Let’s consider a symmetric two-bar structure under a compressive load, as shown in the following figure:

*Two bars under compression.*

We assume that the bars are linearly elastic so that the force in a bar, *F*, is

F=EA \frac{\Delta}{L_0}

where Δ is the elongation and *L*_{0} is the original length.

Using Pythagoras’ theorem, the vertical force can then be written as an explicit function of the vertical displacement:

P = EA \left(\sqrt{1-\kappa^2\delta(\delta-2)}-1 \right) \frac{\kappa(1-\delta)}{\sqrt{1+\kappa^2\delta(\delta-2)}} \approx EA \kappa^3\delta(\delta-2)(\delta-1)

The following quantities have been nondimensionalized:

- The normalized displacement , where is the deflection under the load. Thus, when the bars are horizontal and when the structure is upside down.
- The parameter is the aspect ratio: the initial height relative to initial bar length.

The force as a function of displacement is shown in the graph below. The example actually shows as a buckling problem with snap-through. Between points A and C, no unique solution exists. In a previous blog post, we further discuss the concept of buckling in structures.

The compressive force in the bars increases until they are horizontal (), but the vertical projection decreases even faster beyond point A. This is why the vertical force decreases.

*Force as a function of vertical displacement.*

If we build a finite element model of this structure and try to increase the load, the analysis will probably fail when we reach the first peak at point A. We can, however, easily trace the solution by prescribing the vertical displacement at the loaded point, rather than the force. The applied force can then be obtained as the reaction force. The graph above was created using that method.

The tangential stiffness for this single degree of freedom system is defined as the rate of change in force with respect to displacement:

k_{\mathrm t} = \frac{dP}{dw} = \frac{EA \kappa^3}{h}(3\delta^2-6 \delta+2)

The stiffness is thus negative between points A and B. A negative stiffness is often related to numerical and physical instabilities.

*Stiffness as a function of vertical displacement.*

There are several material models within the field of solid mechanics that contain a negative slope of the stress-strain curve, either as an intentional effect or with certain choices of parameters. For example, some models for concrete are designed like this. In the physical interpretation of this behavior, cracks form when the material model is loaded in tension. The load carried by a test specimen will then decrease. The cohesive zone models used for describing decohesion in the COMSOL Multiphysics® software also show this type of behavior.

*A strain-softening material.*

At the material level, decreasing stress with increasing strain indicates a negative stiffness:

\frac{d\sigma}{d\epsilon} < 0

Such a material can only be tested under a condition of prescribed displacement; otherwise, it will fail immediately when the peak load is reached. The negative stiffness is thus related to a material instability.

In general, the stress and strain states are multiaxial. Stress and strain are represented by second-order tensors. In the multiaxial case, we must use a more general criterion for material stability: For any small change in the strain state, the corresponding change in the stress state must be such that the sum of the products of all stress and strain components is positive. That is,

d \boldsymbol{\sigma}: d \boldsymbol{\varepsilon} >0

Or, written in component form,

\sum_{i=1}^3\sum_{j=1}^3 d\sigma_{ij} d\varepsilon_{ij} > 0

This is called *Drucker’s stability criterion* or *Hill’s stability criterion*.

The discretized form used in finite element analysis implies that the constitutive matrix relating stress increments to strain increments must be positive definite in order for the material to be stable. This is a condition that is generally computationally expensive to check for nonlinear materials. For a linear elastic material, the requirement can be directly converted into the well-known requirements and .

How can we mediate that we sometimes need to work with material models that do not fulfill the stability criterion? The important fact is that the material can be locally unstable, while the structure as such is still stable.

To understand this behavior, we can think of the material in the structure as connected springs. Some springs are purely elastic and represent the undamaged material, while a certain spring fails. Consider the three springs in the figure below.

*A three-spring system. The extension of the failing spring is denoted u _{1}.*

The spring k_{1} represents the material with the damage model, whereas the other two springs are purely elastic. The material model for the first spring is bilinear.

*Material model for the nonlinear spring. The peak force F _{m} is reached at the displacement u_{m}.*

The force in the lower branch is independent of damage:

F_l = k_3 u

Before the peak load is reached, the force in the upper branch is

F_u = \frac{k_1 k_2}{k_1 + k_2} u

since the two springs are connected in series.

The damage starts when the force in the upper branch is ; that is, when the external displacement is

u = \frac{(k_1+k_2) F_m}{k_1k_2}

and the corresponding external force is

F = F_m \left (1 +\frac{k_3(k_1+k_2)}{k_1 k_2} \right)

During the degradation, the force in the damaged spring can be written as . The same force also passes through spring 2 so that .

These two relations determine *u*_{1} as a function of the external displacement:

u_1 = \frac{k_2u-F_m-k_fu_m}{k_2-k_f}

In order to give a reasonable solution, *u _{1}* must increase when the external displacement is increased. Thus, it is necessary that . This is actually a clue to a very general result. A quick decrease in the force (or stress) is more susceptible to instability than a slower decrease.

Finally, we can derive the relation between the total external force and displacement during the degradation phase:

F = F_l + F_u = k_3 u-k_2\left( \frac{k_fu-F_m -k_fu_m}{k_2-k_f} \right) =\left ( k_3-\frac{k_2k_f}{k_2-k_f} \right ) u +\left( \frac{F_m+k_fu_m}{k_2-k_f} \right)

Thus, the external force can either increase or decrease when the external displacement increases, depending on the relative stiffness in the two branches. This simple model can thereby predict two types of instability:

- The upper branch can become unstable if
- Even if , the total system will be unstable if

In either case, a slower decrease of the force in the damage model is beneficial. In other words, the stiffer the surroundings, the more plausible it is that the whole system will be stable.

*A globally stable system (left) and a system where the stiffness in the lower branch is too small to maintain stability (right).*

In reality, we are not free to make arbitrary choices about force and stiffness. The area under the triangular force-displacement curve in the material model represents the energy dissipated by the process. The energy dissipation and the displacement (or strain) at final failure have a physical meaning.

The damaged part of a structure elongates while its force decreases. If the external displacement remains fixed, then the elastic parts of the structure must contract to compensate. This means that elastic energy is released. The only way the energy can be absorbed is by doing work on the damaged part. If, for a certain incremental displacement , the energy released by the elastic parts is larger than the work needed to produce the same displacement in the cracking part, the state is unstable.

Years ago, a friend of mine at the Department of Solid Mechanics at KTH Royal Institute of Technology in Stockholm performed some interesting experiments where he studied the stability of cracks in a ductile steel using extremely long three-point bend test specimens. The tests highlighted that crack stability is not only a function of the local stress state, but also of the capacity that the stored energy in the test specimen has to drive crack propagation. The longest test specimen in the experiments was 26 meters and occupied a large portion of the lab! The experiment was reported in the article “The stability of very long bend specimens” in the *International Journal of Pressure Vessels and Piping*.

With softening material models, it is extremely difficult to achieve convergence in a finite element model if the stress state is homogeneous.

In a physical material, the strength does not have a perfectly uniform distribution. When increasing the load, a crack will form at the location with the lowest strength, even if the stress state is homogeneous. When this happens, the surrounding material is unloaded.

Consider this example of three elastic blocks joined by two glue layers:

In real life, one glue layer will fail before the other. The slightly stronger layer will then be unloaded as the force through the part decreases. We cannot predict which layer will fail, since that is controlled by manufacturing inaccuracies. In the mathematical model, however, both layers fail simultaneously. Numerically, the iterations may not converge because the failure jumps back and forth between the two layers.

In a finite element model, the stresses are evaluated at each integration point within each element. When the load is increased above the maximum value, the failure may even jump between the elements or individual integration points within the same element (if the stress is the same everywhere).

This behavior implies that if we implement our own material model containing strain softening, we should test it using a single first-order element and under prescribed displacements. In this way, we ensure a homogeneous prescribed strain field and the stress is the same everywhere in the element. One example is Mazar’s damage model, which we described in a previous blog post. If we were to change the element shape functions to quadratic in that model, the analysis would no longer converge.

Does this mean that damage models are meaningless? Not at all. However, we must be careful to avoid indeterminate states. If a structure and its boundary conditions are symmetric, that symmetry must be employed in order to avoid indeterminacy. We can often solve problems with axial symmetry by using an axially symmetric model, while this may be impossible using a model of a 3D solid sector. Another approach is to allow a slight random spatial disturbance of the material data. This approach actually mimics nature, where strength values are randomly distributed. Also, it is important to increase the loading slowly in order to avoid large portions of the structure switching to a failed state at the same time.

In some material models, for example, within soil plasticity, strongly mesh-dependent thin layers with high shear strains can occur. These layers are called *shear bands*. When yielding is first initiated, the surrounding elements or even integration points are unloaded. The first elements to yield continue to accumulate plastic strains. It is interesting that this type of instability can actually be seen in real soil and is not only an artifact in the numerical model. Just as in nature, we cannot predict the exact location and distribution of the shear bands in the model.

As mentioned in the initial example, using prescribed displacements rather than prescribed forces is a good way to stabilize the numerical problem. However, this approach is essentially limited to the following cases:

- A single point load can be replaced with a prescribed displacement.
- The strain state is homogeneous, as when performing single-element tests of a material model, so that the displacement is the same over an entire boundary.
- The instability can be controlled by the external boundary conditions. In the spring device discussed above, a global instability caused by too small of a value of
*k*_{3}could be cured by using a prescribed displacement, but not an instability within the upper branch.

There is a more general method, which we can use to continue solving past a point of instability. In this method, we first prescribe an arbitrary quantity that is known to monotonically increase and then add an extra equation that solves for the corresponding value of the prescribed load or displacement.

To display this technique, let’s augment the initial example with a spring, so that the load is applied by prescribing the deformation of the end of the spring. If the spring is very stiff, this is essentially the same as prescribing the displacement directly.

*Bar system loaded through a spring.*

If the spring is softer, the system may become unstable, since too much energy can be released by the spring. The critical value is

k>\frac{EA \kappa^3}{h}

This is the most “negative stiffness” of the bar assembly, which occurs when the bars are horizontal. The relation between force and displacement at point 1 when varying the spring stiffness is shown below. The spring stiffness is given as

k = \beta \frac{EA \kappa^3}{h}

where the coefficient *β* is varied from an essentially stiff spring to values below the critical value.

*Force as a function of the displacement at point 1 when varying the spring stiffness.*

For values of *β* smaller than one, the solution fails when the spring stiffness equals the “negative” stiffness of the bar assembly.

If a prescribed force is used instead, all solutions will fail at the first peak load. By using prescribed displacement, it is possible to continue the analysis further. For lower spring stiffness values, we are still limited by the state when the internal instability causes failure.

The solution that we want to track has a monotonous vertical displacement at point 2, but prescribing it directly is not possible, since this would change the problem fundamentally. Instead, we add an equation stating: “Set the spring end displacement at point 1 so that the monitored displacement at point 2 has the prescribed value.” To do this, we add a *Global Equation* node in which a new unknown variable `disp_at_P1`

is added.

*The Global Variable definition.*

The equation determining the value of `disp_at_P1`

states that `disp_at_P2-delta = 0`

. The variable delta is the monotonous parameter incremented in the Stationary study step and ` disp_at_P2`

is a variable that contains the current value of the displacement at point 2.

*Settings for the study step, where delta is used as the auxiliary sweep parameter.*

The displacement at point 2 is then prescribed to have the value that satisfies the global equation.

*Settings for the prescribed displacement at point 1.*

With this modification, it is possible to trace the solution through the instability. As seen in the following graph, even strong instabilities can be bypassed using this method.

*Force as a function of the displacement at point 1 when varying the spring stiffness after stabilization with a* Global Equation *node.*

- Browse these Application Gallery examples to learn more about modeling negative stiffness and instabilities in structures:
- S. Kaiser, “The stability of very long bend specimens”,
*Int. J. Pres. Ves, & Piping.*17 (1984) 1–17.

Imagine a cricket ball sailing through the air at around 145 km/h (90 mph). A batsman stands ready, bat in hand. In the brief moment before the ball arrives, the player is most likely thinking of how to best hit a shot. There are many ways for the cricket ball to connect with the bat, but if a batsman knows the location of a sweet spot, he or she may be able to deliver a better shot by taking advantage of an optimal zone that enables maximum stroke power with the least amount of effort.

*A batsman during a cricket game aiming his shot to hit the sweet spot of the bat. Image by Pulkit Sinha — Own work. Licensed under CC BY-SA 2.0, via Flickr Creative Commons.*

Current research on the physics and science behind the game of cricket centers on the performance of the batsmen and bowlers. In fact, we’ve even covered this topic before in a blog post highlighting swing bowling techniques. However, one area of cricket that seems to lack in research is the cricket bat itself. For instance, a structural mechanics analysis can help to find sweet spots in a bat’s design that can improve the quality of the batter’s shots.

*Richie Latchman (left) and Yogeshwar Mulchand (right) in front of their poster “Determination of the “Sweet Spot” of a Cricket Bat using COMSOL Multiphysics®“.*

Researchers from the University of the West Indies, St. Augustine took a swing at this challenge by using COMSOL Multiphysics to investigate the sweet spots in a cricket bat. This research is useful not only for players and coaches, but also for sporting equipment companies, where simulation is used to analyze sporting goods.

To start, let’s delve into the physics behind cricket bats. The bending modes of a bat are the main vibrational modes affecting its performance. While a freely supported bat has several bending modes of vibration, a handheld bat can be seen as a clamped cantilever beam.

A bat’s first two bending modes are important to its performance, and between them is a “sweet zone” distinguished by its minimal vibrations and energy loss. This information comes from research by D. A. Russell (Ref. 6 and Ref. 11 in the research paper).

In a typical cricket bat, the handle is most sensitive to strain when a ball is played. According to research by Jones (Ref. 14 in the research paper), the thicker edge has increased durability. Further, the area with more wood behind the blade, the swell position, yields better rebounding qualities and transfers greater force to a struck ball. It follows that the sweet spot could be located above this wider area of the bat.

*Schematic of a cricket bat. Image by Y. Mulchand, A. Pooransingh, and R. Latchman and taken from their COMSOL Conference 2016 Boston paper.*

For their studies, the research team defined a sweet spot as the bat position in which the maximum energy is conveyed with the least amount of vibration. Note that there are other ways the term “sweet spot” can be defined for sporting equipment.

At the core of the team’s research is a 3D model of a common willow cricket bat. They selected the Kingwood material in COMSOL Multiphysics to account for the willow wood that is used to make cricket bats. The team added further parameters to the material based on their research into willow wood. The bat was also modeled as a free object in all areas except for the handle, which was fixed in space.

*The front (top image) and back (bottom image) of a 3D cricket bat model constructed in COMSOL Multiphysics. Images by Y. Mulchand, A. Pooransingh, and R. Latchman and taken from their COMSOL Conference 2016 Boston paper.*

The researchers used the Structural Mechanics Module to analyze the deformations as well as stresses and strains in the solid structures. They also performed an eigenfrequency analysis to discover the natural frequencies of vibration and the related mode shapes of the bat.

Through this work, the team found the cricket bat’s first six mode shapes, eigenmodes, and eigenfrequencies, as shown in the images below. In their results, the color bar indicates displacement from the bat’s natural position. Here, red shows a large movement and blue represents a lack of vibration when the bat is in its rest position at the specified frequency.

*The first six mode shapes of a cricket bat. Top row: The cricket bat at mode shape 1 (left), mode shape 2 (middle), and mode shape 3 (right). Bottom row: The cricket bat at mode shape 4 (left), mode shape 5 (middle), and mode shape 6 (right). Images by Y. Mulchand, A. Pooransingh, and R. Latchman and taken from their COMSOL Conference 2016 Boston paper.*

Let’s take a closer look at these results, focusing on modes 1, 3, and 6, which are of interest for the game. The research shows that bat deformation causes a vertical motion around the handle, with high displacement and vibrations at the bat’s toe in mode shapes 1, 3 and 6. In mode shapes 3 and 6, we see that the bat acts like a pivot with no displacement or vibrations in the lower-mid region. The bottom-right figure, which analyzes mode shape 6, is the only case where the bat acts like a pivot with no displacement or vibrations in the upper-mid region.

Mode Shape | Eigenfrequency |
---|---|

1 | 1.1 Hz |

2 | 1.5 Hz |

3 | 9.6 Hz |

4 | 10.3 Hz |

5 | 17.2 Hz |

6 | 27.9 Hz |

*The eigenfrequencies of the cricket bat at the different mode shapes.*

When observing the simulation results, note that the researchers assumed that the cricket bat model has the exact same dimensions and material properties as an actual cricket bat. They also didn’t consider the bat’s age. While the sweet spot locations are determined solely by the geometry used, changes in the material data will affect the model’s natural frequencies.

Based on the results of the research team, there is a sweet spot located in the middle of the bat that is concentrated at the lower-mid area, 10 to 15 cm from the bat’s toe. There is another sweet zone 20 cm from the handle’s base, where the handle connects to the shoulder.

As for if these results can help you improve your cricket stroke, you’ll find out when you take a shot.

- Read the full paper “Determination of the “Sweet Spot” of a Cricket Bat using COMSOL Multiphysics®” and check out the conference poster
- On the COMSOL Blog:
- Simulating the Art of Swing Bowling in Cricket
- The Physics of Tennis Racket Sweet Spots
- Browse our Physics of Sports blog posts for more information on using simulation for sports applications

Solid objects change their size, shape, and orientation in response to external loads. In classical linear elasticity, this deformation is ignored in the problem formulation. As such, the equilibrium equations are formulated on the undeformed configuration. In many engineering problems, the deformations are so small that the deformed configurations are not appreciably different from the undeformed configuration. Ignoring the changing geometry therefore makes practical sense as this yields a linear problem that is easier to solve.

On the other hand, for problems like metal forming, where the deformation is large, the equilibrium equations have to include the effect of changing geometry. Updating the equilibrium equations to include the effect of changing geometry introduces a nonlinearity known as geometric nonlinearity.

*Model geometry for a sheet metal forming process, where deformations can be rather large.*

When geometric nonlinearity is included in structural analysis, the COMSOL Multiphysics® software automatically makes a distinction between *Material* and *Spatial* frames. The material frame corresponds to the undeformed configuration, while the spatial frame corresponds to the deformed configuration. The software allows us to make a new geometry out of the deformed configuration; what we refer to as *remeshing a deformed configuration*. We can use this geometry as part of a new geometry sequence. Drill a hole in it, subtract it out of a bounding object, or simply add other geometric objects. Finally, solve a new physics problem on the composite domain. The new physics can be applied to the same COMSOL Multiphysics model in a different *component*, or in a different *model*. This is the first point that we will address.

If geometric nonlinearity is not included in structural analysis, the software does not distinguish between the material and spatial frames. Does that mean that if you do not want to include the effects of geometric nonlinearity in the equilibrium equations, you can not remesh a deformed configuration? The answer is no. You can split the two frames and force linear strains in the equilibrium equations. This is the second item that we will address.

For three-dimensional problems, there is an additional option. Surface plots can be exported as STL files. These files can be imported and used for solid modeling. In this process, we do not need to split the material and spatial frames. This is the third and last item we will discuss in today’s blog post.

Please note that

remeshing a deformed configurationmeans simply obtaining the deformed shape computed in structural analysis. When we use this deformed geometry for a later analysis, we are not considering residual stresses. If the second analysis is another structural analysis, keep in mind that the remeshed configuration is being used as a stress-free configuration for subsequent studies.

To consider effects of finite deformation in structural analysis, we have to select the *Include geometric nonlinearity* check box in the settings window of the study step. In some cases, COMSOL Multiphysics automatically enables geometric nonlinearity, such as when you include hyperelastic or other nonlinearly elastic materials, large-strain plastic/viscoelastic materials, or add any contact boundary conditions.

After we complete our structural analysis, we use the *Remesh Deformed Configuration* command to get the deformed shape. This is done in the meshing section of the Model Builder. Finally, the deformed mesh can be exported and imported back as a geometry object.

We demonstrate the above steps in the following sections.

Let’s consider the problem of squeezing a circular pipe between two flat stiff indenters. Because of the large deformation involved, geometric nonlinearity is included in the structural analysis, as shown in the screenshot below. Because of symmetries, we consider only a quarter of the geometry.

*The original geometry (outline) and the deformed geometry.*

The next step is to remesh the deformed configuration. This can be done by right-clicking on the data set (*Study 1/Solution 1* in this example) and choosing *Remesh Deformed Configuration*. Alternatively, we can use *Results > Remesh Deformed Configuration* from the menu while the data set is highlighted.

In either case, this adds a new mesh to the mesh sequence and opens the *Deformed Configuration* settings window. Next, we click on *Update*. Note that for parametric or time-dependent problems, we have to pick a parameter value or time step.

*Each parameter of a parametrized data set has its own deformed configuration.*

Finally, we go to the new mesh under *Meshes > Deformed Configuration* and build it.

*Remeshing a deformed configuration creates a new meshing sequence.*

One possibility is to reuse the deformed configuration in the same model file. To do so, we add another component and import the deformed mesh in the *Geometry* node of the new component, as highlighted in the screenshot below.

*A deformed mesh from one component can be imported in the geometry sequence of another component.*

We can now add more items to the geometry sequence. Let’s cut out from the bent pipe. We probably do not need the rigid indenter once we have used it to squeeze the pipe and will therefore get rid of it. The result is shown in the screenshot below. A new physics can be added to the second component.

*Deformed objects resulting from structural analysis can be used as part of a new geometry sequence.*

To use the deformed configuration in a different model file, export it to a separate file first.

If the *Include geometric nonlinearity* check box is unchecked, the spatial frame stays the same as the material frame. Therefore, we can not remesh the deformed configuration. If we do select the check box, COMSOL Multiphysics will include nonlinear terms in the strain tensor. What if we have a problem with infinitesimal strains and do not want to include expensive and unnecessary nonlinear strains in the equilibrium equations? The solution is to select the *Include geometric nonlinearity* check box in the study step, while ignoring the nonlinear strain terms by selecting the *Force linear strains* check box in the material model.

*Splitting material and spatial frames while keeping only linear strains in the equilibrium equation.*

The procedure for remeshing the deformed configuration remains the same as in the previous section.

The above method, including geometric nonlinearity and remeshing the deformed configuration, can be applied to both 2D and 3D problems. In 3D cases, we have an additional option via STL files. Any 3D surface plot can be exported as an STL file. This file can then be imported in the geometry sequence of another component or model file. By adding a *Deformation* node to a surface plot before exporting, we can get the deformed geometry. Do not include geometric nonlinearity, unless your problem is a large deformation problem.

*Add a deformation to a 3D surface plot and export the surface plot in the STL format.*

We can edit the *X*-, *Y*-, and *Z*-components of the displacements in the *Deformation* settings window of the above screenshot to introduce anisotropic or nonuniform scaling of the displacements. In fact, these quantities do not need to be structural displacements. By typing any valid mathematical expression for deformation components, we can subject the original geometry to arbitrary transformations.

To use the deformed geometry in a new file or component, the STL file generated in the above step can be imported in a geometry sequence, as shown below.

*Importing an STL file to a geometry sequence.*

COMSOL Multiphysics allows seamless coupling of different physics effects. If you want to couple structural analysis with another physics on the same domain, you will find built-in tools within our software that enable you to do so. The *Moving Mesh* and *Deformed Geometry* interfaces are often used together with physics interfaces to solve problems on evolving domains.

However, if you want to use the deformed configuration from a structural analysis as part of a new geometry sequence, where you add new objects to the deformed shape or include it in Boolean operations, you can apply the strategies demonstrated above.

As always, if you have any questions, please feel free to contact us.

]]>

Whenever you apply compressive forces that press physically separate solids together, mechanical contact at the boundaries deforms the solids such that the touching boundaries conform to each other. If you instead apply tensile forces that pull the domains apart, then there is no contact. This effect can be modeled using traditional contact modeling in COMSOL Multiphysics. If the objects instead stick together, it means that they support a tensile or adhesive force.

It turns out that when modeling forces related to contact and adhesion, special care needs to be taken with respect to what happens to forces acting in the tangential direction. While objects are in contact, there are three possible “tangential states”: frictionless sliding, sliding with friction forces, or sticking due to friction. As an additional complication, there are several processes in which two boundaries will begin sticking together only when some physical condition is fulfilled. It could, for example, be an adhesive material that cures only above a certain temperature and thus only then becomes actively adhesive. All of these phenomena can be represented with the new adhesion and decohesion functionality in version 5.2a of the Structural Mechanics Module.

Let’s consider two solid parts that are joined together by a layer of glue (this can be actual glue or something that conceptually behaves like glue). In COMSOL Multiphysics, the key to joining these two boundaries is the new *Adhesion* subnode, available as a child node to the *Contact* node in the model tree in the Model Builder.

To use the *Adhesion* subnode, you must select the option *penalty formulation* for the contact modeling. This formulation can be viewed as using a stiff, unidirectional spring to model the contact. When the two boundaries press on each other, a virtual thin elastic layer exists between the boundaries. When the “sticking” mode is initiated, the spring is made bidirectional, and it is also given a tangential stiffness. If there is an actual adhesive layer between the two boundaries, you can utilize a stiffness based on real material data. Otherwise, you can use a high stiffness, so that the two boundaries are virtually welded together.

When it comes to describing the onset of adhesion between the two layers, you can choose between four different criteria:

- When a certain contact pressure is exceeded
- When the two boundaries come within a certain distance of one another
- From the very beginning of the analysis
- When a user-defined Boolean expression is fulfilled

*Stress and deformation for a sticking cylinder.*

To begin, let’s take a look at the above animation. Here, a cylinder is pressed down into a flexible support and its motion is then reversed. The contact is modeled with an adhesion triggered by the contact pressure. When the cylinder moves back up again, it is actually pulling the foundation upward. The bending stress below the cylinder is more or less constant on the way up, since the foundation has to assume the constant curvature of the cylinder. Additionally, you can see the stress concentrations at the transition from the sticking to the nonsticking parts of the boundaries. This effect could, in reality, cause partial decohesion of the adhesive layer — a fact that we will return to at a later point.

The option to enter a user-defined adhesion criterion provides you with a great deal of flexibility in your contact modeling. You can, for instance, model a glue that requires a certain temperature or certain time to cure. Let’s move on to another example that illustrates this.

In the following case, a slider is pulled with constant speed along a larger foundation, while the whole assembly is heated up from the initial room temperature. The criterion for initiation of adhesion is selected so that the temperature at the contact boundary should exceed 365 K. The geometry and boundary conditions are highlighted in the following set of figures, along with the user-defined adhesion criterion.

*Left: The mechanical boundary conditions (rollers on three boundaries, prescribed horizontal displacement on one side of the slider, and contact between the slider and the foundation). Right: The thermal boundary conditions (convective heat flux on the top of the slider and bottom of the foundation). Thermal contact is modeled between the two parts.*

*Entering a user-defined adhesion criterion.*

When a time-dependent analysis is performed, the slider moves almost without resistance and as long as the temperature at the contact boundary is below 365 K. Once that temperature has been reached, an elastic bond is created so that a large force is required to further move the slider.

*Time-dependent analysis in which the domains are colored by temperature. The green contour is the adhesion temperature at 365 K. The arrow shows the force that is required to move the slider.*

*Development of shear force, plotted together with the interface temperature.*

As an additional note, this simulation includes a *Pair Thermal Contact* node in the model tree, through which the thermal resistance between the two parts is a function of the contact pressure. The contact pressure increases over time due to the inhibited thermal expansion in the vertical direction. As such, the heat transfer between the two parts is relatively small at the start of the simulation.

Up to this point, we have discussed how two boundaries are made to stick together. You can, however, also model the opposite situation, where two boundaries are torn apart as soon as the force is large enough. Such behavior is controlled via the *Decohesion* section of the *Adhesion* subnode.

*Settings for decohesion.*

You can use the new decohesion functionality for simulating either delamination between two layers, or for describing crack growth in a continuous material. In the latter case, the crack path must be known prior to conducting the analysis. The formulation, called a *cohesive zone model* (CZM), is based on a material model where the following applies:

- The stress in the adhesive layer is a function of the separation distance between the boundaries.
- The behavior of the layer is linearly elastic up to a certain separation distance between the boundaries.
- When the peak elastic deformation has been reached, the stress decreases with further deformation.
- Once a certain energy has been consumed, the bond between the two layers is completely broken.
- If unloaded before the bond is fully broken, the layer is considered to be damaged, thus featuring a reduced elastic stiffness.

In the graph below, the normal stress versus the boundary separation for a pure tension case is shown. The input data required is the maximum stress and the area under the blue curve, which can be interpreted as the energy release rate . The sloping red line is the elastic path, which would be followed during unloading from a partially damaged state.

*Stress versus boundary separation for the linear separation law.*

A similar curve relates the shear stress to the shear deformation. So, for the pure tension and pure shear cases, the decohesion behavior is uniquely defined. For more general cases, a mixed-mode separation law is used. This law essentially provides a weighting of the two basic cases, similar to how an effective stress is used for multiaxial stress states in plasticity.

When it comes to the different constitutive laws, you can choose from one of three options. In addition to the linear separation law outlined above, a polynomial law and multiaxial separation law are also available.

*The polynomial and multilinear separation laws, respectively.*

To show how you can model decohesion, we’ll use our Mixed-Mode Debonding of a Laminated Composite tutorial model from the Application Library of the Structural Mechanics Module. This example simulates an experimental setup known as a *mixed-mode bending (MMB) test*. The purpose of the test is to study the delamination of a laminated composite beam. The geometry is such that a well-defined state of mixed tension and shear can be created.

*The geometry of the test specimen for the MMB test.*

During the test, the initial crack will start growing when the load exceeds a critical value. As the crack begins to grow, the structure will become more flexible so that the force is reduced. This is illustrated in the graph below.

*A graph comparing force and displacement at the outer edge of the beam.*

The physical experiment, as well as the simulation, must be performed under controlled displacement conditions. Otherwise, unstable crack growth will occur once the peak load is reached.

*Effective stress in the upper layer and forces applied at the outer edge of the beam. The delamination, accompanied by a reduction in load, is clearly visible. The deformations have a true scale.*

For this example, we have utilized the option to implement the effects of adhesion from the start of the simulation. Note that the actual bonding process is not part of the simulation. There is, however, a way to combine these two effects.

In our first example, very high stresses were visible at the end of the adhesive layer. But what if we chose to add a decohesion rule as well? The final result of such a simulation is depicted below. The extent of the sticking layer is reduced due to some debonding that has occurred. At the turning point, and during part of retracting motion, the results of the two simulations are equivalent. Later on, however, the stresses in the adhesive layer exceed the decohesion limit, causing the contact to be lost.

*Final state of the simulation after only applying adhesion (top) and when adhesion and decohesion are combined (bottom).*

Consider a case where adhesion is active, but you have set the shear stiffness of the adhesive layer to zero. This means that the two boundaries are connected to each other in the normal direction, but will be free to slide in the tangential direction. There are some cases where you could make use of this behavior — modeling bearings is one example.

Two semicylinders, shown in the following animation, are joined in such a way. The larger cylinder has roller conditions that restrict vertical motion and rotation, with an elastic spring that resists horizontal displacement. The smaller cylinder, meanwhile, has a prescribed translation and rotation. At the start of the simulation, the force between the two objects is predominantly tensile. Toward the end of the simulation, the smaller object pushes on the larger object. Throughout the simulation, the tangential force between the two connected boundaries is zero.

*Semicylinders that are connected only in the normal direction.*

The new functionality for modeling adhesion and decohesion in COMSOL Multiphysics version 5.2a provides you with several new possibilities for performing high-fidelity structural mechanics simulations. These tools are particularly powerful in the analysis of manufacturing processes in which parts are being joined. Decohesion modeling is also important when studying the maximum load-bearing capacity of structures. By delivering accurate and fast results, this new contact modeling functionality can help foster the development of more efficient and reliable manufacturing processes across a range of industries.

- Head over to the Release Highlights page to learn about all of the features and functionality available in COMSOL Multiphysics version 5.2a
- Watch this video to learn how to create contact pairs when modeling structural contact
- Browse additional applications of structural mechanics modeling here on the COMSOL Blog

The food that we consume on a day-to-day basis, particularly carbohydrates, is a powerful source of energy for the human body. For the body to utilize energy from carbohydrates and store glucose for later use, it is crucial that its cells properly absorb the sugar. The key to this process is *insulin*, a hormone the body signals to the pancreas cells to release into the bloodstream, allowing sugars to enter the cells and be used for energy.

But what happens when the body fails to produce enough insulin or if it doesn’t work in the way that it should? In this case, the glucose fails to be absorbed by the cells and will instead remain in the bloodstream, resulting in rather high blood glucose levels. Referred to as *diabetes*, this metabolic disease relates to cases where the body produces little or no insulin (Type 1) or does not properly process blood sugar or glucose (Type 2). Note that in the latter type, a lack of insulin can develop as the disease progresses.

*A device for injecting insulin. Image by Sarah G. Licensed under CC BY 2.0, via Flickr Creative Commons.*

In both Type 1 and Type 2 diabetes, insulin injections serve as a viable treatment option. These injections, however, can cause pain when applied by a heavy single-needle mechanical pump. To minimize patients’ discomfort, researchers have investigated the potential of using a microneedle-based MEMS drug delivery device to administer insulin dosages. Not only would the stackable structure be minimal in size and easy to apply to the skin, but it would also provide a safer and less painful approach to applying injections.

Here’s a look at how a research team from the University of Ontario Institute of Technology used simulation to evaluate such a device…

Let’s begin with the design of the micropump model. The researchers developed a MEMS-based insulin micropump, placing a piezoelectric actuator on top of a diaphragm membrane comprised of silicone, with a viscous Newtonian fluid flowing through it. Note that the design itself is based on the minimum dosage requirement for diabetes patients — this typically ranges from 0.01 to 0.015 units per kg per hour.

Vibrations from the actuator create a positive/negative volume in the main chamber of the pump, which then pulls the fluid from the inlet gate and pushes it toward the outlet gate. Two flapper check valves control the direction of the fluid from the inlet to the outlet leading to the microneedle array, with a distributor connecting the outlet gate to the microneedle substrate. The established discharge pressure then pushes the fluid out of the microneedles to the skin’s outer layer.

The following set of images show the dimensions and cross section of the micropump as well as a more detailed layout of the model setup, respectively.

*The MEMS-based piezoelectric micropump design. Image by F. Meshkinfam and G. Rizvi and taken from their COMSOL Conference 2015 Boston paper.*

*A 2D layout of the micropump model setup. Image by F. Meshkinfam and G. Rizvi and taken from their COMSOL Conference 2015 Boston paper.*

To accurately study the performance of the micropump, the researchers utilized three different physics interfaces in COMSOL Multiphysics: the *Solid Mechanics*, *Piezoelectric Devices*, and *Fluid-Structure Interaction (FSI)* interfaces. The fluid flow that occurs from the inlet to the outlet via the action of the flapper check valve is described by the Navier-Stokes equations. Upon a wave signal exciting the piezoelectric actuator, the diaphragm disk and piezoelectric actuator move together, with an FSI moving mesh presenting the deformed solid boundary to the fluid domain as a moving wall boundary condition. Within the solid wall of the pump, this moving mesh follows the structural deformation. The FSI interface also accounts for the fluid force acting on the solid boundary, making the coupling between the fluid and solid domains fully bidirectional.

For their simulation analyses, the research team applied different input voltages and input exciting frequencies to the micropump design, studying various elements of the device’s behavior. The range of the voltages spanned from 10 to 110 V, while the exciting frequencies ranged from 1 to 3 Hz.

Let’s look at the results for an input voltage of 110 V and an input exciting frequency of 1 Hz. The plot on the left depicts the inflow and outflow rates, showing very little leakage for both. The plot on the right shows the established discharge and suction pressures at the inlet and outlet. At the inlet gate, a negative pressure denotes suction pressure, while a negative pressure at the outlet gate represents discharge pressure.

*Left: Inflow and outflow rates. Right: Discharge and suction pressures. Images by F. Meshkinfam and G. Rizvi and taken from their COMSOL Conference 2015 Boston paper.*

As part of their analyses, the researchers measured the stress and deflection of the flapper check valves as well as the velocity field of the fluid. You can see their results in the following set of plots.

*Left: Von Mises stress in the flapper check valves and velocity field of the fluid. Right: Deflection of the flapper check valves. Images by F. Meshkinfam and G. Rizvi and taken from their COMSOL Conference 2015 Boston paper.*

The studies shown here, as well as those conducted with alternative inputs, indicate that the micropump design performs properly from the minimum to maximum spectrum of pressure and flow rates. Such a configuration can therefore serve as a viable alternative for applying insulin injections, providing a safer and less painful method of treatment for diabetes patients. The researchers hope to use their simulation findings as a foundation for creating more durable and dynamic insulin micropump designs in the future.

- Learn more about the research presented at the COMSOL Conference 2015 Boston: “Design and Simulation of a MEMS Based Piezoelectric Insulin Micro-Pump“
- Explore further applications of simulation for improving methods of treatment on the COMSOL Blog:

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

The Pratt truss bridge has been a popular structural design among civil engineers for many years. This type of structure can be easily identified by the diagonal beams on each side that, aside from the ones at the very end, slant toward the center of the span of the bridge. Due to its design, the diagonal beams are only subject to tension, and can be made from a lighter and less expensive material. The shorter vertical beams, which are not as sensitive to buckling, undergo compression.

*A Pratt truss bridge. Image by Jeffrey Beall — Own work. Licensed by CC BY-SA 2.0, via Flickr Creative Commons.*

As with any class of civil engineering structures, exposure to various forces, from vehicles to wind, can greatly impact the safety and stability of Pratt truss bridges. Accounting for these factors requires an understanding of the different loads placed on the structure as well as the dimensions of the particular bridge. Computational apps deliver the capabilities for assessing both of these elements, all while spreading simulation power to a larger number of people through an easy-to-use interface. Let’s take a look at one example…

The Truss Bridge Designer is an app based on our tutorial model of a Pratt truss bridge. The embedded model, and the underlying theory, are hidden behind a simplified interface that is easy for users to navigate and utilize. As the designer of the app, it is up to you to decide how to organize the layout and design of your app, as well as select the parameters that you want to include.

*The user interface (UI) of the Truss Bridge Designer app.*

The demo app, shown above, includes two main sections: the *Inputs* section and the *Results* section. Within the *Inputs* section, users can modify the dimensions of the bridge, cross-section data of the supporting beams, and thickness and drag coefficient of the roadway. The *Wind load* subsection can be used to specify if a wind load is applied and set the wind direction and intensity. The *Truck load* subsection, meanwhile, gives users the option to specify the location and mass of the trucks applied in the stationary analysis. When adding the number of trucks, the following criteria must be met:

- A truck can be positioned in a way that just one axle is inside the bridge, but it can’t be completely outside of the bridge
- A truck can’t have wheels that are outside the bridge in the
*y*direction - Trucks must not overlap each other when several of them are added

If the truck positions don’t meet the above criteria, a warning message will appear and the *Compute Stationary* button will be disabled. Notifications such as this help provide guidance to users as they run their own simulation tests, ensuring consistency in the results.

Now that we’ve reviewed the *Inputs* section, let’s move on to the *Results* section. Here, you will find a series of tabs featuring multiple plots. The *Preprocessing Data* tab, for instance, includes four selectable plots. As the bridge dimensions are modified, the *Geometry* plot will automatically update. The *Truck Load*, *Wind Load*, and *Beam Orientation* plots can be updated manually by simply clicking the *Update Preprocessing* button to reflect changes in the input data.

The *Stationary Results* tab features four selectable plots as well: *Displacement*, *Force and Moment in Beams*, *Stress in Beams*, and *Stress in Roadway*. Users have the option to select the component of force or moment that they want to plot for the force and moment plots, as well as if they want to plot their results on all of the beams or just a group of them.

The final tab is *Eigenfrequency Results*. This section shows the normalized displacement of the mode shape that is specified in the selector located right above it.

What if the user wants to share their simulation results with others? With the *Generate Report* button, this step is simple. By clicking the button, they can generate a report that includes simulation results from the app and, carrying on with the theme of customization, further details that they wish to highlight.

Every design team experiences their own set of challenges. With the Application Builder, you can create a tool that is tailored to your specific design, while enabling additional members of your team or other departments within your organization to run their own tests. As we have demonstrated today with a Pratt truss bridge example, simulation apps can serve as a viable foundation for analyzing classes of civil engineering structures, customizing the analyses to fit specific structural designs and load conditions.

Feeling inspired? Use the resources below as a jumping-off point to start building apps of your own.

- Download the app presented here: Truss Bridge Designer
- Watch this video for a quick introduction on turning COMSOL Multiphysics models into apps
- Browse the COMSOL Blog for further inspiration and guidance in building simulation apps

To help extend simulation capabilities to a wider audience, numerical modeling apps are designed with simplicity and ease-of-use in mind. While the interface that users interact with appears this way, there are many other important layers to consider behind an app’s design. The underlying theory and the embedded model, for instance, are crucial elements, as they help to ensure accuracy in the simulation results obtained by users.

So how do we connect the dots between these different elements — the theory, the model, and the app? Today, we’ll demonstrate this relationship by looking at the theory and model behind our Linear Buckling Analysis of a Truss Tower app. While an app sometimes merely embeds a model and places a simplified user interface (UI) on it, this case involves using an app to generate an advanced extension of the built-in functionality available in COMSOL Multiphysics.

*Linear Buckling Analysis of a Truss Tower demo app.*

To begin, let’s focus on the problem that the app is designed to study: buckling. If a tall vertical structure is subject to an increasing compressive load, deformations will be very small until the critical value of the load is reached. If the load is slightly increased after this point, the structure can suddenly collapse. My colleague Henrik Sönnerlind discussed this phenomenon, known as *buckling*, in an earlier blog post. Here, we will focus on buckling as it specifically relates to a truss tower design.

Truss towers are slender structures that can face the risk of buckling. In this model, we will consider the effects of the weight of the truss structure itself, the tension effects of the optional guy wires, and a concentrated vertical force at the top. The latter is the “payload”, typically large antennas.

From the viewpoint of buckling, a load can be considered *live* or *dead*. A dead load, like the self-weight, has a fixed value. The live load, the weight of the antenna in this case, is the load against which we want to compute the safety factor.

COMSOL Multiphysics does not include a built-in setup for solving this problem that allows us to distinguish between the live load, gravity, and wire tension effects. But with some understanding of the theory behind buckling and how the software works, such a study can be set up. We will have to write some extra equations, *weak contribution*s as they are more often called, which are simple to incorporate into the model. This represents an important strength of COMSOL Multiphysics: Users can adjust and extend the capabilities of available features by modifying the existing implementation or writing new mathematical terms.

The tower that we will consider has a rectangular cross section with four vertical bars at the corners. Three types of members — longitudinal, transverse, and diagonal — form the tower structure. The guy wires, which are attached to the tower at two different levels, give the structure greater stiffness to protect it against, for instance, wind loads. Note that the wires are under pretension, otherwise they would not provide any stiffness. The bottom part of the truss is pinned to the ground. The screenshot below depicts the model tree structure for the buckling analysis.

*Model tree settings for the truss tower buckling analysis.*

The nodal labels in the above diagram are self-explanatory:

*Linear Elastic Material 1*specifies the material properties of the truss elements*Linear Elastic Material 2*and*Linear Elastic Material 3*relate to the material properties of the guy wires*External Stress*specifies pretension in the guy wires*Gravity*considers the weight of the truss members and guy wires*Point Load*allows us to apply the vertical load on the truss tower*Weak Contribution 1*and*Weak Contribution 2*enable us to add in extra mathematical terms

*Study 1* in the model tree is a predefined buckling analysis study that is included in the *Truss* interface and consists of two individual study steps. The first is a stationary study step in which you compute the state of stress in a structure for a given load. The second study step allows you to solve an eigenvalue problem to determine the critical load as a multiple of the load you applied. In a typical analysis of a structure, we are interested in identifying the nodal displacements due to a load acting on it. If we put all of the nodal displacements in a vector and if the structure stiffness matrix is , then this amounts to solving a system of equations of the form

\mathbf K \mathbf u_0=\mathbf f_0.

The stiffness matrix can be split into linear and nonlinear parts. Thus, , where is the linear part and is the extra contribution caused by considering geometric nonlinearity. Note that the nonlinear part of the stiffness matrix depends on the applied load. In a linear buckling analysis, we assume that the nonlinear part of the stiffness matrix is a linear function of the load (i.e., , where is a scalar multiplier). When the structure buckles, the deformation is unbounded. Numerically, this manifests itself in a singular stiffness matrix, so we must solve for the value of that renders the matrix singular.

\left( \mathbf K_L + \lambda \mathbf K_{NL}(\mathbf f_0) \right) \mathbf u = \mathbf 0

In other words, we solve the eigenvalue problem defined above. The smallest eigenvalue is the critical load factor, and the corresponding eigenvector defines the buckled shape.

Now, let’s try to understand the current problem with respect to the theory explained above. Remember our assumptions? We want to include the weight of the tower and cables, as well as the pretension in the wires, in the analysis. These loads, however, do have fixed values so that their contribution to the nonlinear stiffness matrix should not be scaled by . Therefore, we are interested in solving a modified eigenvalue problem:

\left( \mathbf K_L +\mathbf K_{NL,d}(\mathbf f_d) + \lambda \mathbf K_{NL,l}(\mathbf f_{l0}) \right) \mathbf u =0 \label{BucklingEq}

where captures the effect of the dead loads. The eigenvalue step in the buckling study, however, only allows you to solve the standard buckling problem where all loads are considered as live loads. To change this in order to accomplish our goals, we need to look at additional mechanisms that COMSOL Multiphysics offers.

The first step in solving our problem is to perform a stationary analysis to isolate the stiffness due to dead loads. Once this is done, we can manipulate the eigenvalue solver to include the effects of the dead loads in the problem. The plan is to solve three stationary problems, respectively, in succession:

- Solve for gravity effects and pretension
- Consider the effects of pretension in the guy wires only
- Analyze the combined effects of live weight and wire pretension

We must include the wire pretension in all static load cases. Without it, the wires have no stiffness, so the problem would be singular. As such, it is not possible to directly create a load case containing only the live weight.

To solve three different load conditions within one single stationary study step, we can group them as load groups and define appropriate load cases within the solver. In the example below, we have created three load groups: *Gravity Load, Point Load,* and *External Stress*. These groups correspond to gravity, point load, and stresses in the wires, respectively. To create these load groups, simply right-click on the *Global Definitions* node in the model tree and select *Load Group*. This generates a new load group for you, the name of which you can adjust as needed. Say you want to include the gravity node under the load group *Gravity Load*. In that case, simply right-click on the node and choose the *Gravity Load* option under *Load Group*.

*Defining load groups and grouping load types.*

The reason for adding these load groups will be clear when we look at the *Stationary* node of *Study 1*. In the *Study Extensions* section, we can define a number of load cases to create several different stationary analyses within the same study step. In the following screenshot, three load cases are defined:

*Dead Load 1*: Gravity (GR) and pretension in wires (ES)*Dead Load 2*: Pretension in wires (ES)*Live Load*: Point load acting on the tower (PL) and pretension in wires (ES)

In the case of *Dead Load 1*, as it may already be intuitively clear to you, the stationary solver will only solve for gravity and pretension effects, excluding the point load from the analysis. Similar considerations apply to other cases as well.

*Defining load cases in the stationary solver.*

So why we are interested in solving the stationary problem for the load cases that we just defined? We want to compute nonlinear stiffness due to dead loads, which is generated by the first stationary analysis. In this case, the effects of the weight of the truss, the weight of the guy wires, and the pretension in the wires are all included. The second stationary analysis isolates the pretension effects in the wire. Note that the weight of the wire is excluded in this step. These results are then used to eliminate the effects of guy wire pretension in the eigenvalue solver. In other words, we are solving the original problem as

\left (\mathbf K_L + \mathbf K_{NL}^{1}(W_1+W_2+ES) + \lambda \mathbf K_{NL}^{3}(f_0+ES) -\lambda \mathbf K_{NL}^{2}(ES) \right ) \mathbf u =0 \label{BucklingEq}

where denotes the nonlinear stiffness matrix coming from the solutions of the corresponding load case scenarios. With the assumption of linearity in the nonlinear stiffness matrix contributions, this is exactly the problem that we want to solve.

To get the extra stiffness contributions, we must manually enter two terms via the *Weak Contribution 1* and *Weak Contribution 2* nodes. It is important to note that these weak contributions should be active only during the eigenvalue solver stage of the problem, not during the stationary study. This can be controlled in the settings for the individual study steps.

The next step involves understanding what to write in the fields of these nodes. In the case of geometric nonlinearity, the basic truss equation is

\frac{d}{d\hat{x}}\left(YA \left( \frac{d \hat{u}}{d \hat{x}} + \frac{1}{2} \left(\frac{ d \hat{u}}{ d \hat{x}}\right)^2\right)\right) = f,

where is the Young’s modulus, is the cross-sectional area, and is the displacement. As the formatting of the dependent and independent variables emphasizes, the equations are written in local directions. The equation above is the so-called strong form equation of truss. The corresponding weak form is given by the expression

A \cdot S \cdot \delta E

where is the axial stress and is the axial strain. The symbol denotes variation and is represented by the `test()`

operator in COMSOL Multiphysics. This is the type of expression that COMSOL Multiphysics understands, and it uses it to generate the stiffness matrix. In fact, if you go to the *Equation View* of *Linear Elastic 1*, you will see the same expression written under *Weak Expressions*, as highlighted below.

*Axial strain and weak expression for the truss tower model.*

The expression for the strain, `truss.en`

, can actually have two different values,

`0.5*((truss.tlex*(2uTx+uTx^2+vTx^2+wTx^2)+truss.tley*(vTx+uTy+uTy*uTx+vTy*vTx+wTy*wTx)+`

truss.tlez*(wTx+uTz+uTz*uTx+vTz*vTx+wTz*wTx))*truss.tlex+

(truss.tlex*(vTx+uTy+uTy*uTx+vTy*vTx+wTy*wTx)+truss.tley*(2vTy+uTy^2+vTy^2+wTy^2)

+truss.tlez*(wTy+vTz+uTz*uTy+vTz*vTy+wTz*wTy))*truss.tley+

(truss.tlex*(wTx+uTz+uTz*uTx+vTz*vTx+wTz*wTx)+truss.tley*(wTy+vTz+uTz*uTy+vTz*vTy+wTz*wTy)+

truss.tlez*(2wTz+uTz^2+vTz^2+wTz^2))*truss.tlez)

or

`(uTx*truss.tlex+0.5*truss.tley*(vTx+uTy)+0.5*truss.tlez*(wTx+uTz))*truss.tlex+`

(0.5*truss.tlex*(vTx+uTy)+truss.tley*vTy+0.5*truss.tlez*(wTy+vTz))*truss.tley+

(0.5*truss.tlex*(wTx+uTz)+0.5*truss.tley*(wTy+vTz)+truss.tlez*wTz)*truss.tlez

The first expression is the one you would see in the case of a geometrically nonlinear study. The latter strain expression is much simpler, as it is for a geometrically linear case.

Now the plan of action is simple. The linear terms of stiffness are independent of the loads and they are automatically included in the analysis. To include the nonlinear stiffness matrix due to dead loads, we should extract the stresses from the first stationary analysis and multiply this by the test of *only* the nonlinear part of the strain function. The stress from the first stationary analysis can be obtained with the `withsol()`

operator in COMSOL Multiphysics. This gives us the following expression that goes in the *Weak Contribution 1* node.

`-withsol(sol2,truss.Sn,setval(loadcase,1))*test(0.5*`

((truss.tlex*(uTx^2+vTx^2+wTx^2)+truss.tley*(uTy*uTx+vTy*vTx+wTy*wTx)+truss.tlez*(uTz*uTx+vTz*vTx+wTz*wTx))*truss.tlex

+(truss.tlex*(uTy*uTx+vTy*vTx+wTy*wTx)+truss.tley*(uTy^2+vTy^2+wTy^2)+truss.tlez*(uTz*uTy+vTz*vTy+wTz*wTy))*truss.tley

+(truss.tlex*(uTz*uTx+vTz*vTx+wTz*wTx)+truss.tley*(uTz*uTy+vTz*vTy+wTz*wTy)+truss.tlez*(uTz^2+vTz^2+wTz^2))*truss.tlez))*truss.area

A similar expression is used to exclude the effects of guy wire stresses from the eigenvalue analysis. Note that the expression there is multiplied with a at the end. Further note that the stresses from the second stationary analysis are accessed via the `withsol()`

operator. The argument of the `setval()`

function is changed to ` 2`

. Now if you click the *Compute* button, you should get the correct critical load for the truss tower design.

Numerical modeling apps are comprised of various layers. Behind an app’s simplified user interface is an embedded model and underlying theory that helps to ensure both accuracy and efficiency in simulation results. Here, we have highlighted this in the case of an app developed to analyze linear buckling in a truss tower design. As the example shows, the combined flexibility of COMSOL Multiphysics and the Application Builder is powerful in addressing complex problems, fostering efficiency at every step of the design process.

- Already building apps of your own?
- Browse additional blog posts relating to simulation apps for further inspiration and guidance

- Looking to get started?
- Watch this video for a quick introduction on turning your COMSOL models into apps
- Attend a free workshop to get hands-on experience

To begin, let’s consider a famous case of a structure affected by vibrations. The London Millennium Footbridge, as it is officially known, is a steel suspension bridge that allows pedestrians to cross over the River Thames in London. Locally, however, this structure is often referred to as the “Wobbly Bridge’”.

*The London Millennium Footbridge. Image by Rup11 — Own work. Licensed under CC BY-SA 3.0, via Wikimedia Commons.*

Just days after opening in June 2000, the footbridge was closed, as pedestrians’ footsteps produced vibrations that caused the bridge to sway from side-to-side. The unconscious tendency of pedestrians to match their footsteps with the sway of the structure only worsened matters. The bridge itself was closed for almost two years, with design modifications implemented in order to counteract such vibrations. The solution: Install dampers within the structure’s design.

Dampers are an important element in the design of structures, as they help to prevent damage resulting from vibrations due to seismic waves or wind. By doing so, these devices serve as a powerful resource for protecting the longevity of various structures.

Consider, for example, a tall structure like a building. In such cases, dampers that consist of layers of viscoelastic material are often introduced into the design as a means of protection against vibrations. The viscoelastic material (shown in red in the image below) will absorb the vibrations from the mounting and dissipate the mechanical energy as heat. This means that the low-frequency vibrations resulting from seismic waves or wind will be less noticeable and less likely to cause structural damage.

*A schematic of a viscoelastic structural damper.*

With the goal of developing impactful infrastructures and buildings that meet safety requirements for withstanding low-frequency vibrations, viscoelastic structural dampers are a valuable resource to designers. Before these devices can be incorporated into a structure’s design, there is, of course, the need to verify their effectiveness. With the Application Builder, ensuring that these requirements are met has evolved into a much more streamlined process. Our Viscoelastic Structural Damper Analysis app offers insight.

Simulation apps are all about customization. When building an app of your own, you can tailor its design and layout to correlate with your specific analyses. The result is an easy-to-use tool that those with little simulation knowledge can use to set up and solve their own simulation studies.

The Viscoelastic Structural Damper Analysis app is designed for users who wish to model the transient and frequency response of a certain structural damper type given different viscoelastic materials and loads. To determine the effectiveness of the damper’s ability to dissipate energy, the app shows results for important parameters such as the hysteresis loop, loss and storage moduli, and displacement.

*User interface (UI) of the Viscoelastic Structural Damper Analysis app.*

The app’s UI, as shown above, is broken down into a series of sections that allow users to easily navigate through the tool and find the information that they need. The *Ribbon* section features six buttons. These different buttons give users the ability to easily toggle between frequency-domain and transient studies. They further enable them to reset input fields to their default settings, create an animation, access app-related documentation, and generate a report composed of model information and simulation results.

Within the *User Input* section, you will find a number of different parameters that can be modified. Users can, for instance, specify the viscoelastic material model that they would like to use in their damper simulation, with the option to compare results using two different material models as well. They can further define the magnitude of the forces in the holes along with their phase angles. In addition to a sketch that shows the damper’s geometry and respective materials, this section also includes additional input options that are tailored to the different types of studies. For the transient study, users can adjust the frequency of the load and the number of cycles to be analyzed. Similarly, for the frequency-domain study, they can select the range of the frequencies.

Located on the rightmost part of the app’s interface, the *Results* section is comprised of two tabs that show the results for the transient and frequency studies. The changes that occur within these tabs relate to whether the simulations involve a single model or the comparison of two material models.

While their layout is simplified, simulation apps still exploit all of the visualization features available within COMSOL Multiphysics, presenting results in a clear format that is easy to communicate with others.

Running simulation studies is no longer limited to those with simulation expertise. With apps, it is now possible to spread simulation capabilities to a wider audience. As the creator of an app, you have full control over the features and functionality that are included in its design, customizing it to fit your necessary requirements and thus optimize your overall design workflow.

To start experiencing the benefits of designing and deploying computational apps, use the resources below as a jumping-off point.

- Download the example presented today: Viscoelastic Structural Damper Analysis app
- Check out our Intro to Application Builder Videos series for a helpful introduction on how to turn your COMSOL models into apps
- Find further inspiration in the design and use of simulation apps here on the COMSOL Blog

Take a hike in a nearby forest and you’ll come across various examples of porous media: ground soil, rocks, and even your own biological tissue. A porous medium is made up of a solid material, called a *porous matrix*, which contains a network of connected pores saturated with fluids. Consider a basic kitchen sponge that is completely saturated with water, for instance. This is an example of a porous medium.

*Porous rock formations found on Mono Lake in California.*

When a porous matrix is made up of a solid elastic material, and the fluid inside is viscous, this aggregate is known as *poroelastic* material. The study of poroelasticity has applications in geomechanics for structures such as reservoirs, dams, and energy piles. The Leaning Tower of Pisa is one well-known historical example of the negative outcome of building onto clayey porous soils.

Studying poroelasticity helps us predict the damage that can occur in a solid. For instance, in a reservoir, fluid is pumped out and the reduced pressure creates fluid movement that causes in situ stresses. Such stresses trigger gradual deformation in the overburdens above the formation, causing some of the layers to cave in or sink. Gradual deformation can continue over time, leading to the eventual cracking of the design.

As we’ll highlight here, multiphysics simulation offers valuable insight into how porous materials behave in the real world, helping us address and prevent potential deformation in geotechnical structures.

The analysis of porous materials is a true multiphysics problem in that it requires the coupling of fluid flow and structural mechanics and commonly heat transfer as well. The physics behind poroelasticity can be investigated using the Biot theory, which is made up of two main physical laws:

- Linear elasticity equations describe the porous matrix
- Darcy’s law describes fluid flow through the matrix

The *Poroelasticity* coupling in the Subsurface Flow Module allows for the numerical coupling of Darcy’s law and solid mechanics. This enables you to evaluate how a porous medium is deformed due to fluid flow and changes in pore pressure. Let’s look at two instances of studying poroelasticity in COMSOL Multiphysics.

Reservoirs often need to be pumped in order to harvest the valuable fluid inside, such as oil or water. Pumping the fluid generates a decrease in pressure in the pores, which can cause the surrounding sediment to sink. This process leads to vertical compaction and lateral stretching in the reservoir.

In the Biot Poroelasticity tutorial model, we can analyze the behavior of the fluids and solids in the basin of a reservoir with three sediment layers over an impermeable layer of bedrock. In our model, the top two layers have the same thickness, while the bottom layer is deepest at the centerline and the bedrock layer is faulted, creating a “step”.

*The geometry of an oil reservoir.*

Using the *Poroelasticity* interface, we can set up a two-way coupled analysis of fluid flow and solid deformation in the basin. The simulation starts with fluid pumping from the centerline and flowing from left to right. The pumping process causes the fluid in the basin to pull away from the step. Through the results, we can observe changes and deformation in the layers over two, five, and ten years.

*Deformation in the reservoir basin after two (left), five (middle), and ten (right) years.*

The plots above show that pumping causes the basin’s layers to compensate for changes in pressure by shifting laterally, resulting in gradual deformation in the structure.

Heat transfer is another common physics area that needs to be considered when studying fluid flow and structural mechanics in porous materials. Energy piles, which are heat exchangers located within building foundations for effective heating and cooling, are one application that demonstrates this problem.

*The geometry of a basic energy pile. Image by E. Holzbecher and taken from his COMSOL Conference paper submission.*

Within an energy pile setup, groundwater can flow through the porous matrix of a building foundation and change the temperature distribution around the device. The fluid flow can also produce a change in the pore pressure and affect the stability of the subsurface material. A team of researchers used numerical coupling in COMSOL Multiphysics to investigate how thermal effects can exaggerate deformation in the energy pile structure and adjacent ground.

*The temperature distribution (left) and vertical displacement (right) for a model of one energy pile in a porous structure. Images by E. Holzbecher and taken from his COMSOL Conference paper submission.*

The results show that while thermal stress and expansion can have a great effect on the deformation of the energy piles and building structure, fluid compressibility and the thermal properties of the groundwater have negligible and very minor effects, respectively.

The ability to easily couple numerical studies in COMSOL Multiphysics enables us to thoroughly analyze porous structures and evaluate how a porous material will perform in the real world. This, in turn, fosters the development of safer structures and improved geotechnical designs.

- Try it yourself: Download the Biot Poroelasticity tutorial model
- Read the full paper from the COMSOL Conference 2014 Cambridge: “Energy Pile Simulation — an Application of THM-Modeling“
- Browse the COMSOL Blog for additional discussions on poroelasticity:

The magnetostrictive effect is fairly common; in fact, you may have *heard* this effect in action before. Familiar with the humming sound that comes from a transformer or other high-powered electrical devices? At the root of this magnetic hum is magnetostriction.

To better understand magnetostriction, we can begin by taking a closer look at magnetostrictive materials. When exposed to a magnetic field, the tiny ellipsoidal magnets inside magnetostrictive materials realign themselves, as shown in the animation below. This new order results in a macroscopic strain, causing the solid material to stretch or shrink. As such, magnetostriction can be used to convert magnetic energy into kinetic energy. The opposite effect is also possible, as applying stress to a magnetostrictive material can change the material’s magnetic state.

*An animation illustrating magnetostriction.*

Engineers at ETREMA Products, Inc. have experience working with magnetostrictive materials. Using smart materials with magnetostrictive behavior, they design high-precision devices like sensors, loudspeakers, actuators, and SONAR components. Because smart materials respond to external stimuli in different ways, their design can be based on where they will be used and for what purposes. A magnetostrictive material represents a specific type of smart material, one that responds to a magnetic field by changing its shape.

*A magnetostrictive transducer. Copyright © ETREMA.*

Terfenol-D, of which ETREMA is the only commercial manufacturer, is one example of a magnetostrictive material. First developed in the 1970s by the U.S. Navy, Terfenol-D responds to an applied magnetic field with the largest deformation of any alloy. At ETREMA, this material has proven to be a powerful resource in magnetostrictive transducer design. However, due to the nonlinearity of magnetostrictive materials and because they respond mechanically to changes in magnetic fields, designing these devices can be rather challenging. To address such challenges, a team at ETREMA turned to multiphysics simulation, accurately developing models that include several components, custom-defined materials, and multiple types of physics.

The simulation study that they conducted involved two steps. The first step was designed to provide a narrow view that analyzes individual physics. The goal here was to generate a targeted analysis of the design, enabling the engineers to easily evaluate specific physics. The second step was designed to provide an overarching view that analyzes multiple physics. In this case, the team wanted to find out how their design would work in a realistic setting by investigating its overall functionality.

As an example, let’s take a look at their closely packed SONAR source array design, which features a magnetostrictive transducer at its core. Optimizing this device prompted the need for studying its various material properties, as well as interactions between the electrical, magnetic, and structural physics.

*Images showing the components of a closely packed SONAR array. Left: The magnetostrictive transducer. Center: The transducer and power electronics. Right: The full array. Copyright © ETREMA.*

The team began their study by looking at deformation using a single-physics model. The initial study involved applying static loads to estimate fatigue in order to predict how the Terfenol-D core and prestressed bolts would react to system strain. This configuration showed severe bending between the transducer and the load. Further load analyses and structural optimization, however, facilitated the design of a transducer with reduced deformation and stress.

*Deformation in the initial transducer design (left) and the optimized configuration (right). Copyright © ETREMA.*

Another simulation study focused on the magnetic fields of the device. When developing their magnetostrictive transducer, the team of engineers added permanent magnets to the design. While this enabled them to magnetically bias the material to allow for bidirectional motion, as well as minimize nonlinear behavior and frequency-doubling effects, it was not without negative effects. Case in point: Noise problems and corrupted signals can result from stray magnetic fields that are too close to the transducer’s electronics. In an effort to avoid this, separate studies were performed for DC and AC magnetics, with the design and placement of the magnetic circuit and important electrical components also evaluated.

Looking over their simulation results, the team observed that the magnetic fields within their design stayed mostly confined to magnetic components, reducing the exposure of the electronics to the magnetic field. These results empowered the development of a magnetostrictive transducer that was optimized for the competing AC and DC magnetic requirements.

Elaborating on their single-physics models, engineers at ETREMA then used multiphysics models for design validation. This is a crucial step, as transducer technologies are focused on magnetostrictive materials, which include multiple physics. Setting up these models involved using coupled equations where strain is a function of stress and the magnetic field.

The coupled model was used to investigate the device’s deformation, with regards to mechanical stress and magnetic fields as well as its overall electromechanical characteristics. These simulation studies provided a more accurate prediction of how the design would behave in the real world.

*Coupled simulation showing the magnetic fields caused by a 1-ampere input to the coil, with displacements calculated using the maximum current input. Copyright © ETREMA.*

With their coupled linear magnetostrictive model, the team found that their device performed mostly as expected, with only a few adjustments needed. Additionally, they observed that the magnetic fields were still confined to the magnetic circuit and that deformations remained minimal. These findings were later validated by experimental data.

The simulation studies presented here showcase the flexibility of COMSOL Multiphysics and how the software can be used to analyze many different aspects of a design. In this case, engineers at ETREMA were able to develop, analyze, and optimize transducers by using both single-physics and multiphysics models. Such research has improved their knowledge of transducers and transducer designs, fostering further advancement within this field.

- Want to learn more about ETREMA’s use of multiphysics simulation? Browse these resources:
- Read a related article: “Making Smart Materials Smarter with Multiphysics Simulation“
- Watch a conference keynote presentation from Julie Slaughter about modeling magnetostrictive transducers

- See this blog post for more details on modeling magnetostriction in COMSOL Multiphysics