学习中心

Modeling Structures by Coupling Structural Mechanics Interfaces

---

Using the COMSOL Multiphysics^® software and its add-on Structural Mechanics Module, you can model a combination of different types of structures, such as solid, slender, and thin structures. This modeling is accomplished by implementing couplings between the physics interfaces for each structure type. There are different techniques for making such connections, including:

• Adding multiphysics couplings
• Using prescribed displacements
• Renaming dependent variables
• Using multibody attachments and joints

Here, we outline how to implement each of these approaches to couple the structural mechanics interfaces in your model. We also discuss some other considerations you need to be aware of when using multiple structural mechanics interfaces in the same model to model a structure.

Background of Structural Mechanics Interfaces

In COMSOL Multiphysics^®, the different structural mechanics element types are represented by different physics interfaces, such as the Solid Mechanics, Shell, and Beam interfaces. The following table lists the interfaces, the applicable spatial dimensions, geometric entities, and the types of structures they are intended for.

Interface	Spatial Dimensions	Geometric Entities	Type of Structures
Solid Mechanics	3D 2D 2D axisymmetric 1D 1D axisymmetric	Domain	Any structure
Shell	3D 2D axisymmetric	Boundary	Thin, flat or curved structures with significant bending stiffness
Plate	2D	Domain	Thin, flat structures with significant bending stiffness
Membrane	3D 2D axisymmetric	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
Wire	3D 2D	Edge (3D) Boundary (2D)	Slender members that can only sustain tensile axial forces, cables, and wires

Every physics interface has its own set of dependent variables, meaning that two different interfaces are not aware of each other even when they share geometry. Thus, some type of additional coupling is needed. This concept is true for interfaces of the same physics type, such as two structural mechanics interfaces, as well as interfaces for different physics fields, like solid mechanics and heat transfer or shells and acoustics. 

Adding Multiphysics Couplings

There are multiple features available for automating coupling between various combinations of structural mechanics interfaces. Such features are added as predefined multiphysics couplings, where, in this context, they administer coupling between different structural interfaces. You can see what predefined multiphysics couplings are available for your application by adding the relevant structural mechanics interfaces into a single model and then either right-clicking the Multiphysics node or, under the Physics ribbon tab, clicking the Add Multiphysics button.

A cropped screenshot of the Model Builder with the Multiphysics node selected, showing the dropdown menu of available coupling features. The list of multiphysics couplings available for automating coupling between various combinations of structural mechanics interfaces. Here, for demonstration purposes, all structural mechanics interfaces have been added to enable viewing of the entire list of options.

Adding and configuring the settings for a multiphysics coupling is generally handled similarly for all features. As such, the information here can be extended to any coupling features not explicitly discussed.

Solid–Thin Structure Connection 

To couple a solid domain and thin structure such as a shell, the Solid–Thin Structure Connection node can be used. In the Coupled Interfaces section of this connection, you can choose between two types of solid interfaces: Solid Mechanics and Multibody Dynamics. For the Thin Structure setting, you can choose either the Shell interface or the Membrane interface. If you choose the Membrane interface, then the only available Connection Type is Shared Boundaries, which is applicable to a scenario where a thin membrane is used as a cladding on top of the face of a solid. The selection is, by default, all boundaries that are shared between the two interfaces. If you need to make another selection, you can select Manual Control of Selections.

When a Shell interface is selected in the Coupled Interfaces section, two new options for Connection Type become available in the Connection Settings section: Parallel boundaries and Solid boundaries to shell edges. The first option, Parallel boundaries, is straightforward and similar to Shared Boundaries. However, with Parallel boundaries, the distance is taken into account so that the rotation in the shell is connected to the displacements in the solid. It's also important to note that two parallel boundaries might not match in the geometry or the mesh. With the Parallel boundaries connection type, data is mapped from one boundary to another, but only on the parts of the boundaries where they match.

The Connection type menu is highlighted in the Solid–Thin Structure Connection settings window, with the Graphics window showing the associated surfaces of the model in yellow and brown. In the Solid–Thin Structure Connection settings window, the thin structure is set to Shell and the connection type is set to Parallel boundaries.

In order to know what parts the automatic couplings have connected, there are built-in variables called connected region indicators, from which a Connected Region Indicator plot can be generated (through the respective option under Results Templates by right-clicking the Results node). The following image shows an example where the parallel boundary on which the Shell interface is active is somewhat larger than the solid to which it is connected.

A gray block split into several smaller tetrahedra, separated by a gap from a surface, with both a red and a gray region split into several triangles. A Connected Region Indicator plot for an example model consisting of a solid block and a shell in parallel. The model uses the Solid–Thin Structure Connection node to couple the shell and corresponding block face under it. The connected region is indicated in red. The model is available here.

The other type of connection available between shells and solids is Solid boundaries to shell edges. This type of coupling can be used to make a highly accurate transition from a shell to a solid. If large parts of your structure consist of thin parts, using solids where it is really necessary can provide significant savings in computer resources in terms of memory, meshing time, and solution time.

When modeling this type of connection, you can choose between two methods: Flexible or Rigid. The flexible method is more accurate and gives a coupling that is almost completely free from artifacts or artificial stiffening. It does, however, require that the solid is modeled with at least three elements in the thickness direction. This method will add a set of three extra degrees of freedom (DOFs) at each node along the shell edge.

The model tree with a node under the Solver Configurations node selected. The model tree for the shell-to-solid example pictured above.

The model tree with the Compile Equations node selected and the Settings window. The statistics for the Stationary study step, in which we can see the number of DOFs for the model. To learn about estimating and computing the number of DOFs, see this article.

You can connect shells to solids in other configurations, in which case the Rigid method is preferred. The Flexible method is based on the assumption that the stress state in the solid is the same as in the shell.

The following example is of a connection where the thickness does not match, and the shell is connected to the solid at an angle. Again, the coupling is visualized using either a Surface plot or a Shell dataset.

Also in this case, the Connected Region Indicator plot is useful for ascertaining the correctness of the connection.

A close-up view of a block connected to a slanted shell in a wireframe rendering, with a region of the connected surface colored in red. The Connected Region Indicator plot for the example model of a solid domain coupled to a shell at an angle, with red indicating the location of the connection.

Note that by default, the shell thickness is used in such a way that the angle is taken into account. Here, the height of the connection region is sqrt(2)*shell_thickness since the shell is connected at 45 degrees. In addition to the default connection region based on shell thickness, you can manually select the distance from the shell midsurface, or select entire boundaries on the solid.

Shell–Beam Connection

Next, let's have a look at connections between beams and shells, using the multiphysics coupling Shell–Beam Connection coupling. It has four connection types:

• Shell edges to beam points
• Shared edges
• Parallel edges
• Shell boundaries to beam points

These various connection types are demonstrated in the Connecting Shells and Beams tutorial model.

The Shared Edges and Parallel Edges connection types are mainly used when beams act as shell stiffeners. Use Parallel Edges when there is a separate edge at the beam centerline. When using Shared Edges, the beam is placed in the same plane as the shell, and you provide its true location by giving the offset from the common edge.

The two other options, Shell edges to beam points and Shell boundaries to beam points, are used for connecting the end of a beam to a shell, either at an edge or inside a boundary. In either case, you typically want to connect a small part of the object only, a part that is representative of the beam cross section. By default, the software will automatically choose a connection region based on the beam cross-section size.

The model tree with the Shell–Beam Connection coupling selected and the Settings window with the Connection Settings section expanded, showing the dropdown menu of options for the connection type. The options for Connection type for Shell–Beam Connection.

Solid–Beam Connection

The Solid–Beam Connection coupling has similarities with both the Solid–Thin Structure Connection and Shell–Beam Connection coupling nodes.

The model tree with the Solid–Beam Connection coupling feature selected and the Settings window with the Connection Settings section expanded, showing the dropdown menu of options for the connection type. The options for Connection type for Solid–Beam Connection.

The Solid boundaries to beam points, transition connection type is similar to the transition between shells and solids. The underlying assumption is that the connected solid represents a beam with the same cross section used in the Beam interface. When this type of coupling is used for a noncircular cross section, it is possible to improve the accuracy by including warping deformation. When doing that, extra DOFs are added on the connected boundary of the solid. Solving for these extra DOFs efficiently requires a special solver configuration, as seen in the Connecting Beams and Solids tutorial model. The Solid boundaries to beam points, general connection type is used if the end of a beam is attached to an arbitrary surface of a solid. The Solid boundaries to beam edges connection type is intended for beams connected in parallel to a solid boundary, as indicated below.

A gray block with a small yellow beam on top. An example geometry providing a representation of the connection between a beam and the boundary of a solid in parallel, which illustrates the Solid–Beam Connection coupling.

The Solid edges to beam points connection has one important use case: When modeling bolts with beams, the beam at the center of a bolt hole can be connected to the circular edge around the hole, as seen in the Modeling of Pretensioned Bolts tutorial model. For other types of modeling, you must consider how the physical reality matches the properties of the element types. Since the solid does not have any rotational DOFs, any bending and torsional stiffness of the coupling must come from geometrical effects. If, for example, you connect the beam to a straight edge, then the edge will act as a hinge from the perspective of the beam.

Layered Shell–Shell Connection

Use the Layered Shell–Shell Connection node when you want to combine the Layered Shell and Shell interfaces so that some layers in a layered structure are modeled using the Shell interface. The main reason for doing so is that some layers are very thin, in which case the Shell interface offers a more economical and accurate option, as demonstrated in the Analysis of a Composite Blade Using a Multiple Model Method tutorial model.

Layered Shell–Structure Transition

The Layered Shell–Structure Transition node can be used to create a coupling between a layered shell and either a solid or an ordinary shell. In the case of solids, the node is similar to the Solid–Thin Structure Connection feature in that the edge of the shell is connected to the face of a solid. For shells, the node offers a coupling between a layered shell and a nonlayered shell across a common edge. Usage of this node is demonstrated in the Connecting Layered Shells with Solids and Shells tutorial model.

Lumped–Structure Connection

The Lumped–Structure Connection node is used for connecting terminals in a Lumped Mechanical System interface to a standard finite element model. The structural elements can be of any type. Using this technique, you can model subsystems by a simplified mass–spring–damper approach, and then connect to a detailed finite element model of the important parts. Note that since a lumped mechanical system is a scalar representation of a system, it is not until it is used in a multiphysics coupling that it is actually acting in a certain spatial direction. Use of this feature is demonstrated in the Lumped Model of a Vehicle Suspension System tutorial model.

Embedding Elements

The ability to embed elements of a lower dimension into solid elements is also available as a predefined coupling option in the software by adding the Embedded Reinforcement node to your model. You can embed truss, beam, wire, and membrane elements in solids without having to consider matching geometry or mesh. This functionality is typically used for various types of reinforcements. It is also possible to allow a bond slip between the embedded elements and the surrounding solid.

A long, rectangular, gray block with thin layers on the top and bottom that both contain an array of line segments. The geometry for the tutorial model of a concrete beam reinforced with steel bars (rebars), focused on one end of the concrete beam. The rebars are modeled using the Truss interface and the concrete is modeled using the Solid Mechanics interface. Coupling between the structural interfaces is done through the Embedded Reinforcement node.

It should be noted that the local stresses in the solid elements in which other elements are embedded may not be accurate. If there are many embedded elements, like a set of closely spaced reinforcement bars, it may be a better approach to consider the embedding as continuous. You can either choose to embed membranes with an equivalent (possibly orthotropic) stiffness, or use the Fiber feature, which provides fully continuous representation. This concept is explained in further detail on the Modeling Embedded Structures and Reinforcements page in the COMSOL documentation.

Using Prescribed Displacements

One straightforward way to couple different structural mechanics interfaces is by making the displacements match. This approach involves taking the displacement field from one physics interface and then entering its displacement variable into the other physics interface, forcing it to have the same displacement. To implement this approach, add a Prescribed Displacement node or Prescribed Displacement/Rotation node in one of the interfaces, and enter the displacement variable from the other interface in the node settings.

A simple example that demonstrates the use of this approach is pictured below, in which two horizontal beams are connected by a diagonal wire. In the Beam interface, the translational DOFs are named u and v. In the Wire interface, the DOFs are named u2 and v2. Note that the Prescribed Displacement node should only be added to one of the interfaces.

If the model geometry has been finalized using Form Union, whereby the two interfaces are connected at a common geometrical object, the approach shown above is sufficient. If Form Assembly has been used instead, there may be coincident but nonidentical geometrical objects. In this case, use a coupling operator to obtain the displacements from the other interface.

If we assume that the example structure above is instead an assembly, one approach would be to apply an Average operator to each endpoint of the wire and then add a Prescribed Displacement node for each endpoint of the wire (model available here). In the settings for the prescribed displacement, you would then call out the nonlocal coupling operator and use the dependent variable from the Beam interface as the expression.

Renaming Dependent Variables

One simple method for coupling structural mechanics interfaces is to adjust the names of the dependent variables so they are the same and thus the interfaces use the same values. In a situation like we mentioned earlier, placing a thin membrane on top of the face of a solid would require adding two interfaces.

Adding the Solid Mechanics interface first would result in a displacement field named u with the components u, v, and w. Then adding the Membrane interface, the resulting displacement field would be called u2 with the components u2, v2, and w2. To couple the interfaces, edit the field name and change it from u2 to u. This approach works as long as the DOFs physically represent the same quantity (in this case, displacements) and there is a union between the geometric entities of the structural interfaces being coupled. It is a sufficient method when, for example, using membranes as cladding on a solid boundary or truss elements as reinforcement bars in a solid.

Note, however, the following exceptions to using this technique:

• The shape functions used in the Beam interface have special properties. A beam cannot have the same DOFs 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 DOF names for the rotational DOFs.

There are two other possible methods for modeling the structure outlined above: You could implement the coupling using one of the predefined multiphysics couplings (discussed later in this article). You could also avoid the need for including the second interface, the Membrane interface, by instead using the Thin Layer feature in the Solid Mechanics interface for the same effect. This approach enables you to use a boundary condition for handling the thin region instead of explicitly modeling thin domains in your structure.

Using Multibody Attachments and Joints

Using COMSOL Multiphysics^® with the add-on Multibody Dynamics Module, you also have the option to couple structural interfaces by connecting them through joints and multibody attachments. Joints are available under the Multibody Dynamics interface as well as in the dedicated Joints interface. Attachment nodes can be added in the Multibody Dynamics, Solid Mechanics, Shell, and Beam interfaces. To use this coupling method, you need to add an Attachment node in each of the interfaces you want to connect. The two attachments are then connected using a joint, which can have many properties. The attachment formulation is similar to the rigid connector, and all the selected boundaries or edges behave as if they are connected by a common rigid body. The various joints available in the Multibody Dynamics Module use these attachments to couple the interface with any other interface.

Consider the Vibration in a Washing Machine Assembly tutorial model, which demonstrates this coupling method, in which a horizontal axis washing machine is modeled using the Multibody Dynamics interface and Shell interface. To couple the two interfaces, attachments are first 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. A similar procedure is used to model the front and back springs present on the front and back panels of the housing.

The model geometry for a washing machine with some of the exterior surfaces hidden for visibility into the design. The Vibration in a Washing Machine Assembly tutorial model geometry outer housing of the assembly (selected, blue) is made up of shell elements, while the inner components (not selected, gray) are rigid and are modeled using Rigid Material nodes in the Multibody Dynamics interface.

Considerations When Modeling with Several Structural Interfaces

Solver Settings When Coupling Structural Interfaces

Whenever there are multiple interfaces in a model, the default solver will suggest a segregated solver sequence. However, it is not possible to solve a coupled model if the structural mechanics DOFs 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 DOFs in one segregated step. The latter approach is useful when the model also contains physics interfaces from other physics fields, like heat transfer, fluid flow, or electromagnetics.

Features That Need To Be Duplicated

Some features typically need to be added in each physics interface in order to create a model that is consistent. Examples include:

• Gravity
• Rotating Frame
• Linearly Accelerated Frame
• Base Excitation

If using these features, it is good practice to create parameters under Global Definitions and use them throughout your model. When you change the value of the parameter, your model will use the new value everywhere the parameter was entered.

In some cases, constraints may also have to be given in more than one interface. When a constraint is included in multiple structural interfaces, it is important to identify any overlapping constraints to avoid potential conflicts. The software automatically handles conflicts via constraint elimination, but you can also remove potentially conflicting constraints manually, which may be necessary in some cases. Consider the example pictured below, which involves a solid–shell coupling meeting a symmetry plane.

A transparent gray block with dark shading on the surface that is the symmetry plane, purple shading on the surface that is the solid boundary, a red line that is the conflicting edge, a blue line that is the shell edge, and a black line that is the symmetry edge. An example model geometry of a solid–shell coupling meeting a symmetry plane. The solid boundary (magenta) and shell edge (blue) result in conflicting constraints (red) on an edge in the model.

In this example, the Solid–Thin Structure Connection feature couples the displacements of the solid and shell (with the shell DOFs controlling the displacement). A Symmetry boundary condition is included under the Shell interface and applied to the symmetry edge, and a Symmetry boundary condition is included under the Solid Mechanics interface and applied to the boundary on the symmetry plane.

The conflict occurs at the edge that lies on the symmetry plane and also exists on the solid–shell coupled boundary. It occurs as a result of both symmetry conditions resulting in overlapping constraints applied to the same edge. This scenario is explained in further detail in the Suppressing Constraints on Lower Dimensions section of the COMSOL documentation.

Features That Must Not Be Duplicated

There is one case where adding the same feature in more than one physics interface would give erroneous results: when using the Rigid Motion Suppression node. This feature adds a set of constraints that are necessary to keep a structure physically and numerically stable without causing internal stresses when external loads are self-equilibrating. Apply it once to the connected structural system; adding it in multiple interfaces would overconstrain the structure.

Using Rigid Connector

The Rigid Connector feature can be used to create virtual rigid objects and connections across several physics interfaces, using a special technique: Add one Rigid Connector node in each of the involved interfaces, and then make the selection for the parts in that interface. In the Advanced section of the settings for the Rigid Connector node for one of the interfaces, you can then couple a rigid connector in another physics interface. The same center of rotation should be used in all coupled rigid connectors. This method is essentially the same as adding two Attachment nodes and then connecting them using a Fixed Joint feature.

The Settings window for the Rigid Connector feature, with the Advanced section expanded. The Settings window for the Rigid Connector feature, with the Center of Rotation and Advanced sections expanded.

Further Learning

• COMSOL documentation:
  • Couplings Between Structural Mechanics Interfaces
  • Coupling Different Element Types
  • Nonlocal Coupling and Coupling Operators
• Learning Center article:
  • The Usage of Form Union and Form Assembly
• Blog post:
  • Part 2: Mapping Variables with General Extrusion Operators