adding a *Truss* interface to the *Solid Mechanics* interface, which was used for the concrete beam. The model uses a General Extrusion coupling operator, to make the displacement variables in the *Solid Mechanics* interface available for the *Truss* interface. The Prescribed Displacement node is then used in the *Truss* interface to provide the displacement variables from the *Solid Mechanics* interface, using the General Extrusion coupling operator that was defined earlier.

In this model, the mesh for the truss elements is not related to the mesh for the solid elements. The rebars just pass through the solid elements. This is why the coupling operator is needed.

Another modeling strategy would be to let the edges needed for the truss elements also be a part of the definition of the solid geometry.

Perhaps the easiest coupling method is to rename the displacement degrees of freedom so that these are the same for the interfaces that are to be coupled. This is sufficient, for example, when using membranes as cladding on a solid boundary or truss elements as reinforcement bars in a solid. Do note that this method works only when there is a union between the geometric entities of the structural interfaces being coupled.

Also notice the following exceptions:

- The shape functions used in the
*Beam*interface have special properties. A beam cannot have the same degrees of freedom as another physics interface if the same edge or boundary is shared. - The representation of rotations differs between the
*Shell*and*Plate*interfaces and the*Beam*interface. Therefore, it is not possible to use common degree of freedom names for the rotational degrees of freedom.

Let’s apply this method to our model example of a concrete beam with reinforcement bars. We will modify the model to work with the same dependent variables for the *Solid Mechanics* and *Truss* interfaces. Follow the instructions below to solve the problem by renaming the dependent variables of the *Truss* interface.

- In the current implementation of the model, there is an assembly of bars and a solid domain. We need to make a union of the edges and the solid domain in the geometry section.

- Rename the dependent variables in the settings window of the
*Truss*interface.

- Delete or disable the Prescribed Displacement 1 node in the
*Truss*interface.

- Use a Physics controlled mesh.

We can now recompute the studies.

An Attachment feature (requires the Multibody Dynamics Module) is available for the *Multibody Dynamics*, *Solid Mechanics*, *Shell*, and *Beam* interfaces. The attachment formulation is similar to the rigid connector, and all the selected boundaries or edges behave as if they were connected by a common rigid body. The various joints available with the Multibody Dynamics Module use these attachments to couple the interface with any other interface.

To clarify this method, let’s have a look at the Model Library model of vibrations in a washing machine assembly (also in the Model Gallery). In this model, a horizontal axis washing machine is modeled using the *Multibody Dynamics* and *Shell* interfaces. The outer housing of the assembly (gray colored) is made up of shell elements, while the inner components (differently colored) are rigid and are modeled using Rigid Domain nodes in the *Multibody Dynamics* interface.

*Geometry of a horizontal axis portable washing machine, which was modeled using the * Multibody Dynamics *and* Shell *interfaces (top, bottom, front, and left panels of the housing are hidden for better visualization).*

To couple the two interfaces, attachments are first created in the *Shell* interface. The instance below shows the attachment nodes created in the *Shell* interface.

After defining the attachments in the *Shell* interface, fixed joints are created in the *Multibody Dynamics* interface. These fixed joints use the attachments from the *Shell* interface as the source and rigid bodies from the *Multibody Dynamics* interface as the destination, which results in a coupling of the two interfaces.

The screenshot below shows the settings window of one of the fixed joints with an attachment from the *Shell* interface as the source of the joint, and a Rigid Body node from the *Multibody Dynamics* interface as the destination of the joint.

A similar procedure is used to model the front and back springs present on the front and back panels of the housing. Have a look at the Model Gallery (or in the Model Library) entry called Vibration in a Washing Machine Assembly for more details about this model.

Whenever there are multiple interfaces in a model, the default solver will generate a segregated solver sequence. However, it is not possible to solve a coupled model if the structural mechanics degrees of freedom are placed in separate segregated groups. The solution is to either replace the segregated solver with a fully coupled solver or place all structural mechanics degrees of freedom in one segregated step.

Apart from the models discussed above, the below models also demonstrate the coupling of structural interfaces:

]]>

Conducting the structural analysis of a model is an imperative step in the design process. The Structural Mechanics Module, an add-on to COMSOL Multiphysics, offers a virtually limitless amount of capabilities for you to do just that.

This video introduces you to the Structural Mechanics Module and walks you through the entire model-building process for setting up and solving a mechanical problem. This includes demonstrations on how to create parameters, named selections for different parts of your geometry, local variables to implement complicated expressions defined in the model, custom meshes, and tabulated results. To demonstrate the workflow for building and solving a structural mechanics problem, the COMSOL Multiphysics version 4.4 tutorial model of a static bracket assembly is used.

The smallest components, while often overlooked in design, can be the most instrumental ones. Brackets serve as a core component of support for many mechanical devices in numerous industries. In this model, a bracket assembly is fixed in place through eight mounting bolts. A load is applied on the two arms of the bracket, which is representative of a pin being placed between the holes in the bracket arms. As a result, the two bracket holes will experience a loading from this pin. After an initial analysis is complete, the direction of the pin load is varied through a parametric sweep to see the variations in force exertion, stress distribution, and deformation.

- Shown in the video: Bracket — Static Analysis (version 4.4)

*Today, we will be learning how to model a structural mechanics problem, in COMSOL Multiphysics. We will conduct a static analysis of a bracket assembly, and in the end, perform a parametric sweep to analyze a bearing load at different angles. So let’s get started.*

We start our modeling by opening COMSOL Multiphysics, bringing us to the New window. Here we have two options for setting up our model. Use the Model Wizard as a guide for specifying the dimension, physics, and studies you want, instead of starting with an empty model. Here we select our space dimension. When modeling in Structural Mechanics, we can work in 3D, 2D, or 2D axisymmetry, but not 1D or 0D. With our model being three-dimensional, choose 3D for the space dimension.

We are brought to the Select Physics window in the Model Wizard. Here we can add the physics that our model will exhibit. When it comes to choosing physics, this is completely dependent on the model and what meaningful information you are trying to extrapolate from the results. It is advantageous to familiarize yourself with all the physics interfaces available to you, because you may want to add more physics that are relevant to your model later on. Since we are doing a structural analysis of a 3D solid, we go under the Structural Mechanics branch, select Solid Mechanics, and add it to our model. Click Study to enter the Select Study window.

There are several different types of studies to choose from, as shown, depending on the physics interfaces used within the model. Selection of the study type is completely dependent on your analysis objectives. For example, in the case of our bracket model we want to compute deformations and stresses at static equilibrium; so the properties are time-independent. Therefore, under Preset Studies we select Stationary. After clicking Done, you are brought to the COMSOL Multiphysics desktop.

To create parameters and constants in COMSOL Multiphysics in the ribbon, add Parameters. Here we define the parameters and constants that we’ll be using later in this model, which are stored in this table.

Before we add the parameters let’s take a look at the problem we are modeling to have an understanding of where our parameters are derived from. We have a bracket, where the mounting bolts of the assembly are assumed to be fixed, and securely bonded to the bracket itself.

*A pin is placed between the two holes in the bracket arms, and the inner surfaces of the two bracket holes will experience a loading from this pin. We will want to vary the direction of the pin load to see the variations in stress distribution and deformation. After an initial analysis is done with the pin load applied to the bracket holes along the negative *y*-axis at zero degrees, we will perform a parametric sweep of the pin load direction, starting at 0 degrees, and rotating 45 degrees, up to 180 degrees. “theta0” will be used to specify the main direction of the load, and will be the parameter used later in our parametric sweep. “P0” is the peak load intensity applied to the bracket holes. Lastly, “y0” and “z0” are the coordinates of the centers of the bracket holes. It’s good practice to use parameters instead of just the numerical values. When you change these global parameters, they will update throughout the entire model.*

Creating a geometry in COMSOL Multiphysics can be done three different ways. The geometry can be manually created within COMSOL, it can be imported from a file, or you can synchronize the geometry you have open in a CAD program to COMSOL, through any of the LiveLink interfaces. In this example, the assembly of both the bracket and mounting bolts, are available to be imported. In the Geometry section of the ribbon, click Import. Change the Geometry import type to COMSOL Multiphysics file and Browse to where the “bracket.mphbin” file is stored on your computer. This should be located in your COMSOL folder under models, Structural Mechanics Module, and then Tutorial Models. Select the file, click Import, and the geometry will appear in your graphics window.

In the Model Builder Window, under the Geometry node, you can see the Form Union node which is the default setting for finalizing your geometry into COMSOL Multiphysics. Since we are dealing with a set of domains that are assumed to be perfectly bonded to each other, and will not move relative to each other, we use the default Form Union to finalize the geometry. Click Build All.

Creating definitions in COMSOL Multiphysics will help simplify your model, especially when working with large and or complicated geometries. Let’s take a look at a few of the options.

Go to the ribbon, and under the Definitions tab, in the Selections section, add a Box. Box selections allow you to create groups of geometric entities partially or completely inside the box, that would have the same features applied to them. This makes the process of changing materials, model equations, boundary conditions or constraints to different parts of your model much easier to do. In this example we want to make two box selections: the first is for the bolt domains, and the second is for the load-bearing boundaries of the bracket holes.

In the Box settings window find the Box Limits section. Here we can change the limit values which will serve as the dimensions of the box. We want to change these limit values so that the bolts are contained within the box. Under the Output Entities section, in the Include entity if list, choose Entity inside box.

Click the Wireframe Rendering button on the Graphics toolbar and we see in fact that the bolt domains are selected.

We can add a second box, or a cylinder selection to select the bracket hole boundaries, but we will instead add an explicit selection. From the level list, choose Boundary, in the graphics window, select any one of the interior boundaries of one of the bracket holes. Now we can check the box for Group by continuous tangent, and the rest of the interior boundaries will automatically be selected. In the graphics window, select any one of the boundaries of the other hole, and all four of the boundaries will be added.

*Now that we’ve added selections to our model, we can define expressions for adding the boundary load. Local Variables can be used to introduce short and descriptive names for the complicated expressions defined in the model. Go to the ribbon and under the Definitions tab click Local Variables. In the table to define the load, we need an expression for the angle and load intensity, so we enter the following. The angle variable is used to help define the load intensity. This expression evaluates the radial angle, based on its position along the global *z*-coordinate. Since our loading direction will change in only in the *y* and negative *z* directions; or equivalently the 3 ^{rd} and 4^{th} Cartesian quadrants, we can have COMSOL Multiphysics solve for the angle, by computing the four-quadrant inverse tangent. This enables calculating the arctangent in all four quadrants. The load that the bracket holes experience will be sinusoidal in nature, so the sine function is used. This last part of this expression is added to make sure that the load is only applied to the bottom half of each bracket hole.*

*COMSOL uses a global Cartesian coordinate system by default to specify material properties, loads, and constraints in all physics interfaces and on all geometric entity levels. For this model we want to define the orientation of the load applied to the bracket holes. Since the load direction will be rotating about the negative *z*-axis, we need to create a rotated coordinate system. In the Coordinate Systems section of the ribbon, choose Rotated System. This creates a rotated coordinate system, relative to the global system, that defines the orientation of the load applied to the bracket holes. Under the Euler angles subsection, in the beta field type “-theta0”.*

COMSOL Multiphysics comes with a Material Browser, complete with built-in material properties for common materials, as well as materials for specific applications, and any materials created by you, the user. The addition of the Material Library grants users access to the entire COMSOL Multiphysics database of materials. Under the Built-In node, scroll down to select Structural Steel, click Add to Component, and we are done. The material has been automatically assigned to all domains. Here we can see the properties of the newly assigned material. You are free to create your own materials using the New Material function, and you can also use the Add Material button to stay within the main user interface.

Defining the physics and boundary conditions in COMSOL is made as easy as possible, to let you focus on what matters, the physics. To start go to the ribbon and click the Physics tab. Each selection level comes with the various physical properties that can be applied. You can learn about each physical property by adding it, and clicking the Help button in the top right corner of the window.

We first want to set the constraints acting on the structure. Since the mounting bolts are fixed in place, click on the Domains button and add a Fixed Constraint. Under the Domain Selection section from the Selection list, choose Box 1. This assumes that the bolts are rigid and the displacements are perfectly constrained. Next, we want to define the loads acting on the structure. Since the inner surfaces of the bracket holes experience the pin load, in the Physics tab, click the Boundaries button and choose Boundary Load. Choose Explicit 1 for the Selection. Under the Coordinate System Selection section, from the Coordinate System list, choose Rotated System 2, setting the load orientation with a value of “theta0”. Under the Force section, specify the Load vector with the following.

Whenever building a finite element model, we may want to customize the mesh if we anticipate that higher accuracy is needed in some parts of the model. Although we can solve this model with the default mesh, I will demonstrate how to use the mesh settings to get a finer mesh in some regions. In the ribbon, go to the Mesh tab and select Mesh 1. This shows the bracket geometry with the default Normal mesh applied. Although the elements appear as having straight sides, the default mesh used for solid mechanics problems is a second order, or quadratic, mesh. This means that the elements are conformal to the curved geometry.

We will create a second mesh and customize the mesh via the Element size parameters. Click the Add Mesh button. In the Mesh settings window, change the sequence type to User-controlled mesh. This will generate a Size sub node under our second Mesh. Click the Size node. Under the Element Size section, click on Custom. This automatically expands the Element Size Parameters window where the element parameters can be changed. Reducing the Curvature factor to “0.3″ and rebuilding the mesh, results in a finer mesh around the bracket holes. Rotating the geometry, and zooming in on a bolt, we can see the mesh is quite coarse around these small curved faces. The Minimum element size parameter is preventing the changes from the curvature factor. Reduce it to “0.005″ and rebuild the mesh. The elements around the curved edges are now smaller, but the bulk of the geometry remains relatively unchanged.

You can continue to refine the mesh manually if you want. It is also possible to use Adaptive Mesh Refinement to let the software automatically refine and coarsen the mesh, if desired. For the purposes of this example, we will continue with the default Normal mesh size setting.

We continue our simulation with creating a mesh using the default options. Go to the ribbon and in the Home tab, click Build Mesh. Then, in the Study section, click on the eye glasses icon labeled Study 1. Notice the Generate default plots check box. This will create a plot automatically, based on the structural mechanics physics, so in this case, a Stress plot will be created. To solve a stationary study in COMSOL, it is as simple as clicking Compute. COMSOL Multiphysics also defines a solver sequence for the simulation based on the physics and the stationary study type.

After a model has solved in COMSOL, it is time to postprocess the results. We will show you how to add to an existing plot, create a new plot, and extract information from the results.

Here we see the von Mises stress in the bracket and an exaggerated picture of the deformation, which is occurring mostly in the bracket arms. We also want to visualize the plot with vectors, so we can better see the pressure distribution on the inner surfaces of the bracket holes. Under the contextual Stress tab, in the Add Plot section click Arrow Surface. In the Arrow Surface settings window you’ll see an Expression section. From the menu choose Solid Mechanics, Load, and then Spatial load. In the Coloring and Style section, under Number of arrows, the default setting is 200. Increasing the number of arrows will give you a larger volume of arrows that are smaller in size, but heavier in concentration, which allows you to better visualize the load on the bracket holes. Go ahead and experiment with the number to see this yourself. Three thousand seems to give a quality visual. You can now see the load that was applied is displayed.

In this model we’ll also be interested in any displacement that occurs within the bracket geometry. To make a plot showing this, go to the ribbon and in the Results tab under Plot Group, click 3D Plot Group. This will open the newly generated 3D Plot Group 2 contextual tab in your ribbon. In the Add Plot section, click on Surface. The plot for the total displacement experienced by the bracket is automatically generated. Go to the ribbon, and under the Results tab you’ll see different dimensional types for plot groups. In this example we stick to two plot groups, but you are virtually limitless as you can make as many 3D, 2D or 1D plot groups you want for any type of visualization desired.

*Because the mounting bolts are fully constrained, use a volume integration over those domains to accurately calculate the reaction forces. On the Results tab, click More Derived Values and choose Integration, Volume Integration. In the Volume Integration settings window, locate the Selection section and from the Selection list, choose Box 1 to add the bolts. Click Replace Expression here in the upper-right corner of the Expression section, and from the menu choose Solid Mechanics, Reactions, Reaction Force, and the *x* component of the reaction force. Click the Evaluate button. Let’s do this again for the *Y* and *Z* components as well. To save time you can edit the expression, in this case, by changing the component letter.*

*Click Evaluate and the results are shown in Table 1 under the Graphics window. They match what we would expect them to be; the entire load is in the *y* direction while negligible in the *x* and *z* directions.*

It’s often necessary to solve several iterations of a model to find the optimal properties for its design. Instead of manually changing parameter values, and resolving each time, a parametric sweep can be used. A parametric sweep allows you to change the values of a parameter by sweeping the parameter values through a range defined by the user.

Adding a parametric sweep to this model will enable us to solve for different load angles. Go to the ribbon, and in the Study tab, click Parametric Sweep. In the Parametric Sweep window, under the Study Settings section, click the plus sign button to add the load direction as a parameter. To the right of that, click the Range button to define the range for this sweep. We’ll start at zero degrees, and rotate the load forty-five degrees, up to 180 degrees. Click Add and then the Compute button to re-solve the model.

We are automatically brought back to our stress plot. In the 3D Plot Group window, under Data you’ll notice the Parameter value list. Now we have the five different solutions dependent on the angle of the load and can alternate between them by selecting the different values and then clicking Plot.

*After performing a parametric sweep, you can create a table that lists the solutions for each parameter value. This way you can view the different solutions all at once. In the Volume Integration 1 node, click Evaluate and then New Table. The reaction forces at the different parameter values are computed. The reaction force in the *x*-direction is always zero, while the *y* and *z* directions share the load, depending on the angle.*

Traditionally, the way to calculate the effective mass of a particle is to push on it and measure how it reacts to the applied force. One University of Alberta research team (Brad Hauer, Callum Doolin, Kevin Beach, and John Davis) uses simulation as an efficient and noninvasive tool to achieve thermomechanical calibration.

According to Hauer, “The proper calibration of resonators is extremely important, especially in industries where precision is nonnegotiable.”

Because of its accuracy, thermomechanical calibration enables equipment to function both correctly and optimally. The thermal motion of a resonator is proportional to its energy, which is in turn proportional to its effective mass and time-dependent displacement squared. The computation of the effective mass takes into account both the mass and mode shape, and consequently, the displacement of a resonator. Simply put, an accurate prediction of the effective mass of a resonator design allows for proper calibration.

Atomic force microscopy is one field in which very fine measurements are needed. Atomic force microscopy is a way for instruments to inspect surfaces. It works by creating high-resolution images of objects by running a physical probe along them. One downside to this process is that measurements can be completely thrown off by manufacturing errors in the equipment. A device as sensitive as an atomic force microscopy tip requires precise calibration.

The University of Alberta researchers analyzed the fundamental mode shape with the Eigenfrequency Study available in the Structural Mechanics Module. They then derived the effective mass by performing a volume integration of the resonator’s density multiplied by the normalized displacement squared over its entire geometry.

*Simulation of atomic force microscopy tip mode shapes, where light reflected off a cantilever is measured by a photodiode.*

With so many kinds of sensors in use that need to be calibrated, it is a huge benefit to be able to model all geometries in the same software. In the future, the researchers at University of Alberta will work on some cutting-edge designs involving optomechanics. Naturally, they will continue to use COMSOL Multiphysics® to model their designs.

There is a broad range of uses for companies working with nanostructures, nanostrings, and everything in between. The best part is that anyone with the Structural Mechanics Module can get the effective mass of nanoelectronic and nanomechanical devices in a more efficient and scalable way.

*A force transducer able to measure force in increments as small as Attonewtons (10 ^{-18}N).*

- Check out the University of Alberta paper: “Effective Mass Calculations Using COMSOL Multiphysics for Thermomechanical Calibration“
- Familiarize yourself with the Structural Mechanics Module

When a structure undergoes vibrations, its components experience stresses and strains, which are amplified by the excitation of the natural frequencies of the structure. In addition to potential damage to the structure itself, these oscillations can also be a source of discomfort and disruption for occupants.

Whether a rare or persistent hurdle, seismic and wind-induced vibrations, and their effects, are an important consideration in the design process. *Damping* is one influence that has proved valuable in helping to reduce such vibrations, particularly in tall buildings and bridges, and preserve the longevity of these structures.

Did you know that you can model viscoelastic structural dampers using COMSOL Multiphysics? To get you started, we have created a tutorial model. The Viscoelastic Structural Damper model can be found in the Model Gallery as well as within the Structural Mechanics Module Model Library.

The model first analyzes the frequency response of a viscoelastic structural damper. Comprised of two layers of viscoelastic material, the damper is restrained between steel mounting elements.

*Image depicts the two layers of viscoelastic material in bold, with the steel mounting elements shown in light gray.*

Here, two of the mounting elements are subjected to periodic forces, with frequencies ranging from 0 to 5 Hz. Meanwhile, one of the mounting elements remains fixed. The figure below shows the displacement of the damper at 5 Hz. The second figure highlights the relationship between the applied frequency and the storage modulus and loss moduli, a representation of the viscoelastic properties of the material.

*Displacement at 5 Hz.*

*Plot of storage (blue line) and loss moduli (green line).*

Next, we can run a transient analysis to find out the displacement field as a function of time, as seen in the figure below.

*Surface plot of the z-component of displacement field after 1 second of forced vibrations. *

Plotting the applied force versus the displacement at one of the loaded points shows hysteresis loops, which are characteristic for damped problems. Energy is dissipated since the force and displacement are out of phase with each other.

*2D plot relating the displacement to the applied force.*

With the use of COMSOL Multiphysics, Tingcheng Wu, Guillaume Escamez, Clement Lorin, and Philippe J. Mason from the Department of Mechanical Engineering at the University of Houston were able to perform simulations to analyze how individual components of the structure impacted its overall performance. By applying various parameters to the structural design, they were able to conclude which factors had the greatest effect on the machine, both structurally and thermally. Thus, they could determine how to achieve a balance between the two.

The team of researchers modeled the structure as a rotor shaft separated into five individual parts connected by bolts. As a means to provide thermal insulation, different materials were used on particular areas of the shaft, as you can see below.

*Bolts were used to connect stainless steel with G10, a glass fiber material characterized by low thermal conductivity and a high yield stress. Image by T. Wu, G. Escamez, C. Lorin, and P. Mason, and taken from their poster submission.*

Seeking to analyze the issues of heat transfer and solid mechanics in these machines, the researchers used the Heat Transfer Module and Structural Mechanics Module to create their simulations. The figure below highlights the team’s findings regarding temperature, depicting that the G10 components take on the greatest temperature gradient.

In the next figure, the connection bolts underwent the most stress within the structure, a factor that was found to decrease as the cross-section area was decreased.

*Simulations highlight the thermal and structural pressure that the shaft endured, especially along its connection bolts. Image by T. Wu, G. Escamez, C. Lorin, and P. Mason, and taken from their presentation.*

With the continued funding and efforts of NASA and other research teams, progress continues to be made in the design of aircraft. As torque transfer components within fully superconducting rotating machines continue to be optimized, researchers gain momentum in their quest for developing structures with greater power densities and the potential for electric propulsion. In addition to making air travel a quieter and more energy efficient process, implementing this technology paves the way for its potential use within modes of ground transportation as well.

- Access the paper, presentation, and poster: “FEA Mechanical Modeling of Torque Transfer Components for Fully Superconducting Rotating Machines“