Rigid target surfaces are defined in their original configuration, and the motion of the entire surface is then defined by the motion on the pilot node (or the different nodes of the target surface if no pilot node is defined).
You must use a pilot node in any of the following situations to control the boundary conditions (and motion) of the entire target surface:
The target surface is subjected to applied forces.
The target surface is subjected to rotations.
The target surface is connected to other elements (for example, structural mass element MASS21).
The motion of the target surface is adjusted by the equilibrium condition.
When modeling surface-based constraints or a rigid body.
The degrees of freedom of the pilot node represent the motion of the entire rigid surface, including two translational and one rotational degree of freedom in 2D, and three translational and three rotational degrees of freedom in 3D. You can apply boundary conditions (displacement, initial velocity), concentrated loads, rotations, etc. to the pilot node. To account for a rigid body's mass, define a mass element (MASS21) on the pilot node. You can also define a follower element (FOLLW201) on the pilot node. The element-specified external forces and moments will follow the motion of the pilot node.
By default, KEYOPT(2) = 0 for the target element, the program checks the boundary conditions for each target surface. If all of the following conditions are met, then the program treats the target nodes along the respective degree of freedom as fixed:
There are no explicit boundary conditions or prescribed forces for target surface nodes.
Target surface nodes are not connected to other elements.
Neither constraint equations nor node coupling have been used to constrain such nodes.
At the end of each load step, the program releases the constraint conditions that were set internally.
The constraint conditions stored in the results file (Jobname.rst) and the database file (Jobname.db) may be updated due to this change. You should carefully verify whether the current constraint conditions are expected before restarting an analysis or resolving the problem in interactive mode.
If you wish, you can control the constraint conditions of target nodes by setting KEYOPT(2) = 1 in the target element definition.
Assumptions and Restrictions for Target Surfaces that Use a Pilot Node
Each target surface can have only one pilot node.
The pilot node can be one of the nodes on the target elements or a node at any arbitrary location. However, it should not be a node on the contact element. The location of the pilot node becomes important only when rotations or moments are to be applied.
For each pilot node, the program automatically defines an internal node and an internal constraint equation. The rotational DOF of the pilot node is connected to the translational DOF of the internal node by the internal constraint equation. The internal constraint equations do not take stress stiffening effects into account.
Generally, you should not apply external constraint equations (CE) or node coupling (CP) to the pilot node.
The program ignores all boundary conditions on all nodes other than the pilot node when KEYOPT(2) = 0 (default) for the target elements.
When KEYOPT(2) = 0 (default), only the pilot node can connect to other elements.
By setting KEYOPT(2) = 1 for the target elements, you can apply boundary conditions on any rigid target nodes rather than only on the pilot node. In this case, it is your responsibility to make sure the rigid target surface is not under-constrained or over-constrained. It is still recommended that you apply all boundary conditions on the pilot node, even when KEYOPT(2) = 1.
Note: For flexible-to-flexible contact, no special boundary conditions treatment is performed, and KEYOPT(2) = 0 should be used.