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 edges and points which 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.
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.
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 when the Rigid Connector node has been added at the boundary or edge level.
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 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 or 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.
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 edges. The constraints are applied at the center of rotation.
For Centroid of selected entities, a subnode for selection of the entities is added to the Model Builder. The center of rotation is located at the centroid of the selected entities, which do not need to be related to the selection of the rigid connector. When points are selected, It is the geometrical location of the points that is used for computing the centroid. Any offset of the shell at the points is ignored.
-
-
For User defined, in the Global coordinates of center of rotation XC table enter coordinates based on space dimension.
For a rigid connector at edge level, when Centroid of selected entities is chosen, a default Center of Rotation: Edge or Center of Rotation: Point subnode is added, depending on the setting of Entity level.
For a rigid connector at point level, when Centroid of selected entities is chosen, a default Center of Rotation: Point subnode is added.
When a Center of Rotation: Point node is used for selection, any point in the geometry can be selected, even if it is not part of the physics interface.
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 for each spatial direction x, y, and z select one or all of the Prescribed in x, Prescribed in x, and Prescribed in z direction check boxes. Then enter a value or expression for the prescribed displacements u0x, u0y, or u0z.
Prescribed Rotation
Select an option from the By list — Free (the default), Constrained rotation, or Prescribed rotation.
For Constrained rotation select one or more of the Constrain rotation about x, Constrain rotation about y, and Constrain rotation about z axis check boxes in order to enforce zero rotation about the corresponding axis in the selected coordinate system.
For Prescribed rotation enter an Axis of rotation Ω and an Angle of rotation . The axis of rotation is given in the selected coordinate system.
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:
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 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 edges where the rigid connector is coupled to a flexible material, all nodes on such an edge 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.
Advanced
It is possible to couple rigid connectors to each other. In the Connect to list, you can select any rigid connector defined in the Solid Mechanics or Multibody Dynamics interfaces as being rigidly connected to the current one.
When the rigid connector is added at the point level, the section contains the additional Include consistency checks check box. The check box, which is checked by default, controls whether to perform singularity checks for the selections. If the checks give false positives, you can turn them off by clearing the 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.
Location in User Interface
Context Menus
Ribbon
Physics tab with Shell selected: