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“

Modular orthopedic devices, common in replacement joints, allow surgeons to tailor the size, material, and design of an implant directly to a patient’s needs. This flexibility and customization is counterbalanced, however, by a need for the implant components to fit together correctly. With parts that are not ideally matched, micro-motions and stresses on mismatched surfaces can cause fretting fatigue and corrosion. Researchers at Continuum Blue Ltd. have assessed changes to femoral implant designs to quantify and prevent this damage.

Take a few steps and see how your hips rotate. You’ll find that your body weight is continuously shifting between the left and right sides, while your legs bend, swing, and then straighten out with each step. Thus, a good modular hip replacement system will need to be able to freely allow for the natural motions of the human body — walking, running, or going up and down stairs. In addition to this, it has to be durable enough to take the continually changing, and sometimes excessive, loads placed on it during these movements, while being comprised of lightweight materials that fit and interact well with the body.

Modular implants often include stems, heads, cups, or entire joint systems. A range of materials from steel and titanium alloys to polymers and ceramics offer the surgeon many options depending on the needs of the patient. However, material and geometric selections affect the amount of wear and tear that will occur over time, so certain combinations of components are better than others. With so many different factors at play, it is not surprising that these assemblies require tight tolerances and the right material combinations to function properly and last a lifetime.

*Virtual implantation of hip replacement in resected patient femur.*

Studying how a modular combination of parts will behave under dynamic loads and stresses is a crucial part of the design and decision-making process. In order to understand the available combinations better and aid medical professionals in decisions, engineers at Continuum Blue have modeled three combinations of modular femur stem and head implants to investigate the *fretting fatigue*; the fatigue wear caused by the repeated relative sliding motion of one surface on another.

The femur head contains an angled channel for the neck of a femur stem, which in turn must be tapered correctly to fit the channel. The engineers studied three different geometric configurations using different materials for the head and stem to determine which of the three was best for minimizing fretting fatigue.

*Different stem and head configurations with an ideal fit, positive mismatch, and negative mismatch.*

Using kinematic load data from Bergmann et al. and based on averages from four patient sets, Continuum Blue created a COMSOL Multiphysics simulation to analyze the cyclic loading on a femur head. They used their model to determine the loading at different points during a walking gait cycle, knowing that the load would change at different locations in the rotation, and validated their results against the kinematic data.

*Simulation results showing the dynamic loads and stresses during the gait cycle.*

Material fatigue can be determined by studying the mean stress and stress amplitude that occur during the cyclic loading of the joint. Like the loading in the femur head shown earlier, the stresses in the femur stem will change over the course of a gait cycle. With regular leg movements, the stresses observed will take on an oscillation that reflects the repeated motion of the person walking.

*SN curves for the titanium stem and cobalt chromium head used in the study.*

Continuum Blue assessed the three configurations with two different materials: a cobalt chromium alloy for the head and a titanium alloy for the stem of the modular implant. For each material domain, they calculated the stresses observed over a single gait cycle and related these to both the SN curves of the material and the micro-motions of the contact surfaces. This allowed them to predict the number of cycles the device could undergo before fretting fatigue became an issue.

*Areas where fretting fatigue occurs over gait cycle for each configuration.*

Their results showed a surprising fact: the “ideal” fit, where the femur head channel is exactly aligned to the sides of the femur stem, was *not* found to be the best configuration for minimizing fretting fatigue. Rather, the configuration with a slight positive misalignment turned out to be a better choice, exhibiting lower stresses and overall fretting fatigue.

Through their simulation, Continuum Blue was able to predict the stress, contact pressure, and areas most susceptible to fretting fatigue at different points in a gait cycle. There are many other factors that will be accounted for in future research, such as the sensitivity of the implant to varying degrees of misalignment; additional designs and geometric changes; different materials; and the effects of surface finishes, coatings, or roughness that may impact the results. However, their modeling work offers a unique promise for evaluating the lifetime of a modular implant device. It was validated as an accurate way to predict the wear and tear that will occur for these three configurations of the implant. If you ever need a joint replacement analysis — you’ll know who to call.

- COMSOL Conference 2012 presentation: “Fretting Wear and Fatigue Analysis of a Modular Implant for Total Hip Replacement“

Ever since the first offshore wind farm was built off the Danish coast in 1991, offshore wind has been gaining in popularity. Just over two decades later, at the end of 2012, the European Union was producing enough electricity from offshore wind farms to power approximately five million households. In the coming decade, offshore wind farms are expected to generate nearly one fifth of the European Union’s power consumption, jumping from about 6.04 GW in 2013 to over 150 GW by 2030, according to a report by the European Wind Energy Association.

*Windmill park in Oresund between Copenhagen, Denmark and Malmo, Sweden. Photo credit: Ziad, Wikipedia Commons.*

With this huge increase in wind power expected, engineers are being called in to investigate the effect that offshore turbines could have on marine life. In a recent report conducted by Xi Engineering Consultants for the Scottish Government, Brett Marmo, Iain Roberts, and Mark-Paul Buckingham investigated how different types of wind turbine foundations affect the vibrations that propagate from the turbine into the sea, and ultimately how these vibrations could affect surrounding marine life. Also involved in the project were Ian Davies and Kate Brookes of Marine Scotland, who helped define the water depth, turbine size, and foundation types of the turbines modeled in the study based off of the types of turbines submitted to the Scottish Government for licensing permits. Additionally, Davies and Brookes helped identify the marine species most likely to be affected by offshore wind.

I recently interviewed Brett Marmo about the project. “In our research, we explored how different bases affect the noise that is produced by offshore turbines, and whether or not this noise was loud enough to be heard by marine life,” Marmo explained. “We studied three different wind turbine bases and examined the possible effect that noise could have on various types of local whales, porpoise, seals, dolphins, trout, and salmon.”

Vibrations produced by offshore turbines travel from the tower into the turbine foundation and are released as noise into the surrounding marine environment. “Because the noise is emitted at the interface between the foundation and seawater, it’s likely that the intensity and frequency of the noise will vary with the type of foundation used,” described Marmo. “Using finite element analysis, we modeled three identical wind turbines, only altering the structure of the foundation.”

Below, you can see the three most common foundation types: the gravity base, jack foundation, and monopile foundation. Generally, the jacket and gravity base are used in water 50 meters or deeper, while the monopile is generally not used at depths exceeding 30 meters. Due to the different structures, materials, and size of each of these bases, the vibrations that propagate through the base behave very differently, leading to noise produced with different frequencies and sound pressure levels (SPL).

*Three different foundation types are shown: a gravity base structure sitting on the seabed (left), a jacket with pin pile connections to the seabed (middle), and monopile placed onto the seabed with a transition piece (right).*

“Using simulation allowed us to model the noise produced by the foundations under identical operating conditions — something that we wouldn’t have been able to achieve by just taking measurements of in-service wind turbines,” says Marmo. “Without simulation, the different environments and wind loads that these turbines experience would have made it very difficult to determine if it was truly the foundation that was affecting the noise produced and not another unaccounted for variable.”

Before delving into the simulations, let’s first explore where it is that the noise itself comes from. Noise from wind turbines can come from two places; aerodynamic noise is produced by the blades slicing through the air, and mechanical noise is generated by machinery housed in the gearbox. Almost all of the noise produced by the blades themselves gets reflected back from the water’s surface due to the large refractive difference between the air and water, and does not enter the marine environment.

Therefore, the majority of noise is created by mechanical vibrations produced in the turbine’s gearbox and drivetrain by rotational imbalances, gear meshing, blade pass, and by electromagnetic effects between the poles and stators in the generator. Each of these noise sources produce vibrations with a different frequency, which then transmit down the turbine pole and into the foundation. Here is a table of the different frequencies produced and their origin:

Frequency | |
---|---|

Rotational imbalance of rotor | 0.05 to 0.5 Hz |

Rotational imbalance of high-speed shaft between gearbox and generator | 10 to 50 Hz |

Gear teeth meshing | 8 to 1000 Hz |

Electro-magnetic interactions in the generator | 50 to 2000 Hz |

*Frequency bands likely to contain vibration tones produced in the drive train of wind turbines. Table courtesy of Xi Engineering and adapted from their report*.

Once the vibrations enter the foundation, the amplitude of the noise emitted is affected by the size of the excitation force, the frequency of structural resonance, and the amount of damping in the structure. Additionally, higher wind speeds lead to increased torque acting on the rotor, likely meaning that higher noise is emitted.

“Understanding the effect of damping — the dissipation of vibration energy from a structure — was one of the key analyses conducted in our project,” described Marmo. “In general, steel structures such as the jacket foundation have less damping than those built from granular materials, such as the gravity base, which is made of concrete.” The amount of internal damping taking place within a structure will therefore affect the noise emitted by different structures. In order to determine how these factors affected the noise produced, Marmo and the team turned to simulation with COMSOL Multiphysics.

Noise is produced at the interface between the wind turbine foundation and seawater, where the vibration of the foundation oscillates water molecules to produce a pressure wave that radiates from the foundation as sound. Geometric spreading and absorption reduce the intensity of the sound as it propagates farther from the foundation, with high frequency sound being absorbed more quickly and low frequency sound absorbing slower and therefore propagating further.

Marmo analyzed each of the three foundations at three different wind speeds (5 m/s, 10 m/s, and 15 m/s) and found that typically, the higher the wind speed the louder the noise produced. A comparison of the average sound pressure level at a wind speed of 15 m/s at different frequencies for each of the three foundation types is shown below.

*At frequencies lower than 180 Hz, the monopile produces the largest amount of noise. Of the three foundation types, the monopile continues to produce larger SPL values up to 500 Hz. Around 600 Hz, all three foundation types become comparable in average 30 m SPL with the trend of the jacket foundation rising to become the noisiest at frequencies greater than 700 Hz.*

As the graph shows, the jacket base demonstrates the lowest sound pressure level of the three at low frequencies (around 200 Hz and lower). However, at high frequencies, the jacket produces the highest sound pressure level. The monopile and gravity base exhibit comparable sound pressure levels at lower frequencies, while at higher frequencies the gravity base produces the lowest sound pressure level of the three bases. The images below illustrate the sound pressure level around each of the three foundation types at the frequency at which the foundation produces the loudest noise.

Marmo and the team also created a far-field model that used a Gaussian beam trace model to analyze the distances at which a wind farm containing 16 turbines could be heard. As mentioned above, sound at lower frequencies tends to propagate farther than sound at higher frequencies. Additionally, ambient noise can mask the sound produced by wind turbines, making them nearly impossible to hear. This was also taken into account in Marmo’s analyses.

“We found that each of the different bases produced the loudest sound in the far-field at different frequencies,” described Marmo. “At a wind speed of 10 and 15 m/s, the monopile and gravity bases are audible at least 18 km away at most frequencies below 800 Hz, while the jacket is audible at 250 Hz 10 km away and 630 Hz at least 18 km away.” Here is a summary of these results:

The next step in the project was to determine the frequencies at which marine species could detect the sound and over what distances. Each of the different foundation types emitted different sound pressure levels at different strengths and frequencies. Since various marine animals have different hearing thresholds, this also had to be taken into account.

Cormac Booth and Stephanie King of SMRU Marine at St. Andrews University were the key marine biologists who analyzed the hearing thresholds of different marine species and determined whether or not the noise produced could affect the animal’s behavior.

*Hearing thresholds for dolphins, minke whales, porpoises, and seals.*

Of the species examined, the minke whale had the most sensitive hearing at low frequencies (less than 2000 Hz) and was able to hear the turbine from the farthest distances. “We predict that minke whales will be able to detect wind farms constructed of either monopile or gravity foundations up to 18 km away at most frequencies below 800 Hz and for all three wind speeds,” says Marmo. “On the other hand, bottlenose dolphins and porpoises are less sensitive to low frequencies. Dolphins can detect a wind farm on a gravity base 4 km away at wind speeds above 10 ms, but can only detect jackets and monopiles at close ranges of less than 1 km.”

You can view an example of the results found in Marmo’s report, showing the hearing threshold of a seal for different wind speeds and frequencies:

Determining behavior responses was harder to predict. Using a sensation parameter, Booth and King estimated the upper and lower ranges around the hearing threshold of each of the species. Then, they determined what percentage of animals could be expected to move away from the turbines within a certain sound pressure range.

Neither seal species nor bottlenose dolphins were predicted to exhibit a behavioral response to the sounds generated under any of the operational wind turbine scenarios. However, between around 4 kilometers and 13 kilometers, 10 percent of minke whales encountering the noise field produced by the monopile foundation were expected to move away. Overall, jacket foundations appear to generate the lowest marine mammal impact ranges when compared to gravity and monopile foundations.

What does this mean for the future of offshore wind power? Marmo and his team’s report found that there were little to no detrimental effects from wind turbine noise on marine species. Although more studies still need to be conducted, these findings demonstrate that the future of offshore wind is looking positive.

- Explore the full report by Xi Engineering “Modelling of Noise Effects of Operational Offshore Wind Turbines including noise transmission through various foundation types“
- “Offshore Wind May Provide One-Fifth of EU Electricity“
- Check out this resource: Cape Wind, a proposed farm that will likely become the first offshore wind farm in America

Keeping that perfectly round tire shape is important for more than just aesthetics. The lower the air pressure in a tire gets, the harder it is for the car to move forward. Every tiny leak is a source of strain for the vehicle, which can be fixed — as long as the driver is aware of the low pressure in the first place.

Tire pressure monitoring sensors, designed by Schrader Electronics, are meant to mount directly on the wheel assembly and when measurement gets below a certain pressure, a warning goes off.

I was lucky enough to speak with the researchers who work on the Schrader sensor models (their company actually builds 45 million every year). If you find yourself in a fairly new vehicle, chances are it contains a pressure sensor from Schrader. Designing these sensors for functionality and longevity is a huge part of keeping cars effective and safe.

The Schrader research team, led by Christabel Evans, tested out different shapes and components so that the sensors would last and still be able to relay measurement information back to the automobile’s dashboard without external interference. They relied on COMSOL Multiphysics together with the Structural Mechanics Module and CAD Import Module to help them choose the right parameters.

The geometry of their model consists of a circuit transmitter in a solid enclosure. The enclosure takes the brunt of the force and pressure while the wheel spins. For this reason, Schrader needed to model everything the sensor might encounter on the road, including tire fitment, vibration, and shock. They also had to factor in all of the important natural parameters, such as pressure and crush load, centrifugal force, and temperature change.

*Schrader’s tire pressure sensor fits directly into the rim of the wheel assembly. Image courtesy of Adam Wright, Schrader Electronics.*

A model showing the enclosure illustrates that different applied forces can cause deformation in the device over time. By using finite element analysis (FEA) and simulation throughout the process of product design and testing, Schrader was able to isolate or couple variables as needed, allowing them to work towards the best design. This gave them the flexibility to build and refine as they went.

*10x amplification of stress and deformation on the transmitter housing as a result of centrifugal loading, which is produced by the wheel’s rotation.*

As they narrowed down the best design, Schrader also simulated the equipment used for testing the device rotating on the tire. They mapped where the greatest stress occurred and found that it mostly took place along the bolts of the collar. This allowed them to make all of the necessary adjustments to reinforce those areas and continue to optimize the design as they worked.

*The spin test works at a very high speed, simulating conditions the sensors are exposed to. The model shows an increase in stress along all of the sections of the model where bolts are located.*

Perhaps the most useful feature in COMSOL Multiphysics (for the Schrader engineers) was the ability to test various parameters, shapes, and designs. It was much easier to get the most out of their computational power by running several models simultaneously. As they continue their research, they plan to keep focusing on failure analysis to fortify their design and continue to improve their product’s accuracy and life span.

- Learn more about how Schrader used simulation to drive their product design by reading the full-length story “Optimizing Built-in Tire Pressure Monitoring Sensors” in
*COMSOL News 2014*.

The outcome of your golf stroke is basically determined by the movement of the club head just prior to impact with the ball. Considering this, we should be able to see how your golf swing could be improved based on a multibody analysis.

Here, I will show you how I went about modeling various body parts, a golf club, and the connections among them using the Multibody Dynamics Module.

A simple way to simulate a golf swing is by using a *two-link model*, where the arm and club are the two links connected together by a hinge joint. In this model, the arm rotates about a fixed point, located at the base of the neck, and the club rotates about the wrist joint relative to the arm. The two-link model does not allow a sufficiently long backswing and is not actually a true representation of a real-life golf swing.

A better representation is the *three-link model*, which also includes the shoulder as a separate link. Adding one more link eliminates the problem related to the backswing. Hence, we will use this three-link model in our analysis.

*Diagram of the two-link and three-link swing models.*

This analysis focuses on maximizing the club head speed just prior to impact with the ball, by understanding the mechanics of a golf swing. The torque profile, applied by different body parts (shoulder, arms, and wrist) is assumed. It is limited by the maximum torque capacity of the respective parts. Among all applied torques, the wrist torque has quite an important role to play in getting the strike right.

*Modeled geometry of the three-link swing model.*

While simulating the downswing of the club, the entire swing can be divided into two phases. In the first phase, arm and club rotate about the fixed point as a rigid assembly. In this phase, the arm and club are folded to minimize the inertia about the center of rotation, which allows the development of maximum angular velocity for the given arm-torque capacity. Here, the wrist is cocked to the maximum possible angle (the amount it can be cocked before you become uncomfortable or the angle is detrimental to your swing) and the applied wrist torque tries to hold back the club in this position against the other two torques.

In the second phase, the wrist torque starts helping the shoulder and the arm torque by pushing the club forward to increase the club head speed to its maximum. The instance when the wrist torque changes its role is a crucial parameter in determining the stroke quality. To see its effect on the club head speed, we vary the wrist torque parametrically.

*Time history of torque applied by the shoulder, arm, and wrist for (t_w = 0.19 s).*

The driving torque, applied by the shoulder, arm, and wrist, has a maximum capacity and can vary within the defined range. The applied shoulder torque is assumed to start at its maximum positive value, after a short build-up time. The applied arm torque, which acts on the arm and reacts on the shoulder, builds linearly with time to its maximum positive value with the specified rate. The applied wrist torque, which acts on the club and reacts on the arm, is fully negative to start and switches to its maximum positive value at the specified time (t_w).

On the arm and wrist joint, the rotation is not fully free. It is limited in the forward and backward directions by the ligaments, muscles, joint shape, or a combination of all these. In our golf-swing analysis, rotation limit in the backward direction is more important and this limiting value may vary from person to person.

In the beginning of the downswing, due to inertial forces on the body parts, these rotations try to go below the limiting value. Hence, additional torque is applied by the equivalent stiffness and damping of the stop. This makes the *effective* torque applied by the arm and wrist more than what is actually *applied*.

*Golf club head speed during the downswing for different wrist torque switch times (t_w).*

Above, I have plotted the club head speed for various wrist torque switch times (t_w) for the entire duration of approximately 0.25 seconds. It can be observed that for t_w = 0.15 s, we reach the maximum speed before impact — this leads to early hitting. On the other hand, for t_w = 0.23 s, the club head speed couldn’t even reach its maximum value.

For t_w = 0.19 s, the club head speed is higher than the other two cases and close to the optimum value for the given geometrical parameters and muscle strength.

*Comparison of the golf club trajectory for different values of t_w (results are displayed in the increasing values of t_w).*

*Motion of links and the trajectory of arm joint, wrist joint, and the golf club head.*

Maximum arm torque throughout the swing and very high arm speed in the beginning of the downswing can cause an early release, with the club head reaching its maximum speed before actually hitting the ball.

We can also deduce that for the given torque capacity, it’s potentially advantageous to have a long arm swing as well as a large wrist-cock limit angle. Furthermore, the extent to which the wrist can *hold back* the release is limited by its torque capacity. Therefore, your golfing skills are also strongly associated with the delayed release and the late hit.

In the downloadable model, we also consider the shaft flexibility by dividing the club into two parts: the grip and the shaft. These are connected through a hinge joint with finite stiffness and damping. You can see that the effect of the shaft flexibility to the swing is negligible compared to other parameters.

- Check out our Golf Swing model in the Model Gallery for more information. If you log into your COMSOL Access account, you can download the MPH-file and documentation for this model.
- Check out our archived webinar on Multibody Dynamics Simulation
- Explore the Multibody Dynamics Module and Structural Mechanics Module

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

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

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

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

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

(1)

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

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

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

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

(2)

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

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

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

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

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

(3)

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

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

Combining the last two expressions, we get the following:

(4)

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

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

(5)

The elastic bending theory gives the recovered elastic stress as:

(6)

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

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

(7)

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

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

(8)

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

Therefore, the residual stress is then deduced as:

(9)

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

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

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

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

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

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

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

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

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

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

*Analytical vs. computed residual stresses.*

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

*Hysteresis behavior after three loading-unloading cycles.*

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

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

*Hysteresis behavior with kinematic strain hardening.*

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

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

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

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

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

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

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

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

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

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

*Simulation of sheet metal forming.*

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

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

Learn more about the related products:

]]>