Creo Simulate > Modeling Structure and Thermal Problems > Connections > Rigid Links (FEM mode) > About Rigid Links (FEM Mode)
About Rigid Links (FEM Mode)
A rigid link is a rigid bar element that provides a stiff connection between nodes in your model. The rigid link has two sides, dependent and independent. The independent side governs the movement of a node on the dependent side. Motions on the dependent side are determined by the motion on the independent side. The dependent side has six degrees of freedom that you can control and fix selectively according to specific modeling needs.
Rigid links are useful in performing the following functions:
Connect elements with unmatched DOFs. For example, it is common to connect shell elements, which have rotational degrees of freedom, to solids, which do not. In this case, rigid links can minimize perturbation of the elements' stress and strain at the interface boundary.
Tie together components with disconnected meshes. For both hierarchical and flat meshes, rigid links serve as load paths that transmit loads and displacements through assembly components. For more information about the load paths, see Creating Load Paths for FEM Meshing.
Click Refine Model > Rigid Link to create rigid links in your model. After you create a rigid link, you can edit or delete it by selecting the associated icon on the Model tree and using the right mouse button to select Edit Definition or Delete as appropriate. If you are deleting a rigid link, Creo Simulate asks you for confirmation first.
While creating, editing, or deleting rigid links, keep in mind the following:
Use the rules that govern the way you work with the rigid links.
Control visibility of the rigid link icons by using the Simulation Display button on the Graphics toolbar. Creo Simulate places two icons—one for the link, another for the degrees of freedom—on the model.
Place the rigid links on layers.
Use object action to make any changes to the rigid links.
Creo Simulate supports NASTRAN and ANSYS solvers for rigid link outputs. If you try to choose another solver, Creo Simulate ignores the rigid link.
Rigid links are output to the .nas file depending on the type of rigid link created and the value of the configuration option fem_output_rigid_link_as_rbar. For simple rigid links and advanced rigid links that are defined between a single independent side node and multiple dependent side nodes, the rigid links are output as a single RBE2 card for the NASTRAN solver provided the configuration option fem_output_rigid_link_as_rbar is set to its’ default value of no. However if the configuration option fem_output_rigid_link_as_rbar is set to yes or if the dependent side contains a single node, then rigid links are output as RBAR cards.
Refer to the topic Rigid Links in NASTRAN for more details.
If you try to create constraints on the dependent side of a rigid link Creo Simulate prompts you to either delete the rigid link, suppress the rigid link or abort the creation of the constraint. If the constrained nodes happen to merge with the link’s dependent nodes (due to meshing operations), then output to NASTRAN or ANSYS is aborted. Creo Simulate outputs an error message.
Creo Simulate outputs rigid links as CERIG cards for the ANSYS solver.