Rigid Connector
The Rigid Connector is a boundary condition for modeling rigid regions and kinematic constraints such as prescribed rigid rotations. A rigid connector can connect an arbitrary combination of boundaries, edges, and points that all will move together as being attached to a virtual rigid object.
You can add the Rigid Connector node at the boundary, edge, and point levels.
When the selection consists of boundaries only, you can also choose to remove the assumption of rigidity, while still respecting force and moment equilibrium. With this formulation, it is possible to avoid artificial constraint effects at the connected boundaries.
If the study step is geometrically nonlinear, the rigid connector takes finite rotations into account.
Rigid connectors are available in the Solid Mechanics, Multibody Dynamics, Shell, Beam, and Pipe Mechanics interfaces. Rigid connectors from different interfaces can be attached to each other.
You can add functionality to the rigid connector through the following subnodes:
Applied Force (Rigid Connector) to apply a force in given point.
Mass and Moment of Inertia (Rigid Connector) to add extra mass and moment of inertia in a given point.
Spring Foundation (Rigid Connector) to add a translational or rotational spring or damper in a given point.
When physics symbols are shown, a rigid connector is represented by a symbol at the center of rotation, together with a set of lines connecting the center of rotation with the centers of gravity of the selected entities.
The Rigid Connector node is only available with some COMSOL products (see https://www.comsol.com/products/specifications/). Rigid Connector is available for 3D and 2D.
Shell Properties

Interface Selection

Boundary Selection
This section is present when the Rigid Connector node has been added at the boundary level. Select one or more boundaries to be part of the rigid region.
Edge Selection
This section is present in 3D when the Rigid Connector node has been added at the boundary or edge level, and Connection Type is Rigid.
When the Rigid Connector is added at the edge level, select one or more edges that form part of the rigid region.
When the Rigid Connector is added at the boundary level, this section is initially collapsed. Here, you can add optional edges to the rigid region. The edges cannot be adjacent to the selected boundaries.
Point Selection
This section is always present when Connection Type is Rigid.
When the Rigid Connector is added at the point level, select a number of points that form the rigid region.
When the Rigid Connector is added at the boundary or edge levels, this section is initially collapsed. Here, you can add optional points to the rigid region. The points cannot be adjacent to the selected boundaries or edges.
Coordinate System Selection
The Global coordinate system is selected by default. The Coordinate system list contains all applicable coordinate systems in the model. Prescribed displacements and rotations are specified along the axes of this coordinate system. It is also used for defining the axis directions of the moment of inertia tensor of the Mass and Moment of Inertia subnode.
Connection Type
Select Rigid or Flexible. When the connection type is rigid, the whole rigid connector acts as a virtual rigid object. In the flexible formulation, the selected boundaries are allowed to have internal deformations, and the kinematic constraints are fulfilled only in an average sense. The flexible formulation is useful for example when applying loads, since it will reduce local constraint effects.
If a selected boundary is located on a rigid domain, the connection type setting does not matter. The rigid formulation is always used,
The Connection Type section is shown only when the Rigid Connector has been added at the boundary level.
When the connection type has been set to Flexible, the Edge Selection and Point Selection sections are hidden.
If, however, an existing solver sequence was generated while Connection Type was set to Rigid, and you then change to Flexible, no such scaling will be present. In this case, you either have to regenerate the solver sequence, or set the scaling manually under the Dependent Variables node in each study step.
Center of Rotation
The center of rotation serves two purposes.
Select a Center of rotationAutomatic, Centroid of selected entities, or User defined.
For Automatic, the center of rotation is at the geometrical center of the selected geometrical objects of the highest geometrical dimension.
For Centroid of selected entities select an Entity levelBoundary, Edge, or Point. The available choices depend on the physics interface and geometrical dimension.
When Entity level is set to Point, any point in the geometry can be selected, even if it is not part of the physics interface.
For User defined, in the Global coordinates of center of rotation XC table enter coordinates based on space dimension.
Select the Offset check box to add an optional offset vector to the definition of the center of rotation. Enter values for the offset vector Xoffset.
The center of rotation used is the sum of the vector obtained from any of the input methods and the offset vector.
Prescribed Displacement at Center of Rotation
To define a prescribed displacement at the center of rotation for each space direction, select one or several of the available check boxes then enter values or expressions for the prescribed displacements. The direction coordinate names can vary depending on the selected coordinate system.
For 3D components: Prescribed in z direction u0z
Prescribed Rotation
Specify the rotation at the center of rotation. Select from the By list: Free, Constrained rotation, or Prescribed rotation about the center of rotation.
For 2D components, the Constrained rotation and Prescribed rotation is always about the z-axis, so no component selection is necessary.
Constrained Rotation (3D Components)
For Constrained rotation select one or more of the available check boxes to enforce zero rotation about the corresponding axis in the selected coordinate system:
Constrain rotation about x-axis
Constrain rotation about y-axis
Constrain rotation about z-axis
Prescribed Rotation
For Prescribed rotation enter an Angle of rotation ϕ0. For 3D components also enter an Axis of rotation Ω for the x, y, and z coordinates.
Released Degrees of Freedom
In some cases it can be useful to not constrain the displacement in a certain direction. For instance, the radial displacement of a Rigid Connector acting on a circular cross-section could be allowed to be free. To do so, select a local Coordinate system for specifying the directions in which the degree of freedom will be released. The Coordinate system list contains only applicable coordinate systems in the model.
Select one or more of the available check boxes to release the displacement in the corresponding axis in the selected coordinate system:
Release displacement in x1 direction
Release displacement in x2 direction
For 3D components: Release displacement in x3 direction
Note that the Rigid Connector solves for global displacement degrees of freedom (DOFs) and global rotation DOFs – unless they are explicitly prescribed. Since releasing certain displacement field components reduces the number of equations used to solve for the global DOFs, it may become necessary to constrain some global displacement or rotation components to achieve static determinacy.
The section Released Degrees of Freedom is only shown if Connection Type is Rigid (if applicable), and if the check box Use weak constraints for rigid-flexible connection in the section Constrain Settings is not enabled.
Reaction Force Settings
Select Evaluate reaction forces to compute the reaction force caused by a prescribed motion. The default is to not compute the reaction force. When selected, the prescribed motion is implemented as a weak constraint.
Select Apply reaction only on rigid body variables to use a unidirectional constraint for enforcing a prescribed motion. The default is that bidirectional constraints are used. This setting is useful in a situation where a bidirectional constraint would give an unwanted coupling in the equations. This would happen if the prescribed value of the motion is a variable solved for in other equations.
Formulation
Some contributions from a rigid connector will, under geometric nonlinearity, result in a nonsymmetric local stiffness matrix. If all other aspects of the model are such that the global stiffness matrix would be symmetric, then such a nonsymmetric contribution may have a heavy impact on the total solution time and memory usage. In such cases, it is often more efficient to use an approximative local stiffness matrix that is symmetric.
Select Use symmetric formulation for geometric nonlinearity to force all matrix contributions from the rigid connector and its subnodes to be symmetric.
Constraint Settings
On the boundaries where the rigid connector is coupled to a flexible material, all nodes on such a boundary are constrained to move as a rigid body. As a default these constraints are implemented as pointwise constraints. If you want to use a weak constraint formulation, select Use weak constraints for rigid-flexible connection.
This formulation cannot be combined with the Flexible formulation of the rigid connector, which in itself is a special form of weak constraint.
Advanced
When the rigid connector is added at edge or point level, automatic tests are performed to check for selections that would result in a singularity. If these checks give false positives, you can turn them off by clearing the Include consistency checks check box. This could, for example, be necessary if a rigid connector, which in itself is singular, is connected to another one in a way that forms a stable configuration.
When the Rigid Connector is added at the point level, select the Add rotational stiffness for two-point selection check box to automatically suppress singularities when the Include consistency checks check box is disabled. This check box allows to enter a rotational stiffness, kθ, to stabilize the rigid connector. The rotational stiffness is only added if less than three points are selected.
Select Group dependent variables in solverFrom physics interface (default), Yes, or No, to choose how to group the dependent variables added by the Rigid Connector feature in the solver sequence.
You can add a Harmonic Perturbation subnode for specifying a harmonic variation of the values of the prescribed displacements and rotations in a frequency domain analysis of perturbation type.
Assembly with a Hinge: Application Library path Structural_Mechanics_Module/Connectors_and_Mechanisms/hinge_assembly
Location in User Interface
Context Menus
Ribbon
Physics tab with Solid Mechanics selected:
Physics tab with  Layered Shell selected:
Physics tab with Multibody Dynamics selected: