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 edge and point levels.
•
When added at the edge level you can connect edges and points as long as at least one edge is selected. Selecting points is optional.
•
When added at the point level, you can connect a set of points to each other.
If the study step is geometrically nonlinear, the rigid connector takes finite rotations into account.
The feature is similar to the rigid connectors in the Solid Mechanics and Beam interfaces. Rigid connectors from the Shell, Beam, and Solid Mechanics 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.
•
Applied Moment (Rigid Connector) to apply a moment.
•
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.
Edge Selection
This section is present when the Rigid Connector node has been added at the edge level. Select one or more edges to be part of the rigid region.
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 edge level, this section is initially collapsed. Here, you can add optional points to the rigid region. The points cannot be adjacent to the selected edges.
Coordinate System Selection
The Global coordinate system is selected by default. The Coordinate system list contains any additional coordinate systems that the model includes. 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.
•
If you prescribe the displacement of the rigid connector, this is the place where it is fixed.
•
Results are interpreted with respect to the center of rotation.
Select a Center of rotation — Automatic, 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 when the main selection is at edge level, select Entity level — Edge or Point. 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 edges to which the rigid connector is attached. As a special case, you can select a single point, and thus locate the center of rotation at a certain point.
•
For Centroid of selected entities when the main selection is at point level, a subnode for selection of the points is added to the Model Builder. The center of rotation is located at the centroid of the selected points, which do not need to be related to the points to which the rigid connector is attached. As a special case, you can select a single point, and thus locate the center of rotation at a certain point.
•
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.
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 Y, and Prescribed in Z direction check boxes. Then enter a value or expression for the prescribed displacements u0, v0, or w0.
Prescribed Rotation at Center of Rotation
Select an option from the By list — Free (the default), Constrained rotation, or Prescribed rotation at center of 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 at center of rotation enter an Axis of rotation Ω and an Angle of rotation . The axis of rotation is given in the selected coordinate system.
•
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.
•
You can activate and deactivate the rigid connector by assigning it to a constraint group. See Load Cases in the Structural Mechanics Modeling chapter.
•
You can assign the value of the prescribed displacement and rotation to a load group. See Load Cases in the Structural Mechanics Modeling chapter.
•
Rigid Connector Theory
•
Harmonic Perturbation
•
Load Cases
Location in User Interface
Context Menus
Shell>Connections>Rigid Connector
Ribbon
Physics tab with Shell selected:
Edges>Connections>Rigid Connector