COMSOL 6.3 - Rigid Connector

Rigid Connector

The is a boundary condition for modeling rigid regions and kinematic constraints such as prescribed rigid rotations. The selected points will move as a single rigid object.

You can add the node at the edge (2D: boundary) 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.

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.

•

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.

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.

•

When the rigid connector is added at the edge level, such symbols are shown only for the selected edges, but not for auxiliary selections of points.

•

Because of the way physics symbols are evaluated, as a lightweight operation when moving between physics nodes in the model builder tree, it is sometimes not possible to determine the center of rotation. In particular, if an offset is supplied, it will not be taken into account.


	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.


	Boundary Selection This section is present when the Rigid Connector node has been added at the boundary level. Select one or more edges to be part of the rigid region.

Point Selection

This section is always present.

•

When the is added at the point level, select a number of points that form the rigid region.

•

When the is added at the edge (2D: boundary) level, 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 is selected by default. The 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 subnode.


	In order to be applicable, a coordinate system must have axis directions that are independent of the location in space.

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 — , , or .

•

For the center of rotation is at the geometrical center of the selected points. The constraints are applied at the center of rotation.

•

For a subnode for selection of the points is added to the Model Builder.

•

For , in the XC table enter coordinates based on space dimension.

•

Once is chosen, a default Center of Rotation: Point subnode is added.

•

The center of rotation is located at the centroid of the selected points, which do not need to be related to the objects to which the rigid connector is attached. The points do not even have to belong to the physics interface. As a special case, you can select a single point, and thus locate the center of rotation at a certain point.

Select the checkbox 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 checkboxes then enter values or expressions for the prescribed displacements. The direction coordinate names can vary depending on the selected coordinate system.

•

u0x

•

u0y

•

For 3D components: u0z

Prescribed Rotation

Specify the rotation at the center of rotation. Select from the list: (the default), , or .


	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 select one or more of the available checkboxes to enforce zero rotation about the corresponding axis in the selected coordinate system:

•

Prescribed Rotation

•

For enter an ϕ0. For 3D components also enter an Ω for the , , and coordinates.

•

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

•

Harmonic Perturbation

•

Load Cases

Released Degrees of Freedom

In some cases it can be useful to not constrain the displacement in a certain direction. To do so, select a local for specifying the directions in which the degree of freedom will be released. The list contains only applicable coordinate systems in the model.

Select one or more of the available checkboxes to release the displacement in the corresponding axis in the selected coordinate system:

•

For 3D components:

•

For 3D components:

•

For 3D components:

•


	Note that the Rigid Connector introduces its own global displacement degrees of freedom (DOFs) and global rotation DOFs. When certain displacement field components are released, this reduces the number of equations used to solve for the rigid connector's global DOFs, while preserving the number of said DOFs. Therefore, it may become necessary to constrain some of the Rigid Connector's global DOFs to achieve static determinacy.

The section is only shown if the checkbox in the section is not enabled.

Reaction Force Settings

Select 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 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 to force all matrix contributions from the rigid connector and its subnodes to be symmetric.


	Using an approximative stiffness matrix will in general require more iterations. However, since the computational cost per iteration will be cut at least by a factor of two if a symmetric matrix can be used, it is usually more efficient to ignore a weak nonsymmetry. In particular, if the rotation of the rigid connector per time step or parameter increment is small, there will in general be no increase in the number of iterations at all if this option is used. When the global stiffness matrix is nonsymmetric for other reasons, then there is nothing to be gained from symmetrizing the contribution from the rigid connector.

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 .

This formulation cannot be combined with the formulation of the rigid connector, which in itself is a special form of weak constraint.

Constraint Settings

On the points where the rigid connector is coupled to a flexible material, all nodes 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 .

Advanced

It is possible to couple rigid connectors to each other. In the list, you can select any rigid connector defined in the Solid Mechanics, Multibody Dynamics, or Shell interfaces as being rigidly connected to the current one.

Select — (default), , or , to choose how to group in the solver sequence the dependent variables added by the feature.


	When coupling rigid connectors to each other, you must be careful not to add conflicting settings. Typically, you should only assign constraints to one of the connectors, and it is recommended to use a common center of rotation. It is, however, possible to deviate from these recommendations and create other meaningful combinations.


	Rigid Connector

Location in User Interface

Context Menus

Ribbon

Physics tab with or selected: