COMSOL 6.2 - Modeling Embedded Structures and Reinforcements

Lower dimension structural elements such as trusses, beams, and membranes can be embedded into a solid domain by adding an Embedded Reinforcement multiphysics coupling. This modeling technique is intended for efficient modeling of thin structures in solids, where it is unfeasible or not necessary to resolve the geometry of the thin structure. Some typical use cases include:

The connection between the embedded structure and the solid can be set up using different techniques; either a rigid connection by adding constraints between the points in the respective interface, or by adding springs. When a spring type connection is used, the connection can be linear or nonlinear. Using a nonlinear connection can be important when modeling reinforcement in structures, especially when predicting failure and postfailure behavior.

The multiphysics coupling is intended for situations where the volume of the embedded structure is small compared to the solid domain. Hence, no compensation is made for the mass of the small structure. If a detailed model of the connection and composite structure is required, the geometry should include the interface between the embedded structure and the solid. The connection should then be modeled using some other coupling technique as discussed in Coupling Different Element Types, or using Contact Modeling.

	When the Embedded structure is a Beam interface and a Rigid connection type is used, the displacements are only constrained to the solid domain at the mesh nodes of the beam elements. This means that higher-order variations of the displacement field between mesh nodes is allowed. The Spring connection will, however, constrain also the higher-order variations of the displacement field.

	The functionality provided by the Embedded Reinforcement multiphysics coupling to some extent overlaps with other couplings available to different structural mechanics interfaces. For example, both the Embedded Reinforcement and the Solid–Thin Structure Connection can be used to attach a membrane as a cladding on a solid domain. An important difference is, however, that the Solid–Thin Structure Connection will add constraints on the solid domain, while the Embedded Reinforcement will add constraints on the membrane. Depending on the mesh, the results may differ significantly. The same difference applies when comparing the Embedded Reinforcement to a Solid–Beam Connection on shared edges.

When modeling embedded structures, it is sometimes easier to form the geometries of the coupled interfaces from an assembly. In the finalization step of the geometry sequence, you should select in the list. This will also put less restrictions on the mesh of the respective geometry. If is selected in the list, the same mesh will be shared by both interfaces; which has to respect and resolve the geometry of the embedded structure.

While there is no strict restriction on the mesh size when modeling embedded structures in an assembly; a good practice is that the mesh used for the two coupled interfaces is of approximately the same size, or that the mesh of the embedded structure is slightly finer. Use the same shape order in both interfaces when modeling embedded structures that share the geometry and mesh with the solid domain, that is, when is selected in the list.

In some situations, the connection can be sensitive to mesh elements of the embedded structure that are partially within the solid domain. This is especially sensitive for the penalty connection, where the weak equations are evaluated at the integration points of the embedded mesh element. A slight shift in the mesh can cause an integration point to either be inside or outside the solid domain.

When using the spring type connection, the accuracy of the connection is controlled by the spring stiffness matrix. The components of this matrix are most naturally represented in the local coordinate system of the embedded structure, for which only the diagonal components are of interest. Mathematically, the spring stiffness can be viewed as penalty factors that must be sufficiently high to accurately enforce the regularized constraint, but if they are too high the overall stiffness matrix will be ill-conditioned. This means that in most cases, the spring stiffness in only a numerical parameter. However, there can be situations where the interface between the embedded structure and the solid domain has a measurable stiffness, for example, if the connection is used to idealize an interface with a finite, but small, thickness such as a glue layer. In such cases the spring stiffness will have a real physical interpretation.

The default expression for the spring stiffness of the connection is derived from the stiffness and cross-sectional properties of the mesh element of the embedded structure. The available spring connection types and the corresponding default expressions for the spring stiffness are summarized in Table 2-16. All spring stiffness components have the same default expressions.

Table 2-16: Default expression for spring stiffness.
Connection type	Spring Constant per unit length	Spring Constant per unit surface area
Truss	1e3truss.Eequ truss.area/h^2	1e3truss.Eequ truss.perimeter/h^2
Wire	1e3wire.Eequbeam.area/h^2	1e3wire.Eequ wire.perimeter/h^2
Beam	1e3beam.Eequbeam.area/h^2	N/A
Membrane	N/A	1e5mbrn.Eequ mbrn.d/h^2

Many quantities used by the connection, such as the spring stiffness and constitutive models, are most naturally represented in the local coordinate system of the embedded structure. For beam and membranes, the multiphysics coupling picks up the local coordinate system defined by the physics interface. However in the Truss or Wire interfaces, only the direction of the local edge tangent tle is defined. For the multiphysics coupling, two transverse direction are also needed when using a spring connection. Thus, the multiphysics coupling defines a local coordinate system by assuming that tle is the normal to a plane. The actual directions of the two in-plane tangents are not important, and it is assumed that the first tangent points in the global z direction. Hence, the first transverse direction is

and the second transverse direction is

where ez is the base vector that points in the global z direction. Since no distinction is made between t1 and t2, only a single transverse spring constant, kt, has to be entered when defining the spring stiffness matrix.

It is possible to include a bond slip model of the interface when modeling the embedded structure connection with a nonlinear spring. This nonlinear behavior follows a plasticity model, where the relative displacement between the two coupled interfaces is additively decomposed into an elastic displacement and a plastic displacement, or slip. Modeling bond slip is limited to small sliding only, since the mapping between the embedded structure and the solid domain is made in the reference configuration.

The slip is defined using a local constitutive model. This local model adds a set of internal degrees-of-freedom that are solved for and stored in the model at each Gauss point of the embedded structure. Typically, these internal variables include the relevant components of the slip vector ul,p, the accumulated slip upe, and the friction dissipation density Wp. The last variable is only added if the check box is selected in the section. The internal variables used by the multiphysics coupling are shown as separate fields under node in the solver sequence.

The resistance to slide in the bond slip model is determined by the cohesion c, which can be a function of any variable or field present in the model; by adding a generic expression to the initial cohesion c0. A built-in hardening model with respect to upe can be also be added, in which case c = c0+ch, where ch describes some hardening function.

In many applications the bond slip behavior of the interface is described by a Coulomb type friction. However, the bond slip model by default has no dependence on the normal force acting on the interface since the connection has no formal direction of the normal of the interface. A Coulomb type friction model can still be considered if a good estimate of the normal force can be found by adding such a dependence to c0. If, for example, the pressure in the solid domain can be considered as the normal pressure acting on the interface, use an expression like 0.1*<tag>.ExtCplOp(solid.p) to define c0 with a friction coefficient equal to 0.1. Here <tag> is the tag of the multiphysics coupling and <tag>.ExtCplOp(expr) is the operator that maps the expression from the solid domain to the embedded structure.

When adjusting the settings of the solver sequence for a model that includes an multiphysics coupling, make sure that the dependent variables of the coupled interfaces are solved in the same group. Also, note that the fields related to the bond slip model should be included in the same solver group as well. This is only a potential issue if a segregated solver is used, and it is handled automatically by the default solver suggestion.